Re: [PEDA] More SPs for older major versions?
Just for info, take a look at: http://www.bookshop.unimelb.edu.au/x/n?888397230 -Harry At 10:23 AM 1/28/2008, Jon Elson wrote: A sad consequence of all this is that Altium actually lose sales and the community bcomes more closed as a result of cracked versions in circulation. A university lecturer friend tells me that ALL the students in his classes have got hold of (and sometimes use!) cracked versions of Protel and DXP. Well, while it isn't legal, Altium has laughably little chance to sell a university student a $10 grand software package. So, it really is NOT cutting into their revenue. Now, if those students go off into industry and keep using it, that's another matter, but many large companies, at least, are on the lookout for that sort of thing. The original Tango license allowed you to use a home copy of the software, and I used it that way. When I moved over to Protel, I eventually needed to have it at home, and found a way to buy an old Protel for Windows license on the open market and upgrade it to P99SE. So, at least, I'm legal. Jon You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Schematic - Dashed Lines.
Hi Brad, This is an old issue that is well known. It's not really a bug, but a result of how the dotted and dashed lines were produced. In Protel99SE graphical lines were drawn using the Windows Graphics Device Interface (GDI), and the Windows GDI does not support the width property. The bug was allowing a menu choice that didn't work. You can manually create dashed lines of any width by drawing a short solid line with the desired width, then use copy and paste, or paste it multiple times using Paste Array. Regards - Harry At 11:43 AM 1/7/2008, you wrote: The schematic line tool displays dashed (and dotted) lines with the line width of smallest no matter what it is set to. If you change the line back to solid then the line width gets set to the correct value. Is this a known bug? Protel99SE SP6. Tx Brad. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] DXP PCB - 99SE
Hi Rob, The sequence of Protel products is Autotrax Tango Protel 2.x Protel 3.x Protel98 Protel99 Protel99SE DXP DXP2004 Altium Designer 6.x. The PCB file versions are Protel 2 (Version 2.x), Protel 3-Protel98(Version 3), Protel99-99SE(Version 4), DXP-Altium Desiger 6.2(Version 5), Altium Designer 6.3-6.x(Version 6). The latest version of Altium Designer can save files in earlier formats by stripping out features that were added after the target format. However, there is a bug that hasn't yet been fixed. DXP introduced a primitive called a region - it is a type of polygon. The file converter in Altium Designer does not properly strip out that primitive. The result is that files using that primitive will cause a crash in earlier versions when the down-converted file is loaded. The workaround is to manually strip out regions before saving in an earlier format. Regards - Harry At 02:23 PM 9/10/2007, you wrote: I thought P99SE was just P98SE with a few patches, you are saying that they are different beasts and that DXP is closer to 98 than it is to 99. Our DXP, I think, is something like 6.3. The about menu tells me it is DXP2004. I'll have to check with the systems guy to be sure. Thanks again, Rob -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Jeff Condit Sent: 10 September 2007 21:57 To: Protel EDA Discussion List Subject: Re: [PEDA] DXP PCB - 99SE Bob, I have Altium Designer 6.7 up and running. In a pinch I could try loading your DXP design into AD6.7 and than save it as file version 4. However, I haven't done this a lot and so cannot vouch that everything would make it through intact. You'd still have to look it over in P99SE. I think it would be better if you could go directly from DXP to P98SE as they are much more closely related. - Original Message - From: Steve Smith [EMAIL PROTECTED] To: Jeff Condit [EMAIL PROTECTED]; Protel EDA Discussion List peda@techservinc.com Sent: Monday, September 10, 2007 9:43 AM Subject: RE: [PEDA] DXP PCB - 99SE Good luck with that. The primary reason we upgraded to DXP from 99SE was that we had an outside source do a design for us in DXP and when we brought them back into 99SE we had major problems with the file being readable by 99SE. It literally took many multiple attempts to open the file in 99SE, if it would open at all. Regards, Steve Smith Product Engineer Staco Energy Products Co. Web Site: www.stacoenergy.com www.stacopower.com DISCLAIMER AND/OR CONFIDENTIALITY NOTICE: This message, including any attached materials, is intended solely for the use of the individual or entity to whom it is addressed and may contain information that is privileged, confidential, and exempt from disclosure under applicable law. If the reader of this electronic mail transmission is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you have received this communication in error, please e-mail or call Staco Energy Products Co. at (937) 253-1191. Thank you for your cooperation. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Jeff Condit Sent: Monday, September 10, 2007 11:11 AM To: [EMAIL PROTECTED]; Protel EDA Discussion List Subject: Re: [PEDA] DXP PCB - 99SE Robert, I don't have DXP up right now but believe P99SE files are version 4. Can you try doing a Save-As to version 4? - Original Message - From: Robert Gillatt [EMAIL PROTECTED] To: 'Protel EDA Discussion List' peda@techservinc.com Sent: Monday, September 10, 2007 7:40 AM Subject: [PEDA] DXP PCB - 99SE Hi, Does anyone know if I can save DXP .pcbdoc files in a format that 99SE will recognize. I know, I am a lazy man, but it might save me trying out all the variations on the Save As menu. Thanks Rob R`theta Electronics mailto:[EMAIL PROTECTED] -- No virus found in this incoming message. Checked by AVG. Version: 7.5.485 / Virus Database: 269.13.13/998 - Release Date: 9/10/2007 8:48 AM You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL
Re: [PEDA] Show Holes in gerbers
Hi Alfonso, You can't make the PCB Editor in AD output Gerber files with holes showing. All of the thru-hole pads will be solid (AD doesn't have the ability to specify donut pads). What folks have done in the past to get what you are after, is hand edit in CAMTASTIC. You can change the D-Code shape for the desired pads from round to donut and enter the desired hole size. Be aware that tracks terminating in the center of donut pads will at least partially overlay any hole you introduce using this method - if that's a problem, you need to do more hand editing by pulling the track ends back a bit. Once the editing is done in CAMTASTIC, you can print and/or save the modified Gerbers. With regard to your printer output accuracy, I've had better luck on 1:1 prints produced on a plotter. For that reason, I suspect the registration and accuracy are related to how the printer drivers handle the data, and not to anything inherent in AD. Regards - Harry At 08:42 AM 7/17/2007, you wrote: -Original Message- From: Alfonso Baz [mailto:[EMAIL PROTECTED] Sent: Tuesday, July 17, 2007 12:43 AM To: PEDA@techservinc.com Subject: [PEDA] Show Holes in gerbers Hi all I'm currently working for customers who have AD and they prototype small boards in house. The problem I'm having is that the print output, (File-Fabrication Outputs-Final), are not very accurate (regardless of printer type selected) The tracks entering a fine pitch component print slightly off centre (they preview this way also). When I produce gerber files and print those the output comes out right. Unfortunately I can't seem to find a way of producing gerber files with pad holes showing for through hole components. Is there a way of accomplishing this? Cheers You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] BOM generation in DXP
Hi Carlos, Don't use Simple BOM. Use either OUTJOB, or ReportsBill of Materials. From the BOM dialog, drag the common feature (such as description, library reference, or footprint) from the bottom left column of the dialog to the top left column (heading is Grouped Columns). Now your BOM will show the designators and totals grouped according to the feature they have in common. Regards - Harry At 02:20 PM 7/9/2007, you wrote: Hello all, I have a question regarding the bom creation from schematics. I was wondering if anybody could explain to me how I can generate a BOM from schematics that will show the same parts in one row with with the total number of same components and all designators where that part is used in the quantity column and in the designator column. Right now, I get all quantities as 1 and a repeat of those same parts in different rows with different designators. Thanks for your help, Best Regards, Carlos A. Claveria, P.Eng. Net Safety Monitoring Inc. 2721 Hopewell Place N.E. Calgary, Alberta, Canada T1Y 7J7 Tel : (403) 219-0688, Ext: 6083 Direct: (403) 769-6083 Fax : (403) 219-0694 e-mail: [EMAIL PROTECTED] website: http://www.net-safety.com snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] QFN Package
Hi Brad, Your approach to constructing the footprint is the same as I have used many times. Sometimes the primitives used within a footprint don't pick up the net if the component is placed or updated after the netlist has been loaded - the behavior differs depending on what version of the software you are using. Since you didn't mention what version of Protel/Altium software you are using, so you may have to hunt for the menu item. Try running 'DesignNetlistUpdate Free Primitives from Connected Copper'. Verify that the fill and tracks used in the footprint have picked up the net name, and try re pouring the polygon. Be sure that the polygon option is set to pour over same net. Also be aware that Protel/Altium footprint editor doesn't automatically generate mask layers for fills (only pads). Be careful that you manually build the desired solder mask and paste mask for the fill area on your footprint, or you'll end up with no paste mask, and the thermal pad covered in solder mask. Regards - Harry At 01:30 PM 5/3/2007, you wrote: Hi. I have a QFN-10 footprint that I am creating. The data sheet shows a solder pad under the device (fill), 5 vias and 4 tracks all used for heat sinking. I placed a copper fill on the PCB component and placed 5 pads and tracks as shown in the data sheet. The 5 pads have designators that refer to 5 pins in the schematic component. The 5 pins all connect to GND. When I place the PCB part and pour a polygon GND it does not pick up on the fact that the fill, 5 pads and tracks are to be connected to GND. Is this the correct approach? http://focus.ti.com/lit/ds/symlink/tps63000.pdf Brad. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Open source equivalent to Protel
There is really only one open source complete EDA suite for Linux at the moment. It is gEDA, and you'll find it at http://geda.seul.org . -Harry At 09:59 AM 4/24/2007, you wrote: I am a very happy Protel 99SE user but my boss is infatuated with open source and he is asking about open source PCB schematic and layout programs. Personally I see no reason to switch from Protel 99SE or DXP but he wants us all to switch over to Linux sometime in the future. Do any of you have any suggestions for programs equivalent to Protel in the Open Source realm. I have looked at several on the web but I have not tested them out yet. Trentino snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Open source equivalent to Protel
I have not done any serious design work with it. Out of curiosity, I tinkered with it by doing a simple two-sided hobby board. I had to do a bit of source compiling to get it set up. It's the usual Unix collection of tools to do the job - it's not tightly integrated as you expect from commercial EDA software. Unless they've done something with it recently, it's limited to an 8 layer PCB. If you're looking for a free open source professional package to run under Linux - it doesn't exist. At 11:35 AM 4/24/2007, you wrote: Have you used this at all? From: Harry Selfridge [EMAIL PROTECTED] Date: 2007/04/24 Tue PM 01:00:44 CDT To: Protel EDA Discussion List peda@techservinc.com Subject: Re: [PEDA] Open source equivalent to Protel There is really only one open source complete EDA suite for Linux at the moment. It is gEDA, and you'll find it at http://geda.seul.org . -Harry At 09:59 AM 4/24/2007, you wrote: I am a very happy Protel 99SE user but my boss is infatuated with open source and he is asking about open source PCB schematic and layout programs. Personally I see no reason to switch from Protel 99SE or DXP but he wants us all to switch over to Linux sometime in the future. Do any of you have any suggestions for programs equivalent to Protel in the Open Source realm. I have looked at several on the web but I have not tested them out yet. Trentino snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com Dave Schaefer [EMAIL PROTECTED] You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Open source equivalent to Protel
Hi Jon, As a person who has only dabbled in Linux for fun, I'm hardly the one to give a definitive review of gEDA. My impression of gEDA was that it wasn't for high tempo professional work. Everything is done from mostly command line stand-alone programs - like a lot of Unix software. The PCB program is 8 copper layers, not total layers. As I recall, there aren't any mechanical layers upon which to do any of the dimensioning or commenting you might want. Obviously, you can't crossprobe, or do anything that depends on functional integration. Nothing you have done under Protel is usable in gEDA - it speaks a language all its own. Likewise, nothing you do in gEDA is portable to any commercial EDA package (as far as I know). Maintainability is at the mercy of the gEDA developers. It's up to you to compile the code if you're not running a Fedora or Redhat version for which it has already been compiled. There are some reviews online that might give you more insight than I can. Try: http://www.linuxjournal.com/article/8438 and http://linuxfocus.org/English/December2004/article355.shtml . Regards - Harry At 12:06 PM 4/24/2007, you wrote: Harry Selfridge wrote: I have not done any serious design work with it. Out of curiosity, I tinkered with it by doing a simple two-sided hobby board. I had to do a bit of source compiling to get it set up. It's the usual Unix collection of tools to do the job - it's not tightly integrated as you expect from commercial EDA software. Unless they've done something with it recently, it's limited to an 8 layer PCB. Could you compare it in ease of use, flexibility, ability to set up libraries, etc. to P99SE? 8 copper layers (signals plus planes) would not likely be much of a restriction. 8 total layers, including silk screen, solder mask, paste mask, mech etc. would already be a limitation. If you're looking for a free open source professional package to run under Linux - it doesn't exist. I'm less concerned about free as with maintainability. Some day my P99 CD's won't be readable any more, and I'll be in big trouble. I paid a fortune for P99SE, and I'm damned if I'll pay another fortune for Altium's latest boondoggle. Jon snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Power Port Library
Hi Dan, It's been a while since I used 99SE, but as I recall the port symbols are hard coded - you can't modify or add to them. Making your own library is the only solution, as far as I know. Regards - Harry At 11:45 AM 1/22/2007, you wrote: Hello All, I know I probably took the easy way out last time and created my own library component, but I was wondering if anyone can tell me how to modify/create parts in the power port library that shows up in the wiring tools toolbar. Thanks, Dan Enslen Enginering Technician Precision Analog Functions - HPL Texas Instruments - Tucson Voice: 520.746.7324 FAX: (520) 746-7467 [EMAIL PROTECTED] snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] How to import sch from Mentor into P99SE
Hi Leo, I assume you mean Mentor PADS PowerLogic schematic capture (Mentor sells other packages too). Unfortunately, none of the Mentor schematic capture formats can be translated into Protel format without the use of a third party conversion program. You can search the Internet for a company that has the necessary tools, or you can simply redraw the schematic. I did a quick Google search, and I found several companies that claim to be able to do schematic translations. I haven't used any of them, but one that says they can go from PADS to Protel is http://www.edaxchange.com/ . Another route would be to translate the PowerLogic schematic to Orcad, then import the Orcad schematic. Again, a Google search turns up Elgris Technologies, Inc who claims to provide PADS Powerlogic-OrCAD translator in the tool E-studio Pro. Neither of the above appears to be cheap. The first tool is listed at about $1800 USD, the second doesn't list a price on the Internet (possibly a bad sign regarding cost). Regards - Harry At 09:09 AM 1/4/2007, you wrote: Hi folks, I need to combine two of our products into one PCB. Nothing special, you might think. But one of the products is designed in Mentor Graphics:-( And as chance would have it (after all, coincidence does not exist) that is the bigger thingy. Our Mentor engineer has more than enough things to do already so I am the one left with the task of doing it all in Protel Mentor can import, but not export Protel files. Has anyone heard, seen or even know of a way to accomplish this (short of re-drawing the thing)? Just the schematic would do... Leo Potjewijd hardware designer Integrated Engineering Paasheuvelweg 20 NL-1105 BJ Amsterdam Zuidoost The Netherlands T: +31 20 4620755 F: +31 20 4620756 E: [EMAIL PROTECTED] I: www.smart-ID.com snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 500V power supply
Hi Dan, Attachments aren't allowed on posts to this forum - they get filtered out. You would have to post a link to a file, or send it offline to whomever you wished to receive it. IPC-D-275 has been superceded by IPC-2221A. Section 6.3 of IPC-2221A, Generic Standard on Printed Board Design, has the voltage clearance calculations for various configurations of rigid circuit boards. -Harry At 12:40 PM 12/13/2006, you wrote: OK, I guess I didn't really include the attachment. If anyone is interested in enlightening me on the correct procedure for sending attachments, I would be happy to try again. Dan Enslen The only reason time exists is so everything doesn't happen all at once. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Dan Enslen Sent: Wednesday, December 13, 2006 12:57 PM To: 'Protel EDA Discussion List' Subject: Re: [PEDA] 500V power supply Carlos, I've included an attachment here for your benefit. Yes, it is out of the IPC-D-275 spec. I would agree with Mr. Jenkins on consulting with your engineer given the your requirement of space constraint Dan Enslen The only reason time exists is so everything doesn't happen all at once. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of [EMAIL PROTECTED] Sent: Wednesday, December 13, 2006 11:01 AM To: PEDA@techservinc.com Subject: [PEDA] 500V power supply Hello all, I need to design a pcb for a power supply set to 500V and 1ma current output. I was wondering if there's anybody with experience that could give me an idea as to what gap between components is recommended and what minimum distance between tracks I should use. I am working in a very limited space and I need optimal area use. The supply consists of a boost controller and a series of diode/cap multiplier stages to bring the voltage to the required value. Thanks for your help, Carlos snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 500V power supply
Hi Dan, The Yahoo Protel User's Group file library is at: http://groups.yahoo.com/group/protel-users/files/ . You have to login to Yahoo, and you have to be accepted into the group by the moderator to post. I sent some reference material on conductor clearance standards to Carlos offline. Harry At 01:46 PM 12/13/2006, you wrote: Thanks Harry, I sort of remember that now. Wasn't there an alternate location (yahoo group of some sort) that allowed for doing such things. I know I've seen posts that mention board example pictures. Regarding the older standard, I had copied that from one of our former layout people before all of that was outsourced. I doubt I could get them to spring for a copy of the new standard for those of us here who are doing prototyping. Oh well. Dan Enslen The only reason time exists is so everything doesn't happen all at once. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Harry Selfridge Sent: Wednesday, December 13, 2006 2:18 PM To: Protel EDA Discussion List Subject: Re: [PEDA] 500V power supply Hi Dan, Attachments aren't allowed on posts to this forum - they get filtered out. You would have to post a link to a file, or send it offline to whomever you wished to receive it. IPC-D-275 has been superceded by IPC-2221A. Section 6.3 of IPC-2221A, Generic Standard on Printed Board Design, has the voltage clearance calculations for various configurations of rigid circuit boards. -Harry At 12:40 PM 12/13/2006, you wrote: OK, I guess I didn't really include the attachment. If anyone is interested in enlightening me on the correct procedure for sending attachments, I would be happy to try again. Dan Enslen The only reason time exists is so everything doesn't happen all at once. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Dan Enslen Sent: Wednesday, December 13, 2006 12:57 PM To: 'Protel EDA Discussion List' Subject: Re: [PEDA] 500V power supply Carlos, I've included an attachment here for your benefit. Yes, it is out of the IPC-D-275 spec. I would agree with Mr. Jenkins on consulting with your engineer given the your requirement of space constraint Dan Enslen The only reason time exists is so everything doesn't happen all at once. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of [EMAIL PROTECTED] Sent: Wednesday, December 13, 2006 11:01 AM To: PEDA@techservinc.com Subject: [PEDA] 500V power supply Hello all, I need to design a pcb for a power supply set to 500V and 1ma current output. I was wondering if there's anybody with experience that could give me an idea as to what gap between components is recommended and what minimum distance between tracks I should use. I am working in a very limited space and I need optimal area use. The supply consists of a boost controller and a series of diode/cap multiplier stages to bring the voltage to the required value. Thanks for your help, Carlos snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] SUSPECT: Re: Octagonal Pads
If you mean am I tired of the whining about old problems that have been fixed - yup. I see lots of empty words here. It used to be a forum for helping one another get the most out of Protel/Altium Designer. Now it seems to be a marathon bitch session. I haven't seen much constructive discussion in months. -Harry At 11:37 AM 11/28/2006, you wrote: Ooh, struck a nerve, aye Harry? -Original Message- snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] importing stock number into sch librairy
The answer to your question, Would DXP do it better?, is absolutely yes. Altium Designer 6, which is the latest version of DXP, has a feature called database lilbraries. It would seem to be a perfect fit for what you want to do. You can read about the capability in one of the support documents for Altium Designer that is available online at: http://www.altium.com/files/AltiumDesigner6/LearningGuides/AP0133%20Using%20Components%20Directly%20from%20Your%20Company%20Database.PDF There's nothing like that capability in the older Protel99SE. You should be aware that upgrading will involve a fairly steep learning curve - much has changed, and there are MANY new features in the latest version of the software. Regards - Harry At 10:47 AM 11/16/2006, you wrote: Hello, I would like to know if there is an easy way to import my stock list numbers into my schematic librairies so that I can generate a good and accurate parts list. We are using DBA to manage our stock and we are looking for a good way to integrate our stock number to protel. I do not really want to do this manually. I am using protel 99SE. Would DXP do it better??? Thanks Yves Dubois Raytron LTD Montreal Quebec You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] SUSPECT: Re: importing stock number into sch librairy
No - Altium doesn't sell older versions to end users. At 01:37 PM 11/16/2006, you wrote: Can one legally purchase DXP from Altium (the version that the query referred to)? -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Harry Selfridge Sent: Thursday, November 16, 2006 4:28 PM To: Protel EDA Discussion List Subject: SUSPECT: Re: [PEDA] importing stock number into sch librairy The answer to your question, Would DXP do it better?, is absolutely yes. Altium Designer 6, which is the latest version of DXP, has a feature called database lilbraries. It would seem to be a perfect fit for what you want to do. You can read about the capability in one of the support documents for Altium Designer that is available online at: http://www.altium.com/files/AltiumDesigner6/LearningGuides/AP01 33%20Using%20Components%20Directly%20from%20Your%20Company%20Da tabase.PDF There's nothing like that capability in the older Protel99SE. You should be aware that upgrading will involve a fairly steep learning curve - much has changed, and there are MANY new features in the latest version of the software. Regards - Harry At 10:47 AM 11/16/2006, you wrote: Hello, I would like to know if there is an easy way to import my stock list numbers into my schematic librairies so that I can generate a good and accurate parts list. We are using DBA to manage our stock and we are looking for a good way to integrate our stock number to protel. I do not really want to do this manually. I am using protel 99SE. Would DXP do it better??? Thanks Yves Dubois Raytron LTD Montreal Quebec You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] importing stock number into sch librairy
You are absolutely right, Alfonzo. It's been so long since I've used 99SE that I had forgotten. Page 159 of the manual at: http://www.altium.com/files/protel/legacy/handbookp99se.pdf shows how to link schematic libraries to an external database. Regards - Harry At 02:03 PM 11/16/2006, you wrote: There's a whole section in the 99SE handbook on how to link components to an external database -Original Message- ... Hello, I would like to know if there is an easy way to import my stock list numbers into my schematic librairies so that I can generate a good and accurate parts list. We are using DBA to manage our stock and we are looking for a good way to integrate our stock number to protel. I do not really want to do this manually. I am using protel 99SE. Would DXP do it better??? Thanks Yves Dubois Raytron LTD Montreal Quebec You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Pre-routing In 99SE
Hi Bob, I doubt that your component footprint is what is causing the problem. As I recall, the most common reason for the failed to initialize complaint from the 99SE router was a missing or incomplete bounding outline on the keepout layer. There are some suggestions/hints in the knowledge base article: http://www.altium.com/forms/kb/kb_item.asp?ID=1694 Regards - Harry At 11:40 AM 11/10/2006, you wrote: Hi Again, As you can tell I am just getting into 99SE. Believe it or not PCB 2.8 had done all I needed for quite a while. I now have a board with some components at 45 degrees and 2.8 falls apart there. Anyway, I am probably doing this wrong but it has worked for all this time in 2.8. I defined a heat-sink with some fills and no pads. When I would pre-route in 2.8 it would change these fills to what ever might be connected to them, like the tab on a D2PAK. I tried to turn off all the auto-routing in 99SE to get a pre-route but it does not work. It goes through the locked traces and then says it cannot initialize which really does not tell me anything. I am not even sure if 99SE will act the same way as 2.8 did. I may have to re-do the way I define my heat-sink. This is a surface mount heat-sink that has a contact area like a U (Aavid 7109D). The only way I can figure to do this is will 3 fills. As you can tell I am way behind the curve here and would appreciate any suggestions. Thanks, -Bob Robert Ritchey Quest Engineering Development 1328 East Cottonwood Lane Phoenix, AZ 85048-4765 Tel: (480) 460-2652 FAX: (480) 460-2653 E-Mail: [EMAIL PROTECTED] E-Mail: [EMAIL PROTECTED] E-Mail: [EMAIL PROTECTED] E-Mail: [EMAIL PROTECTED] WWW: www.QuestEngDev.com/ WWW: www.Smart-Fly.com/ You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] HIGH LIGHTING CONNECTIONS
Hi Yves, Yes, that is the way Select Connected Copper works. It only selects connected copper on signal layers. It cannot select connections made through a plane. Regards, Harry Selfridge VP Engineering Encore Engineering Services and Products Temecula, California At 10:32 AM 10/4/2006, you wrote: Hi there, I am making right now a 4 layer PCB. I have various split planes (-1V,+30V, +6.2 ect). Our verification process states that we verifythe board trace by trace the layout even if we are using netlists. I am using theSelect Connected Copper function to highlight my connections. I have let's say 10 components connected to a plane and you highlight one track that is connected to that plane why is all the other tracks that are connected to that plane are not highlighted as well. As far as I know it is connected copper. I must assume that it is the way Protel made it. Thanks Yves Dubois Senior PCB designer Raytron ltd Monteal, QC, Canada SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Protel or Altium to PADS conversions
Mentor has free Protel to PADS translator software. http://www.mentor.com/products/pcb/pads/translators.cfm At 10:33 AM 9/13/2006, you wrote: Does anyone know of a way to output a useable ASCII design file to PADS from 99SE or Altium A6? Or maybe a third party conversion package. Mike SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Here is the Snake Oil, straight from the snake's mouth.
Brad, I wouldn't question Ton's claim; however, if you do a forum search using ODB++, you will find a different user's posting in October 2005 claiming that he uses AD2004 ODB++ output exclusively to get 'perfect' boards from his fab. With regard to missing vias, I found only Ton's recent post in the past couple of weeks (which seems to be related to using a new feature added in AD6 before generating ODB++ output). Based on forum postings, others among the thousands of users don't seem to be having Ton's problem. I believe that ODB++ as an example of serious AD6 shortcoming was a poor choice. I could go on to discuss the lack of standardization of ODB++ thanks to Valor. Their free reader won't read an ODB++ file generated by Gerbtool or CAM350 half of the time (and vice-versa). It is a poorly supported standard in the industry that has to be used with extreme caution. Trying to achieve compatibility with Valor's proprietary format-turned-standard is just like trying to get compatibility with Autodesk's proprietary .DWG formats - lots of folks try, but things don't always work (see www.opendesign.com ). Personally, I would never depend on ODB++ to transmit fab data - first: because when it works it contains all of the design intelligence, and second: because of the shaky support for the file format thanks to Valor's closed fist on the file structure. Significant AD6 bugs in my world would be those that prevent, or slow, my production of useful hardware (the purpose of the software). I haven't seen any of those recently. There are glitches and omissions in the software that would make it nicer to use, but they aren't 'show stoppers'. Grump and complain as much as you like, I'll just keep cranking out paying designs using AD6. Altium has earned the dollars I have spent with them over the years, and THAT is the bottom line for me. For me, Altium/Protel software and support has just gotten better over the years. It's still the best cost-to-value EDA package out there as far as I'm concerned. Sincerely, H. Selfridge VP Engineering Encore Engineering Services and Products Anaheim, CA 92801 At 09:05 AM 3/20/06, you wrote: Harry, I failed to type upgrade support, implying the typically included first year Software Assurance. As for the bugs and your comments. I don't believe that perfect, bugless, software is a reality but there are just too many significant bugs in Altium's releases. I figured the internal pads missing from ODB++ output is just the best example of that which I have seen recently. Your comments also show why BETA testing is not a suitable means to catch bugs, nothing says that any particular BETA test or BETA tester will actual try or use any particular feature, that is for ALPHA testing to confirm for all product features. No if, ands or buts about it. Then of course there is Ton's claim that he had reported it Altium well prior to AD6.0. So is it a feature (ODB++ support) or is it a boondoggle money grab? In my books, if you sell a feature then it had better be usable by the majority of typical users. Missing internal pads don't pass that case. Sincerely, Brad Velander Senior PCB Designer Northern Airborne Technology #14 - 1925 Kirschner Road, Kelowna, BC, V1Y 4N7. tel (250) 763-2329 ext. 225 fax (250) 762-3374 -Original Message- From: Harry Selfridge [mailto:[EMAIL PROTECTED] Sent: Friday, March 17, 2006 8:26 PM To: Protel EDA Discussion List Subject: Re: [PEDA] Here is the Snake Oil, straight from the snake's mouth. How did you conclude that the software is being sold without support? You don't need Software Assurance to post on the forum and get help straight from the Altium programmers, and you don't need it to get the patches which are automatic via the web (or can also be manually downloaded and installed if desired). The CEO of the company has personally gone on written record that patches would continue to be provided as part of the purchase price of the program, and would not be subject to separate charges. You don't have to buy Software Assurance unless you want it - I didn't choose to buy it when I sent in my purchase order for AD6 in December 2005. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old
Re: [PEDA] Here is the Snake Oil, straight from the snake's mouth.
How did you conclude that the software is being sold without support? You don't need Software Assurance to post on the forum and get help straight from the Altium programmers, and you don't need it to get the patches which are automatic via the web (or can also be manually downloaded and installed if desired). The CEO of the company has personally gone on written record that patches would continue to be provided as part of the purchase price of the program, and would not be subject to separate charges. You don't have to buy Software Assurance unless you want it - I didn't choose to buy it when I sent in my purchase order for AD6 in December 2005. Software Assurance gets you telephone support, and guarantees you will get the next major upgrade without having to buy it at whatever the prevailing price may be at the time. This is the same as other EDA packages at a significantly lower price than some (ask a Cadence rep for the annual maintenance cost on Allegro and ConceptHDL). It is also worth noting that you MUST buy maintenance on the other big EDA packages to keep your license current - Altium can be used for the rest of your life without buying a maintenance program. With regard to the bugs, did it occur to you that the software has been in the hands of thousands of users for about 3 months? Before that, it was in the hands of Beta Testers for over two months. In that five months NOBODY noticed or reported that ODB++ output was missing vias on inner layers. How important could that feature be to users if it went 5 months without being noticed and reported - or perhaps the bug is specific to an odd hardware/software environment that has only recently surfaced? There are a multitude of similar bugs being reported - important to a few, or only experienced by a few, but not significant or noticed by the bulk of users. I can personally assure you that the other EDA companies DO NOT rush patches out to the users. Just read the Outstanding Issues document included with Mentor or Cadence updates, and compare them with those from a year ago (or three years ago). You might also want to try and fight your way through the phone tree at their companies to get an answer on a problem - it's like trying to call the Internal Revenue Service (for those in the USA). I fault Altium for not publishing a price schedule, but I believe I understand their problem/rational. There are now many 'flavors' of AD - node locked license, floating license, network license, core, fpga, etc. The software is more tightly controlled in regions of the world that have traditionally stolen Protel/AD software in large numbers in the past - hence the higher price and availability of only node locked licenses in those regions. Prices vary according to exchange rates, market demand, etc. There are lots of market driven variables for the company manipulate to try and squeeze out a profit (something we all have to do to stay in business). The impending price increase was announced at the end of November 2005. It is hardly a surprise - unless you consider it a surprise that they waited until now to do what they said they would do at the beginning of the year. I asked for, and received a written quote from the San Diego, California, Altium office in December. It clearly stated that the maintenance cost was a separate line entry, and it clearly stated that prices would increase after the first of the year. I've been producing 18-20 layer, 12-14in, 2K-4K pin, high speed boards with AD6 since December. There are occasional problems with the software, but the new update procedure is smoothing out the bumps. The ones that can be bypassed while we wait for patches have been addressed by the Altium staff on the forum. In my opinion, AD has become much more productive than earlier versions, and can be customized to a degree impossible to match with other EDA software. It is 'hands down' the best EDA package on the market for interactive manual routing - it retains, and improves on, the interactive routing capabilities of earlier Protel/Altium packages. I realize that you folks who want to be angry are going to seize on everything you can find to justify you anger. I use Cadence, Mentor, and Altium products - and have for many years. Of those, I prefer Altium for its support and simplicity. I don't have to fight Altium software to do my designs, and I can get answers from Altium staff just by posting a message on the forum. I dread the days when I have to return to using Allegro or PADS. They just aren't as much fun to use. Harry Selfridge VP Engineering Encore Engineering Services and Products Anaheim, CA 92801 At 05:19 PM 3/17/2006, you wrote: Well guys, There is some truth to the stories that have been slowly spreading amongst us. Below is a cut paste from the Email that I just received this afternoon. You will note that on 4/1/06 the price
Re: [PEDA] 6.0 ? it is here
Hamid, If you were alert during the holiday period, you would have noticed a couple of automated out of office replies to postings on this forum from one of those non-existent Altium monitors. He apparently forgot to turn it off when he went on holiday. In case you missed it - this forum is hosted by one of your competitors (TechServInc - http://www.techservinc.com ). It is NOT an independent host, and it is NOT affiliated directly with Altium. Perhaps that explains the less than overwhelming presence of Altium factory tech support here, and the reason that Altium contact concerning problems discussed here is most frequently dealt with off-line. If you have a legally registered copy of any Altium product, there shouldn't be any reason not to register on the Altium site for their OFFICIALLY supported forum. That is where you would find a very active representation of both knowledgeable users, and Altium technical staff. Several years ago, this was one of onlly two forums where Protel / Altium topics were exchanged. After Altium created their own forum, this forum and the other faded into insignificance. A few of us continue to monitor here, and help when we can; however, the real action is on the official Altium forums. If you are unhappy with Altium products, and Altium support practices, I would be willing to post the contact information for other products you could buy and try - I have all of the significant EDA contacts in my Rolodex. They too have company supported forums for registered users. You also might find one of those forums more receptive to the constant whining and negativity that seems to be common here in recent months. Harry Selfridge VP Engineering Encore Engineering Services and Products Anaheim, California At 08:44 AM 1/18/06, you wrote: Brad Velander wrote: Altium has always unofficially monitored this forum, although they typically have not posted to the forum. At least one long term member vehemently asserted in the very recent past Altium does NOT monitor this forum. I am sure he will have a different interpretation that yours and mine -- coincidence, cosmic alignment, hallucination from the medications (she never got a call) Hamid SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] AD6 component disappears while moving -fixed but VErY slow
You lose the transparent appearance in the graphics without alpha blending. Some of the new features just won't look the same - such as the heads up display. Some machines won't do alpha blending in 16bit mode - some do. I believe it is a function of the graphics chip and drivers. The speed issue is also a result of all the added graphics processing. I have a dual head Matrox Parahelia with DVI LCD monitors and AD6 seems to work well, but I also have 2Gb of RAM to help speed things up. Rumor has it overall speed will improve with the next update - we'll just have to see. In the meantime, the speed isn't an issue as long as you keep to Altium's recommended minimum system - http://www.altium.com/Products/AltiumDesigner/Systemrequirements/ -Harry At 02:31 PM 1/16/2006, you wrote: thanks darren harry ! i went to another box, no issue with moving went back to first machine turned off alpha blending and that did do the trick (fixed problem) so the question is, what if anything will be lost by not using alpha blending? turned alpha blend back on and changed color depth to 32 bit, retstarted AD and that also worked but moving the component was so slow as to be useless card is G450 2 head BTW, the G450 allows 16/24/32 bit depth on screen 1 but only 16/32 on screen 2, or maybe that has to do with the monitor types ?, 1 CRT, 1 LCD, both 21's another note the program sure is poky and jerky while moving the component and my first practice board only has 4 components! it feels like some huge grid, but the snap grid is at 25mils the box w/ the G450 is not too old, 2Ghz, and it does have 512K ram (it had 1G ram but we pulled out one stick about 1 year ago which solved a lot of crashing issues, interestingly replacing the second stick didn't help that either, maybe that is a mobo issue) ds ___ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com Harry Selfridge wrote: AD6 uses Alpha Blending for graphics transparency. One possible source of your problem could be that your graphics card can't process Alpha Blending. Try turning it off in PreferencesPCB EditorDisplay. -Harry At 12:51 PM 1/16/2006, you wrote: Hi i know this has been asked and answered but i couldn't find it just getting starting with AD6, makes me feel quite dumb again when i move a component it disappears under the cursor until it is plopped down how do you see the component while moving it ? i messed w/ the 3 mask level sliders to no effect as far as i know all the color settings etc are all default thanks! Dennis Saputelli SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Large BOM line items
Hi Mike, Any version of MS Excel before version 12 has a maximum column and cell size of 255 characters. Depending on the data, and the specific version of Excel, anything over 255 characters will either be truncated or ignored. You can see a full list of Excel limits here: http://blogs.msdn.com/excel/archive/2005/9/26.aspx Regards - Harry At 06:26 AM 1/14/2006, Mike Reagan wrote: Hi All I am using Altium Designer SP4. Most of our designs have some components which are used more than 50 times. (i.e. decoupling capacitors). I have generated BOMs as CSV, text, and xls outputs. Altium does a great job with any of these formats, however when we import to into MSoft Excel, fields with large amounts of characters such as the reference designators are omitted. The problem is specific to MSOFT Excel since I have used other spreadsheet programs like Quatro Pro. Has anyone else run into this problem? Mike Reagan EDSI SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] PCAD to Protel 2004
Hi Allan, Your converted files are on their way via a zipped attachment in an off-list email. They just needed to be saved as PCAD ASCII files to allow them to be imported by Altium Designer. Regards - Harry At 07:55 AM 1/13/06, you wrote: The PCAD viewer did not indicate the version the files were developed under. When I looked at the file in ASCII mode this showed as the file header. ;ACCEL Tango PCB V15.02.02 ACCEL Tango PCB Binary (Rev 5) Allan Overcast Link Communications, Inc. Remy Sabale [EMAIL PROTECTED] wrote: The file that I have converted was created using PCAD2000 , What version of PCAD files do you try to convert? -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of [EMAIL PROTECTED] Sent: Friday, January 13, 2006 9:15 PM To: PEDA@techservinc.com Subject: Re: [PEDA] PCAD to Protel 2004 Under which version of PCAD were the files created? If I'm not mistaken, Altium takes the same basic stance as others with its model, i.e., it will import contemporary versions (the current competitive version) and their parents (the version just prior), but anything older will fail. aj -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Remy Sabale Sent: Thursday, January 12, 2006 11:08 PM To: 'Protel EDA Discussion List' Subject: Re: [PEDA] PCAD to Protel 2004 I have tried to open a PCAD files into the Protel DXP and it works fine. It also works vice versa -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Allan Overcast Sent: Friday, January 13, 2006 11:37 AM To: Protel EDA Discussion List Subject: [PEDA] PCAD to Protel 2004 I have a friend that brought me some PCAD pcb files to make some changes for. I tried to import them in Protel 2004 (service pack 4) and it fails. I downloaded the PCAD viewer from Altium and it loads perfectly. Does anyone have PCAD and can convert these files into something that Protel can load? I really don't want to re-enter the schematics and pcb into Protel for them to work. Thanks, Allan Overcast [EMAIL PROTECTED] Link Communications, Inc. - Yahoo! Photos - Showcase holiday pictures in hardcover Photo Books. You design it and we'll bind it! You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com -- No virus found in this incoming message. Checked by AVG Free Edition. Version: 7.1.371 / Virus Database: 267.14.17/228 - Release Date: 1/12/2006 You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com This e-mail transmission and its attachments may contain information from Avtron Manufacturing, Inc. that is proprietary, privileged and/or confidential and is intended exclusively for the person(s) to whom it is addressed. Any use, copying, retention or disclosure by any person other than the intended recipient or the intended recipient's designees is strictly prohibited. If you have received this message in error, please notify the sender immediately by return e-mail and delete all copies. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com -- No virus found in this incoming message. Checked by AVG Free Edition. Version: 7.1.371 / Virus Database: 267.14.17/228 - Release Date: 1/12/2006 You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 6.0 ?
So what are they asking? What have some of the people paid here in the USA or Canada? The special upgrade price which ends 31 Dec was about $2995USD for the full package, and $2495USD for PCB without FPGA. You should have called your local sales office to get it in writing. As for features, yes there are a number of features that look interesting, but the bottom line is: 1) Do they actually work? When will the 3rd service pack be available? The majority work exceptionally well - a few need to have the wrinkles ironed out. There probably won't be a 3rd service pack as you have come to know service packs. AD6 has an automated web update capability which allows smaller, more frequent patches - sort of like Microsoft does with Windows. 2) Do they actually improve productivity? Whether or not the new features improve productivity is dependent on the user. You should watch the videos available on the Altium web site and make the decision for yourself. The new video demos show the software in actual operation by the developers that wrote the software. What you will see on the videos actually exists in the finished product. If you do simple boards of only a few layers, you probably don't need all of the enhancements. If you do the sorts of boards I do, with 478 ball BGA's, lots of differential pairs, 16-20 layers, lots of manual interactive routing, etc - I believe you'll find the new capabilities take a lot of the load off. Are there bugs? - Sure there are. Have you ever had a brand new car that didn't have things that needed fixing? We're talking about a piece of software with millions of lines of code that occupies about 6.5GB on the hard drive with a full install. The developers have done a remarkable job of packing in almost everything (within reason) that users have asked for - it's almost too rich in features from my point of view (my antique brain has difficulty remembering all of the tools that are in the box). As for testing - it would be wonderful if every piece of software could be tested until it was completely free of bugs. I don't think it has ever happened, or ever will happen (Windows, the Mars lander, US Northeast Power Grid, ...). In my view, you test until you get it to a point where the software reliably does its intended function. From there on, you release the product into the world of infinite variations of hardware and operating system configurations that is the user community. Let them tell you that the software crashes every time they use instant messaging while watching a soap opera in a minimized window while downloading an mp3, and routing that 20 layer board. All of that with any one of several thousand combinations of motherboards, processors, ram configurations, video cards, sound cards, network cards, printer drivers, resident background programs, etc, etc, etc. My point being that you can only test to a reasonable point. Beyond that, you have to depend on user feedback to try and track down the state related glitches. The first issue needs no explanation. With Altium's history of putting out sparsely tested software, the first release CD is for use as a coaster for putting your soda on the desk. By the time of the third service pack in 6-12 months, the product can actually be tested. This is my experience going back to release 2.0 and I have yet to find any exceptions. With a cynical outlook like yours, you are probably better off waiting until the product is near end-of-life. You can then be sure you'll get something that has been tested to your satisfaction - of course by that time the rest of us will be using AD7. Personally, I trust Altium (Protel) to do the right thing. Nick Martin has always taken care of those who bought his product. When you try to stay cutting edge instead of stagnating like PADS, Orcad, and others in the EDA world, you're going to stumble occasionally. For example, Protel99 was a major change from Protel98 - it bombed. We got 99SE free, and it steadily improved and expanded. DXP was a major change from 99SE - it bombed. We got AD free, and it steadily improved and expanded. The difference this time is that AD6 builds on AD2004, so it has a proven core and runs on the same operating systems as DXP-AD2004. The second issue is extremely important. I go back to the global edits as an example. The new system is far more powerful than the 99SE style system and allows you to do things that were simply not possible the old way. But in the process, it makes the simple everyday tasks slower (requiring more keystrokes/clicks and use of keyboard plus mouse in many cases), reducing the overall productivity. As a result, the new way, while better in a marketing brochure actually reduces productivity and hence is worse in real life. As you seem to be, I resisted FSO when I first got DXP - I liked the old way of doing global edits. After
Re: [PEDA] 6.0 ?
For those who understand, no explanation is necessary. For those who do not understand, no explanation is possible. You don't know if what you say is accurate; however, you are convinced of its veracity. I'm getting off the merry-go-round. Harry Snip Harry, based on what you have said, I strongly suspect that you are one of the beta testers. Yes, I know that the confidentiality agreement prevents you from disclosing that relationship, but it does not prevent you from listening and thinking. As you look back through all the traffic you have seen on the private beta tester forum that gave you direct access to developers and management at Altium, did you see anyone who had strong issues with the product and was willing/able to clearly and logically articulate them? It is my experience from companies other than Altium (no experience with Altium) that other than bug reports, such forums are populated mostly by believers who do not have much critical to say. This leads the management and the developers to think that everything they do is perfect and there are no real issues. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 6.0 ?
Hi Mira, I tried 64bit WinXP for fun, and then set it aside until it matures a bit. AD runs fine under 64 bit Windows, except for port drivers. There is a subsystem in Windows 64 that runs 32bit applications. So theoretically you should be able to run anything you run on 32bit WinXP. The biggest problem is with hardware drivers; the translation subsystem of WinXP64 doesn't translate drivers - they have to be written as native 64bit code. If you are using the FPGA part of AD, you're probably not going to be able to talk to the PC parallel ports. Likewise, you'll have problems finding drivers for printers you may have. The bottom line is that 64bit Windows isn't really ready for general use yet. There needs to be quite a bit of work done on interface and peripheral drivers before you can just plug in the applications you are now using, and expect them to work completely. Regards - Harry At 06:04 PM 12/31/2005, you wrote: SNIP I've got a question - Does anyone use a PC with 64-bit processor and AD running on it? Mira SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] Default paper size
In AD2004, you have a couple of choices for initiating printing - you can print from an Outjob, or you can print from the main editor menu. The Outjob printer settings are stored in the Outjob file, and will be the same each time you print. The editor printing preferences are stored in the specific schematic or PCB file. If you don't use a standard file setup of your own to start a new job, you will see the program default to A4. If you make standard files that you copy into each new project, you can specify your own defaults. If you don't have or use standard setup files, you either have to take the time to reset the printer output each time or you have to start using the Outjob to generate your prints. This has been discussed ad nauseam in the Altium forums. Regards - Harry At 01:37 PM 12/7/05, you wrote: When I try to print it doesn't even go to my Windows default printer, it picks the first one off my list. I'm using the most recent version, AD whatever, SP4. It also defaults to A4 paper every time. Printing is a royal pain! Regards, David Kearney -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Brad Velander Sent: Wednesday, December 07, 2005 12:52 PM To: Protel EDA Discussion List Subject: RE: [PEDA] Default paper size Yeah, I know, I have read the same complaint a number of times both on this forum and the DXP forum. However, across two companies and the last 6 years of constantly using Protel P99SE, I haven't had it default to A4 size even once. It either comes up on Letter or it may come up on 11 x 17/Tabloid if that was what I last set it to for a similar print function. My suggestion was not that it was just the driver, that would mean it 'should' also behave the same way with other apps but rather a combination of the driver and something in Protel's code. Over the whole time I have used Protel I have always been connected to HP laser printers, 5000 or various 5 series printers. Sincerely, Brad Velander Senior PCB Designer Northern Airborne Technology #14 - 1925 Kirschner Road, Kelowna, BC, V1Y 4N7. tel (250) 763-2329 ext. 225 fax (250) 762-3374 -Original Message- From: bob stephens [mailto:[EMAIL PROTECTED] Sent: Wednesday, December 07, 2005 12:15 PM To: 'Protel EDA Discussion List' Subject: RE: [PEDA] Default paper size Hmm... I don't think my particular problem is with the Windows Drivers. It only happens in Protel. There has to be a global default setting somewhere, but I have yet to find it. I set my templates up as B size explicitly and whenever I turn my back the dammed Aussie POS defaults back to A4 or something equally unpleasant. :( Bob You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] New AD release
There is no new release yet - despite the press release. The new version of AD is still in Beta testing. At 04:42 PM 12/6/2005, you wrote: Anyone had a chance at looking at the new AD release? Cheers Alfonso snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Footprint needed
Hi Bill, Are you aware that there is a footprint for this chip shown in the free IPC7351 Viewer? You can download the viewer from: http://www.pcblibraries.com/resources/files/IPC-7351/IPC_Viewer_V4-00B.zip Look in the QFN footprints, and select from the least, nominal, or most library - according to your needs/wants. The specific 'nominal' library footprint for this chip would be QFN50P800X800X100-57V2N. Regards - Harry At 12:31 PM 12/1/05, you wrote: I have a Analog devices part, 56-lead Lead Frame Chip Scale Package LFCSP with an 8X8 mm body CP-56 supposed to be compliant with JEDEC MO-220-VLLD-2. Having a tough time locating a recommended footprint for this one... Any help? Also any issues with mounting? Since this is a direct to board soldered device, it may be subject to CTE mismatches and the like... anyone have experience with this part? Here's a link to the part description. http://www.analog.com/UploadedFiles/Packages/352655155839944545242119821CP_5 6.pdf Bill Brooks - KG6VVP PCB Design Engineer, C.I.D.+, C.I.I. Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510 Datron World Communications, Inc. ___ San Diego Chapter of the IPC Designers Council Communications Officer, Web Manager http://dcchapters.ipc.org/SanDiego/ http://pcbwizards.com SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Gerber viewer.
Brad, Protel 99Se came with a free copy of an older version of CAMTASTIC full feature Gerber editor. It was on a separate disc, not the installation disk for 99SE. You had to have a registered version of Protel99SE installed to license it. If you've lost your copy, you could contact your Altium sales office, and see if they can dig up an old copy for you. There are a bunch of free Gerber viewers available on the Internet. Penatlogix Viewmate is a good one, and you can download a copy from: http://www.pentalogix.com/Products/ViewMate/register.cfm Do a Google search, and you should be able to find others such as Graphicode GC-Prevue, Downstream CAMvu, etc. Regards - Harry At 02:16 PM 10/31/05, you wrote: Does Protel99SE have a Gerber viewer? After creating the CAM files with the CAM Manager and the NC Drill outputs I would like to view the Gerbers. Brad. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] Gerber viewer.
Camtastic is now integrated into DXP / AD2004. It was a separate application when provided with Protel99SE. Protel bought CAMTASTIC, which had been an independent company. After they bought CAMTASTIC, they provided the CAMTASTIC 2000 product to all licensed Protel99SE owners. You had to have Protel99SE installed in order to satisfy the license for the separately provided CAMTASTIC 2000 installation. Harry At 02:53 PM 10/31/2005, you wrote: Is Camtastic a separate application or is it built into Protel? I am guessing the original installer did not install in on the Protel workstation? Brad. -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Brooks,Bill Sent: October 31, 2005 2:24 PM To: 'Protel EDA Discussion List' Subject: RE: [PEDA] Gerber viewer. Protel 99SE came with Camtasic - a Gerber viewer/editor. Bill Brooks - KG6VVP PCB Design Engineer, C.I.D.+, C.I.I. Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510 Datron World Communications, Inc. ___ San Diego Chapter of the IPC Designers Council Communications Officer, Web Manager http://dcchapters.ipc.org/SanDiego/ http://pcbwizards.com -Original Message- From: Brad Kosiance [mailto:[EMAIL PROTECTED] Sent: Monday, October 31, 2005 2:17 PM To: PEDA@techservinc.com Subject: [PEDA] Gerber viewer. Does Protel99SE have a Gerber viewer? After creating the CAM files with the CAM Manager and the NC Drill outputs I would like to view the Gerbers. Brad. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] SILKSCREEN Overlay.
Hi Brad, I assume you are talking about an outline, and not the designator or comment. For the outline, you cannot turn it off selectively. You can double click on the component, unlock the primitives, then change the layer assignment for the outline to an unused mechanical layer, then re-lock the primitives. There is some risk doing it this way - first, you could accidentally move other primitives when they are unlocked; second, if you later update the component from the library, your outline change will be undone. As long as you keep these small risks in mind, you should be OK. If you mean the designator or comment, yes these can be individually turned on or off for each component using the appropriate check boxes. Regards - Harry At 10:23 AM 10/27/05, you wrote: I have a PCB component footprint that includes information on the overlay layer. On a particular component I do not want the overlay layer to show because it overlaps a solder pad on another component. Can the overlay layer be selectively turned on and off a footprint or must new footprints be created with various degrees of overlay information? Brad. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] tenting vias bad ?
Hi Dennis, We have required tenting on some types of boards for over a decade, and we've never had a problem. We've used both LPI and dry film. We have also used reinforced tenting in applications where the board is subjected to a pressure differential. Reinforced tenting involves mask applying a thin resin (LPI type of material) pad over the via, then tenting over the pad. There are some real concerns - as long as you are aware of them, you shouldn't have a problem. For example, if you tent the non-solder side of via-in-pad for BGA's it forms a gas pocket when soldering that can result in blown out joints under the BGA devices. Such tenting would be a rather unusual arrangement anyway. You also don't want to tent over vias under soldered thermal pads - rework becomes impossible. You will also see an argument against tenting that suggests chemicals used in processing the board will be trapped in the tented pocket, thus shortening the life of the board. While this could happen, it also requires that the board has been subjected to rather harsh chemical treatment. Such problems have been ameliorated by modern processes using more benign chemicals. We've never seen the problem on any of the hundreds of tented board designs we have done in the past. With the exception of gas driven solder BGA blowouts and specific rework cases, I would say that tenting is a non-problem. In those instances where tenting can't be used for fear of blowouts, there is the option of silver or copper fill before tenting. Fill adds cost to the board, but you do what you have to do. As an aside, looking at the specs from eprotos, it appears they use some rather old fab equipment. The internal clearance capabilities of 15-18mils is not consistent with the 4-5mils we see from fabs we have used. Likewise their minimum finished pads sizes. It looks like they are geared toward simpler designs. Their advice regarding LPI tenting may be more a function of their experience and equipment rather than the process itself. Regards - Harry At 08:24 AM 10/22/2005, you wrote: the following snip is from the e-protos web site: (http://www.eprotos.com/Design_help.pdf) i never had a fab object or had any troubles w/ tenting, what do you all think? Suggestions for Tenting Via holes: If Liquid Photo Imageable (LPI) solder mask is required, we advise that the via holes not be tented. Tenting the via holes with LPI solder mask will result in the following problems: incomplete encapsulation of the via hole, exposed copper/metal on via holes Solder, on via hole pads and in holes, uncured solder mask in the holes, which results in peeling of LPI and strapping contamination in side the holes. The solder mask pads for via holes can be made about 5 mils bigger than the via drill size. This will result in deposition of solder in the via holes, reduce the possibility of bridging problems during wave soldering operation. If the via plugging is used to fill open holes with the solder mask to block air leakage during In Circuit Test, via plugged one side is the best. We hope the above mentioned is of some help to you. If you need additional information or have any questions, suggestions, please feel free to contact us at (847) 439-5447. ds ___ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Converting Protel 99SE to Mentor Graphics
You don't say what Mentor product they are using. If it is PADS, there is a Protel to PADS converter available to Mentor customers. All they need to do is contact their local Mentor representative. I believe they can also download the converter if they are on the maintenance program. Take a look at: http://www.mentor.com/products/pcb/pads/translators.cfm Regards - Harry At 01:26 PM 9/29/05, you wrote: Received a call from a company who purchased a design I did for another company a couple years ago in P99SE SP6. They need to convert it to their in-house system using Mentor Graphics. Any good tips on the conversion? Utilities to be found anywhere? Thanks to anyone who's done this. Steve Hendrix snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] Conversion from TANGO SCHEMATIC to PROTEL???
Bill, I think you misunderstood what everyone has been saying. You can't import the Tango schematic with any Protel tool. You can import the PCB with Protel 2.8, then save it in ASCII format and import it into any of the newer Protel versions. You can directly import the Tango netlist into any newer Protel version without pre-processing. Been there... tried all of that. Regards - Harry At 08:56 AM 9/23/05, you wrote: The first few lines in the schematic ASCII file read ;Tango-Schematic 1.50 Series II TANGO_SCHEMATIC 1 1 A SHEET 0 0 17000 11000 2 SIZE 344 317 14959 9433 344 317 JUNC 7875 5225 JUNC 7975 3225 JUNC 4675 4475 JUNC 3400 4000 I have not tried PCAD because I don't have a copy of PCAD here to experiment with... I do have Protel 2.8 though and we might try importing with that... Bill Brooks - KG6VVP PCB Design Engineer, C.I.D.+, C.I.I. Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510 Datron World Communications, Inc. ___ San Diego Chapter of the IPC Designers Council Communications Officer, Web Manager http://dcchapters.ipc.org/SanDiego/ http://pcbwizards.com -Original Message- From: PCB Designs [mailto:[EMAIL PROTECTED] Sent: Friday, September 23, 2005 4:29 AM To: Protel EDA Discussion List Subject: Re: [PEDA] Conversion from TANGO SCHEMATIC to PROTEL??? Abd ulRahman, Anyone know how to import a schematic from TANGO SCH to Protel? Also, how about from TANGO PCB to Protel? I know of no way to convert Tango SCH. We can do Tango design if necessary. I think. It has been quite a while. Tango PCB can be imported into Protel using Protel 2.8. I did it quite a few times. I think Bill also has PCad 2K, so there is a possibility here. PCad2K also imports Tango PCBs, even better than Protel 2.8 (on polygons). PCad2K also imports Tango ASCII schematics, the trick here is to have the complete Tango schematic library, then you have to use Library Executive to import the Tango Library to the PCad format, setup the library in the PCad schematic program, and then import the Tango schematic. Hope this helps. Best Regards, Paulo Egon You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Conversion from TANGO SCHEMATIC to PROTEL???
You're out of luck on the schematic - there's no way to do an import into Protel. However, you can bring in the netlist - there are knowledge base articles that describe the procedure. The PCB is another story. You can import the Tango program to Protel version 2.8, save it in PFW format, then open it in any of the later versions of Protel. Regards - Harry At 05:16 PM 9/22/2005, Brooks,Bill wrote: Anyone know how to import a schematic from TANGO SCH to Protel? Also, how about from TANGO PCB to Protel? Bill Brooks - KG6VVP PCB Design Engineer, C.I.D.+, C.I.I. Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510 Datron World Communications, Inc. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] DXP 2004 Netlist import?
The netlist has to be put into AD2004 format first - that can be done with a word processor, or a product like RSI Omninet. To import the netlist, follow the process described at: http://www.altium.com/forms/kb/kb_item.asp?ID=3439 You can import directly schematics done in Orcad, or PCAD, and Specctra DSN files. The netlists for these formats can be generated in AD2004 once the schematic import is completed and cleaned up. At 11:22 AM 9/12/05, you wrote: Hey All Simple question. Is there a netlist import facility in Altium Designer, so you can work from input not using Altium schematic. If not using Altium Designer as freelancer is impossible. Regards Soren Juel snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Parallel Port and Altium Designer Service pack 4 Installation
First - SP4 cannot be run by itself. It is only intended to update an Altium Desginer installation that already has all the previous service packs installed. If you downloaded SP4 from the Altium web site, all you got was the update - it is not a complete installation. The correct sequence of installation is: DXP2004, then SP2 (SP2 is cumulative and contains SP1), then SP3, and finally SP4. If you requested a Demo disk from Altium, it will come with one or more of the service packs already installed - which it has will be marked on the disk and/or jacket. Second - you should look at the Altium Knowledge Base with respect to parallel ports for computers without one. Try as a starting place: http://www.altium.com/forms/kb/kb_item.asp?ID=4877 At 05:28 AM 9/7/05, you wrote: I didn't install AD SP3 on the laptop. I am trying to install the downloaded version AD SP4.I bought the Quadtech PCMCIA to parallel adapter card. The installation failed even after installing the card. http://www.quatech.com/catalog/parallel_pcmcia.php I wish Altium would fix this problem. Any suggestions? -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Tony Karavidas Sent: Tuesday, September 06, 2005 5:27 PM To: PEDA@techservinc.com Subject: Re: [PEDA] Altium Designer Service pack 4 If you say it require a parallel port to do the new installation, how did you do that? SP4 will only update SP3, so you must have installed something before now. I also have a Sony Vaio (620 I think) and it doesn't have a parallel port, but AD installed just fine. Tony Quoting Al-hamra Huq [EMAIL PROTECTED]: I am trying to install Altium Designer SP4 on a laptop without a parallel port. A new installation of Altium Designer requires PC to have a parallel port. Does anyone know how to get around the problem? I get the error message Failed to Load Parallel Port Driver during installation. Thanks. Al-hamra Huq Electrical Engineer Clean Earth Technologies, LLC 13378 Lakefront Drive, Earth City, MO 63045 Ph:(314)-222-4640 ext 130 Ph:(314)-222-4650 Privileged/Confidential Information may be contained in this message. If you are not the person(s) indicated in this message (or responsible for delivery of the message to such persons), you may not copy, deliver or forward this message to anyone. In such case, you should delete this message completely, and kindly notify the sender immediately. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Norton Antivirus software... interfere with Protel?
I would second the suggestion to abandon the Norton software. I was one of Peter Norton's first customers back in the good old DOS days. His software was solid and did a few really useful jobs in DOS and early MS Windows versions. After he sold his stuff to Symantec, the products began to show quirky behavior, and after a couple of years became the source of many problems with Windows 3.1, 95 and 98. I eventually began recommending to anyone who would listen, that the first thing to do when having consistent crashes or lockups was UNINSTALL all Symantec products. That advice fixed more computers than I can count. I haven't used a Symantec/Norton product since, and I haven't missed them. For anti-virus protection, there are alternatives such as McAfee and Kaspersky that have caused me less grief than the years of fighting with Symantec. Harry Selfridge Encore Engineering Services and Products At 05:57 PM 8/24/2005, you wrote: Brooks,Bill wrote: Does anyone have any data that would indicate that the slow performance of Protel 99SE on a windows 2000 Professional based system could be related to the Norton Antivirus program interaction with it? Lately my system is really running slow... I have 99SE and DXP 2004 on my system... Any help much appreciated... My favorite computer guru told me that half of his business was generated by Norton products. Therefore, when I updated my computer with a new hard drive, I did a fresh install of everything and left out Norton. While it is hard to make a fair comparison and I made no measurements, I think that it runs better and I have no plans to install Norton. For example, there are fewer times where I am doing nothing and the hard drive is busy as a beaver. Those disturb me. Jim Walker Walker Power Design, Inc. [EMAIL PROTECTED] snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] AD and 99SE on the same system.
H Something went wrong with the first shot on this reply - it looks like an early edit was sent by mistake. Let me try again. From my experience, the system you describe should work for you. You may see performance hits with large number of polygon pours, or large fills. A large board (over 2K pins) with online DRC turned on may also run somewhat slowly. One thing to watch is drive space. The installation itself is large with all service packs installed (about 3.7 GB, around 890 directories, and 21,000 files - including libraries). Backup files, output files, history files, etc. can build up quickly and eat drive space. In my opinion, a critical component is the video card. AD2004 is VERY graphics intensive. Having said that, cheap older generation Nvidia graphics cards seem to do quite well - but, the faster the better. I have run AD2004 on an AMD Athlon 64 2.6Ghz with 1GB RAM. Subject to the comments above, the performance was acceptable. I have also run AD2004 on a DELL Dimension 6000 laptop - it was slw... but usable at customer locations for review and discussion. Regards - Harry At 09:14 AM 6/27/05, you wrote: Hey Guys, Thanks for all the replies on AD and 99SE. I've now got an evaluation license of AD running and I'm fairly impressed with some of the feature improvements. I can't say I'm looking forward to the learning curve though. So far, AD seems to run on my desktop (P3 2.6G, 1G Ram) fairly well. However, the minimum system requirements seem pretty stiff and the recommended system requirements are almost ridiculous. IME, you usually need better-than-recommended resources to get good performance. Does anybody have a feel for whether this is the case with AD? Or will the minimum system requirements give us acceptable performance? If we have to upgrade several machines, the cost of upgrade is obviously higher than initially thought. We only do schematic capture, pcb layout, and some 3D mechanical stuff, so we're not using some of the obviously resource intensive functionality like circuit simulation. Again, your knowledge and experience is appreciated. Darcy -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Darren Sent: June 17, 2005 6:56 PM To: 'Protel EDA Discussion List' Subject: RE: [PEDA] AD and 99SE on the same system. Hi Darcy, As others have said, no problem, I have had 2.8, 99SE, DXP2004 SP2 and AD SP3 all running fine. I don't share the designs files as a rule, I have a separate image of my files for each version. Darren Moore Hey Guys, For those of you who have used Altium Designer and Protel99SEWill these two programs play nicely together on the same computer? We definitly need access to the 99SE software to support legacy designs. However, we're looking into Altium Designer. As most of you are aware, altium keeps threatening that the upgrade path is going to disappear. However, if we're going to purchase new seats instead, than I don't care about the upgrade path. Darcy snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Altium Community Forums
As far as I can tell watching the Altium Forums, you haven't been orphaned if you use 99SE. You may not realize it, but this forum (PEDA) is maintained by a private company that does the same kind of work you do - it is NOT an Altium sponsored forum. This forum was established before Protel/Altium improved their support and established their own forums. Altium does monitor this forum from time-to-time, but most of their effort is devoted to moving forward - not looking backward. If you registered for one of the active Altium company forums, you probably would find more support. Most of us who moved on from 99SE only occasionally monitor PEDA, but we watch the Altium forums daily. If you want more help from experienced users and Altium programmers, you should consider moving where they have gone. Protel99SE with service pack 6 is two versions older than the current version of Protel (Altium) software, and it is nine revisions behind if you count the service packs. Support for obsolete products is no better from Cadence than it is from any other EDA vendor. If you go back the same number of versions in Orcad, you end up at version 8 (an unmitigated disaster of software bugs!) I have used Orcad since the days of DOS. When Cadence bought Orcad, support went into the toilet. Cadence maintains Orcad as their low end product, just as Mentor bought PADS as their low end product. Unless you are willing to pay for a support contract, you'll play hell trying to get detailed answers from them. Bottom line - if you choose to use old software, you can use the old forum archives and troll for answers among those who are doing likewise. The company experts are going to be found concentrating effort on new problems, not old ones. Altium is the only company with whom I deal that doesn't charge for direct answers from their software engineers regarding product problems and improvements - old or new. At 10:59 AM 6/24/05, you wrote: Brad Velander wrote: From what I read from various lists with OrCAD users, you think you are any better off with a tool that has been delegated to foreign ESL programmers to simply maintain? Being maintained by ESL programmers is a hell of a lot better than what we have with 99SE -- completely orphaned. Hamid You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] Altium Community Forums
Hi Brad, I don't believe there would be loud objections to questions regarding 99SE - just my personal opinion based on the character of the Altium folks with whom I have dealt. I do believe that the kind of obnoxious, snotty, attitude that is presented by some folks on this forum might be ignored or earn them an invitation out the door. Polite, intelligent, questions seem to get attention. Regards - Harry At 04:30 PM 6/24/2005, you wrote: Thanks Harry, Well put. It saved me from replying to say basically the same thing but I wouldn't have been quite so concise and coherent. However, Since Altium has previously announced an end to P99SE support, I am sure they do not want people posting P99SE issues on the new forum. I am not sure if you were suggesting such but I highly doubt it. Sincerely, Brad Velander Senior PCB Designer Northern Airborne Technology 1925 Kirschner Rd., Kelowna, BC, V1Y 4N7. tel (250) 763-2329 ext. 225 fax (250) 762-3374 -Original Message- From: Harry Selfridge [mailto:[EMAIL PROTECTED] Sent: June 24, 2005 1:53 PM To: Protel EDA Discussion List Subject: Re: [PEDA] Altium Community Forums SNIP Bottom line - if you choose to use old software, you can use the old forum archives and troll for answers among those who are doing likewise. The company experts are going to be found concentrating effort on new problems, not old ones. Altium is the only company with whom I deal that doesn't charge for direct answers from their software engineers regarding product problems and improvements - old or new. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] AD and 99SE on the same system.
We have 98, 99SE, and AD2004(SP3) all playing together nicely on a Windows XP Pro system. We haven't run into any problems with the various versions conflicting. At 10:23 AM 6/17/05, you wrote: Hey Guys, For those of you who have used Altium Designer and Protel99SEWill these two programs play nicely together on the same computer? We definitly need access to the 99SE software to support legacy designs. However, we're looking into Altium Designer. As most of you are aware, altium keeps threatening that the upgrade path is going to disappear. However, if we're going to purchase new seats instead, than I don't care about the upgrade path. Darcy snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA]Easy way to make a Plated Slot?
Nopenothing easier than describing it with a fab note. At 05:08 PM 5/18/2005, you wrote: Is there an easy way to make a plated square slot in 99se other then defining one in a fab drawing? Thanks, J. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] IPC Format Bill of Material
If you were looking for one simple BOM format, you are out of luck. There are several IPC documents that may be relevant. You have to pick through them to find out what applies to your situation. Each of the documents mentioned below will also give references to other documents that might apply. IPC D-325A - Documentation Requirements for Printed Boards (describes the parts list) This document has to be purchased from IPC, and can be found on the IPC website in the Standards section IPC 2578 - Sectional Requirements for Supply Chain Communication of Bill of Material and Product Design Configuration Data - Product Data eXchange (PDX) This can be downloaded free at - http://webstds.ipc.org/2578/2578pub.pdf IPC 2571 - Generic Requirements for Electronics Manufacturing Supply Chain Communication - Product Data eXchange (PDX) This can be downloaded free at - http://webstds.ipc.org/2571/2571pub.pdf IPC 2518A - Sectional Requirements for Implementation of Part List Product Data Description [PTLST] This can be downloaded free at - http://webstds.ipc.org/2518/2518Apub.pdf The automated data exchange concept, noted above as PDX, is described at http://www.pdxstandard.org/pdx/. There is also an article that describes the overall PDX concept at http://smt.pennnet.com/Articles/Article_Display.cfm?Section=ArticlesSubsection=DisplayARTICLE_ID=214389 At 02:42 AM 5/14/2005, you wrote: Hi All, I am in search of IPC format Bill of Material files so that we can streamline our components ordering process for circuit boards. Can someone provide me with a link having the info about the aforesaid standard regarding the BOM files. Regards, Adeel Malik snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] PCB: Place from file?
Soren, I assume you must be using Protel99SE, since DXP2004 has special utilities for doing multi-channel boards. I just tried it and it works perfectly using Protel99SE. I saved a PIK file, moved a component off the board and rotated it, saved my modified board, then auto positioned using the PIK file I saved earlier. The component ended up back where it was before I made the changes. There are a couple of things you possibly have not tried: - After you save the PIK file, and you change the component coordinates - did you save the changed PCB file? You have to save a file after changes have been made in order to operate on it with the PIK file. If you don't want to modify your original, you can do a Save As with a different file name. - After you use 'auto position using a file', did you refresh the display? You can do that manually using hotkeys 'VR'. Regards - Harry At 10:07 PM 5/7/2005, you wrote: Thanks for the answer, but this is what I have done on two different computers! I have created the pik file from the design and have inside protel changed the mid x coordinate for one component. Then doing what you write nothing happens. I have 5 channels I like place like channel 1 but with other x coordinate, 1000 components, so I had hoped it worked for me. regards Soren Harry Selfridge wrote: This should more correctly be called component relocation because components matching those in the PIK file already have to be on the board somewhere for this to work. For Protel99SE, you go to 'ToolsAuto PlacementPlace from File' and select your PIK file. The designators and footprint names have to be the same for both the components to be relocated and those in the PIK file. For DXP2004, it works the same except you go to 'ToolsComponent PlacementPlace from File' and select your PIK file. At 02:14 PM 5/7/2005, you wrote: Hey All I know this issue has been up before, but my disk crashed and I lost all mail. How to place components from a *.pik file? It does not seems to work. regards Soren Andersen snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
RE: [PEDA] PCB: Place from file?
Hi Brad, The initial reply went out to the discussion list. Even though I'm in the same state as their server, I note that it takes about 2 hours before I see my posts reflect back. I can exchange email with a client in Boston (3000miles away) almost instantaneously. I too occasionally see a reply without seeing the original post. You may yet see the original post that I made at 4:39PDT yesterday. With their server - who knows? Regards - Harry At 01:57 PM 5/8/2005, you wrote: Harry, just wondering, did you reply directly to Soren the first time? I saw him reply to your response and I see your second response below but didn't get your initial reply. Seems the PEDA server is acting up and missing on the delivery of some messages. Sincerely, Brad Velander Senior PCB Designer Northern Airborne Technology 1925 Kirschner Rd., Kelowna, BC, V1Y 4N7. tel (250) 763-2329 ext. 225 fax (250) 762-3374 -Original Message- From: Harry Selfridge [mailto:[EMAIL PROTECTED] Sent: May 8, 2005 10:06 AM To: Protel EDA Discussion List Subject: Re: [PEDA] PCB: Place from file? Soren, I assume you must be using Protel99SE, since DXP2004 has special utilities for doing multi-channel boards. I just tried it and it works perfectly using Protel99SE. I saved a PIK file, moved a component off the board and rotated it, saved my modified board, then auto positioned using the PIK file I saved earlier. The component ended up back where it was before I made the changes. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] PCB: Place from file?
This should more correctly be called component relocation because components matching those in the PIK file already have to be on the board somewhere for this to work. For Protel99SE, you go to 'ToolsAuto PlacementPlace from File' and select your PIK file.The designators and footprint names have to be the same for both the components to be relocated and those in the PIK file. For DXP2004, it works the same except you go to 'ToolsComponent PlacementPlace from File' and select your PIK file. At 02:14 PM 5/7/2005, you wrote: Hey All I know this issue has been up before, but my disk crashed and I lost all mail. How to place components from a *.pik file? It does not seems to work. regards Soren Andersen snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Bypass capacitors
You don't say what version of software you are using. If it is Protel99SE, open the PCB file, go to FileCAM Manager, follow the wizard and select BOM as the output, you can then press F9 to generate the BOM or you can go to ToolsGenerate CAM Files. Your BOM will be generated for all the components on the board. If you are working with DXP2004, open the PCBDOC, go to ReportsBill of Materials. There are various add-ins, scripts, etc to tailor the BOM. The above is just the barebones way of getting the basic report. At 12:15 PM 5/6/05, you wrote: The bypass capacitors for each of the IC's in a project I've taken over are displayed on the PCB Layout view but not on the BOM or the schematic. How do I get those components listed on the BOM? snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] negative net length?
Craig, Now that you have SP2 installed, you can save your preferences as a file, and import them into any future reinstall (ToolsPreferences - Save button at bottom of window). Menu, toolbar, and shortcut customization is saved, along with schematic and pcb default primitives. Workspaces can also be saved (FileSave Workspace as). Altium made it happen because paying customers asked for it. Blame the minor inconvenience of re-licensing on pirates that don't want to pay for the software or the improvements (including the ability to save program customization). Regards - Harry At 04:12 PM 5/3/2005, you wrote: I just installed DXP 2004 SP2 Not only did I have to go though the licensing/activation procedure again, I find that all my customised setting have reverted to defaults. Protel, you've done it again. Imagine if every time you applied a Windows SP you lost your profile and had to set it all up again. Not happy Jan Craig snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Physical Properties of Polyamide
Jeff, I don't think you're going to find a simple answer for this one. There are just too many variables - temperature, maximum flaw size, copper thickness, direction of force, etc. I believe your best bet is to mechanically restrain the component such that it doesn't transfer force to the pad. The force should be absorbed by fasteners that transfer the shock to the board and/or board supports. This sort of question is why prototypes are built and tested on shake tables. Regards - Harry At 07:59 AM 4/27/05, you wrote: Does anybody know how much force I can apply to a pad before it will brake loose? I plan to mount a surface mount component on a polyamide PCB which needs to handle a 10G shock. Jeff Stout P.S. I'm grateful for any information provided. snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] DXP 2004 SP2 Netlist Import Warnings.
I saw an error like this when trying to import an IPC-356 file generated by PADS. It has been long enough that I can't recall how it was resolved. The best place to post your problem is in the Altium DXP forum. The programmer that does the Camtastic portion of DXP monitors the forum, and jumps in whenever he sees Camtastic in the subject line. If you're not already a member of the forum, you can join at: http://forums.altium.com/ At 06:49 AM 4/26/05, you wrote: I am trying to import an IPC-356-D netlist created from Eagle into CAMtastic 2004. All the lines of the netlist produce the Warning message: Warning: Invalid Record Length - 71. The length should be 74. Record skipped. In some cases the 71 is a different number but in all cases the record length is 74. Has anyone used the IPC-356-D netlist import successfully? Does anyone have a sample netlist I could try/compare with the Eagle generated netlist. Thanks, Ken -- Ken Bowers IR Halifax 7020 Mumford Road Halifax, NS, Canada B3L 4S9 902.431.1644 x250 You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] manufacturing export problems
It is a peculiarity of Gerber editors that they don't open Gerber files - they open their own version of CAM files. You have to IMPORT Gerber files. Go to FileImportGerber (or drill, or aperture), and select your files. Your files will open just fine. Note that, depending on the editor/viewer, you may have to choose all files to display the files with Protel Gerber extensions. Some editors/viewers expect all Gerber files to have the extension .gbr or .pho. The Protel extensions give you more info about the file, and they don't prevent you from importing them - you just have to train the Gerber editor/viewer. At 03:22 AM 4/19/05, you wrote: Hello all: I have the following trouble: In protel 2004, after creating a PCB board with 2 layers and some drills and vias, I create the output manufacturing files (gerber and nc drill) but none of this files can be opened in a gerber viewer software. Can somebody solve this problem? Posted from Association web site by: muixego snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] DXP 2004 Netlists (Corrected)
Nuts! I typed too quickly and made a couple of mistakes. I fixed them below. First, you should install Service Pack 2 for DXP2004. There have been a lot of bug fixes and improvements since the version you are trying to use. The files that your project is complaining about were probably not kept in their original relative folder locations when the project was sent to you. The project file keeps pointers to all the associated document locations when they are saved. If your customer moved files around from folder-to-folder or changed folder names to send them to you, there is no way for the project document to find them automatically. If they are present in the files you got, you can put the documents back into the project by right clicking on the project name in the 'Projects' tab, and then using Add Existing to Project. As for your specific questions: 1) Open the Projects tab, right click on the project name, select Open Project Documents. That will open all the documents that the project file knows about and can find. If there are too many documents for a single tab across the workspace, a compressed tab will appear that says something like '(x) y.schdoc. Click on that compressed tab and a menu will drop down for you to select the page you want to look at. 2) With the top sheet of the schematic open, go to ProjectCompile Project. That will run a check on the schematic against the design rules. The results will be under the Messages tab. Double click on the error messages and it will take you directly to the trouble spot in the schematic. Some of the messages will just be warnings to check and be sure you really want to do what you have done - they aren't show stoppers, they're just cautionary. Show stoppers will be obvious errors instead of just warnings. 3) Go to http://www.altium.com/downloads/2004_outputters.asp after you have installed SP2 as I suggested above. Download the specific netlister for your needs, and install the .out and .dll files to the Altium2004 system directory. You can then output a netlist specifically for the correct version of PCAD from the menu DesignNetlist for Project (or Netlist for Document). 4) See (2) 5) Install SP2, your output files will then appear in a 'Project Outputs' folder under the main project folder. If I remember correctly, in the version of DXP2004 you are trying to use, the output went by default to the Windows Document folder for the user. 6) A project is a collection of all the documents - schematics, layout files, reference documents, netlists, reports, etc. A design is the individual layout document or schematic document within the project. At 01:51 PM 4/18/05, you wrote: Background: I was sent a set of files to open and make into a PCB. They are DXP 2004 vintage. I open DXP 2004 (Build 8.0.4.1272) and look for a schematic. There are a bunch of SCHDOC files, a DOT file, and a PrjPcb file. I open the PrjPcb file and there are 3 errors: 1) a SchLib could not be found even though it is listed among the files, 2) and IntLib could not be found but didn't exist in the files, and 3) A SchDoc could not be found but didn't exist in the file. It said all 3 were removed from the project. OK, a bunch of files come up. Looks pretty much like a set of schematic sheets. Questions: 1) How do I open all schematic sheets so I can easily browse through them without having to open them one at a time? 2) How do I run DRC on the schematic? 3) What is the best Netlist format to export to P-CAD 2002. In the past I was using the *.alt file format (Master Designer?) from 99SE, but that does not appear to be available any more. 4) Do I need to compile this and if so how? 5) When I choose any of the .prj file or .SchDoc files I can do Design = Netlist For Project. I then select the Tango format. When I do this is seems to go through all the sheets, and then... The DXP closes altogether. There does not appear to be any netlist file generated, in the directory or referenced in the project when I try to open it up. 6) What is the difference between a project and a design? Jeff You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current
Re: [PEDA] DXP 2004 Netlists
First, you should install Service Pack 2 for DXP2004. There have been a lot of bug fixes and improvements since the version you are trying to use. The files that your project is complaining about were probably not kept in their original relative folder locations when the project was sent to you. The project file keeps pointers to all the associated document locations when they are saved. If your customer moved files around from folder-to-folder or changed folder names to send them to you, there is no way for the project document to find them automatically. If they are present in the files you got, you can put the documents back into the project by right clicking on the project name in the 'Projects' tab, and then using Add Existing to Project. As for your specific questions: 1) Open the Projects tab, right click on the project name, select Open Project Documents. That will open all the documents that the project file knows about and can find. If there are too many documents for a single tab across the workspace, a compressed tab will appear that says something like '(x) y.schdoc. Click on that compressed tab and a menu will drop down for you to select the page you want to look at. 2) With the top sheet of the schematic open, go to ProjectCompile Document. That will run a check on the schematic against the design rules. The results will be under the Messages tab. Double click on the error messages and it will take you directly to the trouble spot in the schematic. Some of the messages will just be warnings to check and be sure you really want to do what you have done - they aren't show stoppers, they're just cautionary. Show stoppers will be obvious errors instead of just warnings. 3) Go to http://www.altium.com/downloads/2004_outputters.asp after you have installed SP2 as I suggested above. Download the specific netlister for your needs, and install the .dll file to the Altium2004 system directory. You can then output a netlist specifically for PCAD from the menu DesignNetlist for Project (or Netlist for Document). 4) See (2) 5) Install SP2, your output files will then appear in a 'Project Outputs' folder under the main project folder. If I remember correctly, in the version of DXP2004 you are trying to use, the output went by default to the Windows Document folder for the user. 6) A project is a collection of all the documents - schematics, layout files, reference documents, netlists, reports, etc. A design is the individual layout document or schematic document within the project. At 01:51 PM 4/18/05, you wrote: Background: I was sent a set of files to open and make into a PCB. They are DXP 2004 vintage. I open DXP 2004 (Build 8.0.4.1272) and look for a schematic. There are a bunch of SCHDOC files, a DOT file, and a PrjPcb file. I open the PrjPcb file and there are 3 errors: 1) a SchLib could not be found even though it is listed among the files, 2) and IntLib could not be found but didn't exist in the files, and 3) A SchDoc could not be found but didn't exist in the file. It said all 3 were removed from the project. OK, a bunch of files come up. Looks pretty much like a set of schematic sheets. Questions: 1) How do I open all schematic sheets so I can easily browse through them without having to open them one at a time? 2) How do I run DRC on the schematic? 3) What is the best Netlist format to export to P-CAD 2002. In the past I was using the *.alt file format (Master Designer?) from 99SE, but that does not appear to be available any more. 4) Do I need to compile this and if so how? 5) When I choose any of the .prj file or .SchDoc files I can do Design = Netlist For Project. I then select the Tango format. When I do this is seems to go through all the sheets, and then... The DXP closes altogether. There does not appear to be any netlist file generated, in the directory or referenced in the project when I try to open it up. 6) What is the difference between a project and a design? Jeff You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Landscape Printing to PDF995
I don't use PDF995, but Acrobat also needs to be set up using Properties from the Printer Setup Menu. It will default to the Windows printer values as set in the Windows Printer dialog. Try going to the Printer Properties, and setting the landscape option there as well. At 02:18 PM 4/18/05, you wrote: The schematic DXP 2004 schematic I inherited is landscape tabloid (17 wide by 11 tall). It is defined as 1 less in each direction in the document options. No matter what combination of landscape/portrait I choose in either the printer setup or the print screen I cannot seem to get the landscape schematic to print on the landscape sheet. It always comes out a landscape image shrunk to fit across a portrait sheet. Any ideas? Jeff snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Mechanical Stresses on PCBs
Hi Darcy, The following is strictly my opinion from an engineering standpoint. There are too many variables to define excessive flexure. Deflection of a PCB in one direction may cause no problem, but may crack a SMD capacitor if it happens 90deg offset. Likewise, flexure across a pcb trace may cause no harm while flexure in line with the trace might crack the trace. Amount, direction, rate of flexure, number of deflections, board composition, board stackup, copper weight, surface plating, temperature, component sizes, size and location of board mounts, etc, all would affect the end result of flexure. There are some tried-and-true methods for stiffening a board in areas of concern. A vertical metal rib can be soldered to the top or bottom of the board. Mounts can be placed under the point of pressure (screwed or glued plastic or hard rubber bumpers) to limit travel. Sockets/connectors can be mounted to the enclosure to transmit insertion force to the enclosure rather than the board. Stiffening support frames of plastic of metal can be mounted to the enclosure. Etc. Flex mounting the board can be done in a number of ways. There are press-fit nylon board standoffs, and flexible screw type nylon standoffs. Belleville, or wave spring washers can be used under the board at the mounting points. Mounting holes can be inserted with rubber or plastic grommets. Mounting screws can be bottomed in mounting standoffs, leaving drift clearance. Etc. The right solution for your problem is going to be unique to your application. It may be one, or a combination, of some of the kinds of things I mentioned above. Regards - Harry At 07:50 AM 4/14/05, you wrote: Hey Guys, One of the latest issues we've run across (while trying to balance weight, size, money) in a current design is that there is some potential for mechanical stresses to be induced into the PCBs in the end user product. This causes a couple issues. The first is the obvious solder joint integrity and the possibility of damaging components or traces on each PCB. The second is the alignment of a board to board connector (Hirose DF12 series) between two PCBs. My first gut reaction is absolutely no stresses are acceptable in the PCB, but since we're balancing the above objectives, I thought I'd throw some questions out. 1) Has anybody got an opinion or has read some article on allowable stress or flexure of populated PCBs? 2) Have you seen any sort of flexible mount that could be used to float the PCBs. Currently we're using 3mm screws to secure the PCBs so we're looking for a solution that would be the same order of magnitude in size (ie. Chev 454 motor mounts are too big!) Thanks for any suggestions you may have. Darcy Davis Design Engineer, Dynastream Innovations, Inc. You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Wanted: P99SE
Hi Mira, Below is the response I got when I asked our local sales office via email about a used copy of Protel99SE we were planning to buy: QUOTE-- Good morning. Thank you for notifying us of the pending license transfer. Our records do indicate that this is a valid license, and has yet to be upgraded to Protel DXP, thus would qualify for an upgrade if you were to acquire the license. In order for us to properly transfer ownership of this license, I will need an authorized letter (fax is fine) from the current owner stating that they are selling the license, as well as an indication as to whom they are selling it. I will be happy to facilitate this, so please contact me if you have any questions or additional concerns. Best regards, Matt Clark Altium - Making Electronics Easier! == 17140 Bernardo Center Drive, Suite 100 San Diego CA 92128 Phone: (858) 485-4624 Fax: (858)-485-4611 Email: [EMAIL PROTECTED] --END QUOTE This is quite different from the response you received. Either Altium has changed their view, or you talked with a sales representative who doesn't know the company policies. It would probably be beneficial to call again and speak with someone who has been with the company for a while. Regards - Harry At 11:26 PM 4/9/2005, you wrote: I talked to our rep about buying an used package and they told me that it would be my own risk because I wouldn't get the license transfered to me and my copy wouldn't be legal. They said that Altium has never had policy to transfer licenses and they didn't sell used packages. Mira --- Abd ulRahman Lomax [EMAIL PROTECTED] wrote: At 11:38 AM 4/7/2005, Steve Allen wrote: I'm working with a customer that has interest in purchasing his own copy of P99SE. I'm hoping some of you can help answer some questions we have. 1. I thought I saw a PEDA post that indicated that Protel no longer offers upgrade discounts from P99SE to Protel 2004. Is this still true? It looks like they no longer offer upgrades at all. Rather, they offer legacy 99SE customers an unstated (on the web site) discount on the purchase of 2004. I haven't had an opportunity to call them since I noticed this, so I don't know what the discount it. I might think that an upgrade price and a discounted price were the same thing; but if I assume that they are different, I can only imagine: Protel has long considered that an original license was subsumed into an upgrade license. So, for example, once a license was used for upgrade, it was no longer an independent license and could not be sold unless the newer license were sold with it. Actually, they claimed that if the old license were sold, they would consider that the new license was also sold, they would not transfer them independently. However, a discount in the purchase of a new license, which is how they stated it on the web site, would imply that the new license is independent of the old license. This might, under some circumstances, actually increase the market value of an older license, because some buyers might indeed want two licenses, albeit one for 99SE and one for 2004. Perhaps 99SE could be used for schematic entry and the creation of footprints, and 2004 by another engineer or designer for PCB design. And, should they become surplus, either license could be sold. But I haven't looked at a recent 2004 license. Protel might still restrict the transferability of a license used for discount. Or there might be other nasty surprises; it is a bit troubling that the actual policies are not explicitly published. Based on the history, however, I'd be surprised if something truly harmful to users has happened. 2. Is there still a Protel 99SE resale market? It has never been very active. But there is traffic on the list [EMAIL PROTECTED] I don't personally know of any recent sales, but I'd not necessarily hear about it. 3. If so, what's a used copy of 99SE selling for? Before the policy changed, the last price I knew of was $3500. Depending on the details of Protel's new policy, the current value might be higher or lower than that. For example, suppose that the appearance is real, that an upgrade right has been replaced by a discount offer, in which event the new license is independent of the old and both of them are now transferable, or, at least, the older one is. And suppose that the discount is $4000. The older license would have a use value, which could easily be $2000, comparable to Circuit Studio 2004. If we devalue the discount by 25% -- people expect some kind of savings when they buy used licenses, though, in the past, used licenses have been quite the same as new ones -- that would leave the value of a 99SE license at $4000. In other words, it is possible that the market value of an older license has increased as a result of the change. I would expect that Altium might refuse to allow a legacy
Re: [PEDA] RJ45 Pin Numbering Scheme for Notch at the Bottom and notch at the top
Pin 1 on the RJ45 is always in the same place relative to the locking tab (I assume it is the notch for the locking tab to which you refer). If you look into the socket from the front, and the locking tab notch is on the bottom, pin one is on the left. If you turn the socket over, such that the locking tab is on the top, pin one is on the right. Likewise, if the socket is manufactured to mount with the locking tab up, pin one is on the right. Is there more to this question? At 08:43 AM 4/9/2005, you wrote: Hi All, RJ45 Socket which has a notch at the bottom of the package (when looked from front) has its Pin1 on the left. I want to ask where will be the Pin 1 for the RJ45 Socket which has its notch at the Top. Can someone help me as I don't have the RJ45 Socket in hand that has Notch at the top. Regards, Adeel Malik snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Porting P99SE libraries to DXP
This rings a bell - are your misbehaving component names being truncated by any chance? I seem to remember a problem with long part names getting characters dropped, and that confuses the compiler. I may not be recalling the circumstances correctly, but I remember an issue with the length of the component name field at some point. At 04:26 PM 3/29/2005, you wrote: Hi Gang, Does anybody here have any idea why I would be getting the following error message on several P99SE library parts that I am trying to port from my P99SE libraries into a DXP integrated library? All three parts exhibiting the problem are simple logic gates (ie. 4 gates (parts) of a 2 input NAND). There are the 2 input pins and 1 output pin on each gate and then on the 4th gate there is the additional VCC and GND pins. The message I get is: [Warning] IC_99.LIB Compiler31-13-000 CMOS 74HTC MM74HCT00M: Could not find ' ' Every pin has a pin number, none are (blank). So I don't understand what the message is trying to point out. I have seen this same message on some special parts where there was a pin with a blank pin number, so I have been trying to find the same in these symbols but a blank pin number just doesn't exist. I have many more multi-part logic gates that work just fine, thus far I cannot determine what is different to make these few fail while the others integrate just fine. Any ideas, suggestions? What is the error message trying to point out that I am missing? Just plain brain-dead on this one, Brad Velander Senior PCB Designer Northern Airborne Technology 1925 Kirschner Rd., Kelowna, BC, V1Y 4N7. tel (250) 763-2329 ext. 225 fax (250) 762-3374 snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 44L-TQFP PCB footprint
Leo, I was referring to the QFP44 PCB footprint in the default PCB library supplied with Protel98. If you measure the primitives using hot keys RM (Report Measure), you will see that the supplied footprint is nearly a perfect fit for your device - all I would do to improve it for hand assembly would be to modify the silkscreen outline and increase the pad width a couple of mils. To edit the existing QFP PCB footprint using the library editor takes less than 5 minutes. Using the library editor from the datasheet to build a new PCB footprint takes about 10 minutes. You really should give it a try - depending on others to do the work for you will almost certainly lead to disaster. If you learn to do it yourself, you can take into account the soldering method you will be using, the alignment tolerances of any placement equipment, the board real estate available, etc. Regards - At 06:38 AM 1/18/05, you wrote: Hi Harry, I hope you were not referring to a schematic library. I don't think it would be possible to edit a pcb library file in 10 minutes. Also, I have found quite a few .lib files that match the QFP44 criteria but all of them differ in some way or the other. That is why I am specifically looking for a 44pin TQFP package for PIC18f452. Regards, Leo --- Harry Selfridge [EMAIL PROTECTED] wrote: You must have missed the QFP44 footprint that is included in the Protel98 default library. If it doesn't suit you, you have two more options: 1. Use the library editor to make a footprint - it will take you less than 10 minutes; or 2. Use the library editor to edit the QFP44 footprint to your liking. At 02:40 AM 1/17/2005, you wrote: Dear Sir/madam, I am currently using Protel98 for my schematic and PCB development. I am in need for a 44pin TQFP PCB footprint for the PIC18f452(Microchip) SMD chip. Kindly mail me the the PCB footprint if possible or guide me where I can find one. Kind Regards Leo snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com = -- I'm not miles away, Just a [EMAIL PROTECTED] away! Leo Jose [EMAIL PROTECTED] -- __ Do you Yahoo!? All your favorites on one personal page Try My Yahoo! http://my.yahoo.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 44L-TQFP PCB footprint
You must have missed the QFP44 footprint that is included in the Protel98 default library. If it doesn't suit you, you have two more options: 1. Use the library editor to make a footprint - it will take you less than 10 minutes; or 2. Use the library editor to edit the QFP44 footprint to your liking. At 02:40 AM 1/17/2005, you wrote: Dear Sir/madam, I am currently using Protel98 for my schematic and PCB development. I am in need for a 44pin TQFP PCB footprint for the PIC18f452(Microchip) SMD chip. Kindly mail me the the PCB footprint if possible or guide me where I can find one. Kind Regards Leo snip You are subscribed to the PEDA discussion forum To Post messages: mailto:PEDA@techservinc.com Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Cannot locate server initialization file:, Answer2053
For crying out loud people! Give it a rest. I just ran the system year out to 2040 for a quick test, and the Protel99SE software starts and runs just fine. I don't have the time to do a year-by-year test, but it isn't rocket science. I might add that a well known email program crashed with the 2040 date, and a couple of other business programs wouldn't start - but the Protel software fired right up. I've run Protel software since the DOS days, and I've had every version they've published - including beta versions. NONE have ever had a time bomb. IF there is a date that the software doesn't work, I'm very sure that it will be found to be Microsoft related, and not Protel related. If there are people running cracked copies of the time limited demo software - there might be an issue that stops them at some time in the future. I haven't bothered to see how the time limited code checks dates. I also have no sympathy for them if the crack fails and the software locks them out - perhaps they should get lawyers... At 11:06 AM 12/3/04, you wrote: [EMAIL PROTECTED] wrote: Don't get your proverbial panties in a twist, boys... If 2005 (as suggested below) is not a tested, confirmed cutoff date for Protel, my suggestion is this: Perform a date test yourself. The fact is, if Altium has placed a time bomb in the software, so that it will not run at some reasonable time in the near future, it is interstate fraud, and quite prosecutable. I would hope we (99 users) don't have to band together and hire a lawyer, but that is a possibility. So, has anyone done a date test to find out when D-day is? Jon snip You are subscribed to the PEDA discussion forum To Post messages: mailto:[EMAIL PROTECTED] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] 99SE on Windows XP Pro
I wouldn't calll it insight, but it runs on XP Pro SP2 just fine here. At 09:30 AM 11/19/04, you wrote: I know Protel does not like Windows XP, but has/is anybody running it on XP Pro? Not sure if I should setup Pro on my machine or re-install Windows 2000. Thanks for any insight! Dale snip You are subscribed to the PEDA discussion forum To Post messages: mailto:[EMAIL PROTECTED] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/proteledaforum@techservinc.com Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/peda@techservinc.com
Re: [PEDA] Reading gerbers with Camtastic
Which version of Camtastic - the one that came with 99SE or the one that is integrated into DXP2004? With the older version of Camtastic, I think I remember that the software expected the kind of files generated by Protel. Although the article applies to importing Gerbers into the PCB editor, I believe the information in the following applied also to the older version of Camtastic: http://www.altium.com/protel/kb/kb_item.asp?ID=2215 In general, Protel software doesn't like to import files with negative coordinates. If your Gerbtool files have a center reference, there are negative coordinates in the generated files. You should relocate the reference point such that all data has positive (x,y) coordinates. What kind of Gerber file - RS274 or RS274X? If they are RS274 format, remember you will also have to load the apertures before loading the Gerber files. At 07:44 AM 10/15/04, you wrote: Does anybody know why Camtastic will not import gerbers generated from Gerbtool? When I import, It just give a blank screen. No error message, nothing. Does Camtastic only read Protel and it's own generated gerbers? Thanks for any help. Dale SNIP You are subscribed to the PEDA discussion forum To Post messages: mailto:[EMAIL PROTECTED] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search previous postings: http://www.mail-archive.com/[EMAIL PROTECTED]
