Re: [PEDA] Synchronizer Mystery
Re: [PEDA] Synchronizer Mystery
At 11:30 PM 12/8/01 -0500, Darryl Newberry wrote: ... Macro 683: New Node Add node J9-10 to net CFD0 Macro 684: New Node Add node J9-10 to net NCFON_3P3V ... Macro 819: New Node Add node J3-10 to net QMUTE Macro 820: New Node Add node J3-10 to net BAT_POS ... Why is the synchronizer trying to attach the same pin to 2 different nets. Isn't this a netlist error by definition? There is nothing wrong with the schematic AFAICT--each pin has a single wire stub with the net label sitting on it. There is no obvious relationship between the pin and the 2nd net name. QMUTE and BAT_POS are single-node nets, whereas CFD0 and NCFON_3P3V each have multiple nodes. I don't know what is causing this, though I can list some suspicions. Most of them would be detected by ERC. (I advise setting the ERC matrix to detect every possible warning or error, but duplicate part checking is not matrixed, instead this error is hard-coded into ERC.) (1) as hinted, duplicate parts. (2) duplicate pins within a part, especially a hidden one which will create a net with its name. (3) bad schematic database. The first step is to run ERC. All ERC errors and warnings reported should be corrected or verified as spurious -- i.e., they should be thoroughly understood (such as being a deliberately open output) before being suppressed with No-ERC Directives. Ultimately, one wants a completely clean ERC report. This leads to another possibility: (4) A duplicate part error has been suppressed with a No-ERC Directive. The next step, if fixing errors has not corrected the problem, would be to generate a net list instead of running Update PCB. Verify that there are two occurrences of the pin names in the net list, which is what we expect to see from the reported symptoms. If there are not two names and the net list still generates the problem macros when loaded into the PCB, then we have a serious PCB problem. I will assume that this is not the case. Run the Schematic Cross-Reference Report. Look for two occurrences of the part in question. But the following procedure may be more comprehensive. With all sheets of the schematic open, set the Panel Browse for Primitives/Pins. Check All in Hierarchy and press Update List. Look for two occurrences of the pins in question. If they are there, you can read the pin locations and you can jump to them. It this does not uncover the problem, attempt to pare down the schematic to a minimum file that still shows a duplicate pin. As part of this process, you should be able to remove any confidential information. Then, I would be interested in seeing the file; also, if we cannot find the problem, it should be submitted to ProtelCSC. But let us have a crack at it first. [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Synchronizer Mystery
With all sheets of the schematic open, set the Panel Browse for Primitives/Pins. Check All in Hierarchy and press Update List. Look for two occurrences of the pins in question. Found it right away using the above approach. Duplicate pin numbers in the part. DOH! The pin numbers were hidden but the pin names (same as pin numbers) were not. Would be nice to have a pin number cross-check when creating the part. Thanks to all who replied so quickly. This list is truly value added! Darryl Newberry Freedom Scientific 2850 SE Market Pl Stuart FL 34997 (561) 223-6443 tel (561) 223-6413 fax http://www.freedomscientific.com All information contained or disclosed herein is proprietary and confidential to Freedom Scientific. Opinions expressed by the sender do not necessarily reflect Freedom Scientific corporate policy. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Synchronizer Mystery
Found it right away using the above approach. Duplicate pin numbers in the part. DOH! The pin numbers were hidden but the pin names (same as pin numbers) were not. Would be nice to have a pin number cross-check when creating the part. Darryl: There is a component rule check under Reports when you are creating components. It will tell you if you have duplicate pins and pins missing in sequence as well as other things. There is a bug in the duplicate pin reporting however, only one error is reported when there are multiple duplicates. Brock * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Starting out with Protel99, Questions
Howdy, 1) Is there a standard or rule of thub that can be applied to the seperation for a split plane ? I use a 50mil separation everywhere I can unless there are rails over +/-12. If the difference in voltage of the split planes next to each other is over 25V I try to use a separation of 100mils. This is an imperical method and may not be practical in all applications. 2) For plated pads and vias, is hole size in layout before or after plating. ie if i set hole size to be 50mil, will it compensate for fact hole will be plated and compensate drill size so hole is 50mil after plating? It can. I specify Finished Hole Size in the drill chart on the fab drawing, and I have never had any problems from doing so. If memory serves, the Copper Connection advises against against what I just wrote. 3) Is there a standard or rule of thumb for dimensions of pad in relation to hole size ? From most of the library components I looked at, it seems hole is about 2/3 pad size. I use a pad 20mil over drill (10mil annular) for pins unless otherwise specified or impractical. 4) Is there a standard via size/sizes ? I use an 11mil drill and a 25mil pad due to the board houses my customers use. When I need to get a 5mil trace between the pads of a fine pitch BGA, I use a 24mil pad. 5) For a given size diameter component lead is there a guidline for hole size ? For round leads, I like to use 10mil hole over the lead size. 6) for a component with square pins, .025mil (+- .005) mil on a side, I was going to use pads of diameter 80, hole 52. This sound reasonable. For square leads, I like to use 5 over diagonal. Pythagorean's theorum is a^2 + b^2 = c^2. |\ a| \ | \c | \ - b To find the diagonal of a right triangle, c = square root of (a^2 + b^2). 7) For a thick track, say 30mil to 50mil, is it normal to use multple small vias ? Absolutely. I prefer to use multiple small vias rather than one large via for most designs. Any other pointers welcome. Any help greatly appreciated. To save my customer money in the fabrication of the board, I will combine hole sizes within 2mils of each other, except for press-fit or other critical applications. The aspect ratio of drill hole to board thickness is a very important issue and can greatly affect the cost of the design. A hole size that is ten times smaller than the thickness of the board may affect the cost of the board more than any benefits gained. Try to stay at or under 8:1. Cheers! Drew * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Sch part pins (was Using Multiple Vcc for same part)
There is another matter I would also like to comment on concerning schematic components, to wit, being able to re-arrange pins (locations and orientations) within components within schematic files (as opposed to schematic *library* files). Regards, Geoff Harland. Yes, this would be a great help. A bit of thought would have to go into the technicalities of updating parts from the SCH library (do the pins revert to default positions etc) and what happens if a part is deleted and replaced with the same part with a different default pin arrangement from a different library resulting in incorrect connections. IMO the benefits would far outweigh the dangers. If they fix the library linking problems in the next version everything would be a lot safer. Michael Beavis * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] HI Again...
Warning Unable to process data: multipart/mixed;boundary==_NextPart_000_0003_01C180F1.25E7B3A0
[PEDA] RV: HI Again...
SORRY, THIS IS THE ADDRESS FOR THE DATASHEET: http://usuarios.arnet.com.ar/mendezmh/redcc.jpgis a picture -Mensaje original- De: Mariano Méndez [mailto:[EMAIL PROTECTED]] Enviado el: Domingo, 09 de Diciembre de 2001 08:36 p.m. Para: 'Protel EDA Forum' Asunto: HI Again... Here I'm sending to you the datasheet of my display. This is the display that i want to create the footprint, can someone help me?? Thank you all again... YOURS... Mariano H. Méndez * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] Now see what you did ! ! !
Re: [PEDA] Now see what you did ! ! !
Re: [PEDA] RV: HI Again...
You should be able to layout that part pretty easily. We cannot do it for you because there isn't any pinout info in that drawing. Just the mechanical stuff. It's only 10 pads plus the outline, right? Tony -Original Message- From: Mariano M ndez [mailto:[EMAIL PROTECTED]] Sent: Sunday, December 09, 2001 3:45 PM To: 'Protel EDA Forum' Subject: [PEDA] RV: HI Again... SORRY, THIS IS THE ADDRESS FOR THE DATASHEET: http://usuarios.arnet.com.ar/mendezmh/redcc.jpgis a picture -Mensaje original- De: Mariano M ndez [mailto:[EMAIL PROTECTED]] Enviado el: Domingo, 09 de Diciembre de 2001 08:36 p.m. Para: 'Protel EDA Forum' Asunto: HI Again... Here I'm sending to you the datasheet of my display. This is the display that i want to create the footprint, can someone help me?? Thank you all again... YOURS... Mariano H. M ndez * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Now see what you did ! ! !
They have just come but online. They have been up and down over the last couple of days. There was a message: --- Under Construction The site you were trying to reach does not currently have a default page. It may be in the process of being upgraded. --- Please try this site again later. If you still experience the problem, try contacting the Web site administrator. --- Regards, Darren Moore -Original Message- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]] Sent: Monday, 10 December 2001 11:26 To: Protel EDA Forum Subject: Re: [PEDA] Now see what you did ! ! ! In a message dated 12/9/2001 7:22:43 PM Eastern Standard Time, [EMAIL PROTECTED] writes: You have been talking too much about how Protel is trying to rip us off by abandoning support for their established customers unless we pay an exorbitant ransom (Altium Total Support), and now you have freaked out the Altium Lawyers so much they took down the www.protel.com website (it has been missing in action every time I have tried it today (Sunday)). Better check your browser. I just looked at both Protel.com and .au, and they're both up. My browser sometimes gets stuck like that; perhaps yours has a similar problem. Steve Hendrix * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] PCB Move-Component selection filter doesn't stick
When I tried the M-C command and click on a blank area of the PCB, it brings up a handy dialog box allowing me to choose from a list of components placed on the board. I want to just see the resistors, so I enter R* for the filter and it works as expected. The problem is when I want to do this AGAIN, the R* reverts back to * which causes all components to show up again. I have to type R* AGAIN and AGAIN. I think to make this more useful, the filter should persist between access to this dialog. Does anyone else disagree?? Tony * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] AW: CAMTASTIC GERBER TO PROTEL TRANSLATOR?
At 08:04 AM 12/5/01 +0100, Georg Beckmann wrote: I sent it to Abdulrahman Lomax he wanted to bring it to the file section in this forum. But anyway, I send it to your e-mail address. I have zipped and uploaded Mr. Beckmann's utility to the filespace for [EMAIL PROTECTED] I have not tested this utility. http://groups.yahoo.com/group/protel-users/files/Protlgbr.zip [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Now see what you did ! ! !
Steve, I actually had tried several times using two different systems and ISP's (earthlink.net and sbcglobal.net), before I posted to the list, but no sooner than I posted it was back up. May be some routing or other problems involved with the various services due to the time of year and heavy volume of online shopping over the weekend. They do appear to be back on line, but I am still having some real problems accessing their site, especially the knowledge base. Notwithstanding, I think my post makes some valid points and is foder for further discussion. JaMi - Original Message - From: [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Sunday, December 09, 2001 4:26 PM Subject: Re: [PEDA] Now see what you did ! ! ! In a message dated 12/9/2001 7:22:43 PM Eastern Standard Time, [EMAIL PROTECTED] writes: You have been talking too much about how Protel is trying to rip us off by abandoning support for their established customers unless we pay an exorbitant ransom (Altium Total Support), and now you have freaked out the Altium Lawyers so much they took down the www.protel.com website (it has been missing in action every time I have tried it today (Sunday)). Better check your browser. I just looked at both Protel.com and .au, and they're both up. My browser sometimes gets stuck like that; perhaps yours has a similar problem. Steve Hendrix * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Now see what you did ! ! !
It's probably the new screen saver email virus circulating through their server. I've seen other site go up down through the past few days. Brian Guralnick - Original Message - From: Darren Moore [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Sunday, December 09, 2001 7:39 PM Subject: Re: [PEDA] Now see what you did ! ! ! | They have just come but online. They have been up and | down over the last couple of days. | | There was a message: | --- | Under Construction | The site you were trying to reach does not currently have | a default page. It may be in the process of being upgraded. | --- | Please try this site again later. If you still experience | the problem, try contacting the Web site administrator. | --- | | Regards, | Darren Moore | | | -Original Message- | From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]] | Sent: Monday, 10 December 2001 11:26 | To: Protel EDA Forum | Subject: Re: [PEDA] Now see what you did ! ! ! | | | In a message dated 12/9/2001 7:22:43 PM Eastern Standard Time, | [EMAIL PROTECTED] writes: | | | You have been talking too much about how Protel is trying to rip us | off by | abandoning support for their established customers unless we pay an | exorbitant ransom (Altium Total Support), and now you have | freaked out the | Altium Lawyers so much they took down the www.protel.com | website (it has | been missing in action every time I have tried it today (Sunday)). | | | Better check your browser. I just looked at both Protel.com | and .au, and | they're both up. My browser sometimes gets stuck like that; | perhaps yours has | a similar problem. | | Steve Hendrix | | | | * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] ATS and ALU share price
At 09:26 AM 12/5/01 +0100, Edi Im Hof wrote: I heard a _rumor_, the sales has dropped noticable after the price increase last summer. Not everybody at Altium is pleased with this strategy. I don't know how sales have been going, but I'd think there would be a third quarter report out there Raising the price of a software package by 33% without introducing new features or other improvements is a bit dicey. It's not as if their cost per unit had gone up! If they had released the autorouter, they might have pulled it off. But they didn't. [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] RV: HI Again...
It is very easy to create a footprint for this part using the Protel PCB component wizard. As a test, I just created one for this part in less than ten seconds! Open up an existing PCB library database for editing or create a new one in your current database (File New... then select PCB Library Document from the icons) Select Tools New Component The first page of the component wizard will appear. Click on Next Select Dual Inline Package (DIP) and Imperial units. Click on Next. Edit the labels for the pad dimensions to be appropriate for the component leads (e.g. 25 mil hole in a 60 mil round pad for all three layers of the pad stack. Click Next. Edit the labels for the pad spacings (100 mils between pads and 600 mils between pad columns). Click Next. Accept the default silkscreen width of 10 mils by clicking on Next. Edit the total number of pads to be 10. Click Next. Enter the name of the footprint. Click Next. Click Finish. Verify that the footprint is correct. You are done! (don't forget to save the modified library) John Williams Mariano M ndez wrote: SORRY, THIS IS THE ADDRESS FOR THE DATASHEET: http://usuarios.arnet.com.ar/mendezmh/redcc.jpgis a picture -Mensaje original- De: Mariano M ndez [mailto:[EMAIL PROTECTED]] Enviado el: Domingo, 09 de Diciembre de 2001 08:36 p.m. Para: 'Protel EDA Forum' Asunto: HI Again... Here I'm sending to you the datasheet of my display. This is the display that i want to create the footprint, can someone help me?? Thank you all again... YOURS... Mariano H. M ndez * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SPs for earlier versions (ex Altium Total Support Brochure)
It's an old saying that monopolies don't have to apologise to their customers. However, when competition does exist, it is a bad move to alienate your customers, and when competition doesn't exist (or is weak), bad attitudes can result in customers taking their complaints to a regulatory agency. And some times, in some places, these agencies kick a*** And some times, in some places, these agencies kiss a**. I am referring to U.S. Dept. of Justice vs. Microsoft, of course. And some times, in some places, the agencies kick a**, but the enforcee has their a** covered with titanium/kevlar armor with case-hardened steel spikes. I am referring to the U.S. vs. Exxon Valdez case where the big punitive fine was overtuned on appeal. How much taxpayer money did the U.S. gov't waste letting that one get overturned? What's this got to do with Protel? We should not rely solely on law or threat of law enforcement to get what is fair. As time goes on, governments everywhere are becoming more and more hijacked by big business special interests. We users need to do what we can to protect ourselves from unfair practices, because government action is always slow, expensive, and unreliable. Yes, there is a lot to be said for turning to the government as a last resort, rather than in the first instance. And I would concur that the phenonomen of governments being hijacked by vested interests is not confined to the USA. I lived in New Zealand up until a bit less than three years ago, but I have still been keeping up with much of what has been happening there. Just during the weekend just passed, I think I finally figured out why one organisation there has been so keen to dump a certain service (which is not profitable, but probably would be, had it been promoted with that objective in mind). If my hunch is correct, taxpayers have the potential to be considerably out of pocket, which is all the more insulting given that two of its current major shareholders are renown for regarding their fiscal obligations as being voluntary in nature. That corporation hires the services of a certain spin-doctor, who just happens to also provide such services for the current leader of the Opposition. (And his political party is chaired by yet another spin-doctor, whose actions while working for those two parasites were regarded as so reprehensible by the professional body for the PR business that she was officially censured by this (not that that seems to have had a detrimental impact upon her employability).) If my hunch is correct, there are detrimental implications for the region which that individual represents (and regardless of whether taxpayers in general end up out of pocket or otherwise). However, he has previously/already made it clear that he is untroubled by such considerations, or at the very least is happy to cut off his nose to spite his face. That means demanding that software work properly, service packs remain available, and seriously considering alternatives where they exist. Supporting each other when the software vendor ceases support. And making sure the software vendor knows what we think! Ivan Baggett Agreed, and some. Given that a SP is no use by itself (i.e. without a copy of the software for which it is a SP), I don't see any reason why Protel users can't provide these to one another, or at least whenever these cannot be downloaded from Protel's website (or otherwise acquired from Altium). Even though Altium presumably would prefer that users update to the current version of Protel, the older versions don't have an expiry date, so anyone who wants/prefers/needs to continue to use these should be able to do so with whichever SPs were released for them. (I did in fact send a copy of SP1 for Client3 myself, but my associated email message was not delivered because the attached file was executable in nature; before I got around to resending that file enclosed within a Zip file, someone else did so instead.) It will be interesting to see whether Phoenix (the next major version of Protel) adds a (Boolean) Mirrored field for Component objects (in PCB files). Personally, I am not enamoured to the alternative scenario of not being able to mirror components at all, but time will tell what happens in that regard (with the other possible scenario being to continue to warn users whenever components are about to be mirrored, as has been provided by SP6 for Protel 99 SE). My vision is that if components still can be mirrored, and a Mirrored field is provided, than users will be warned, prior to the generation of Gerber files, if any of the components in the PCB file are detected as being in a mirrored state at the time. Users would also have the capability of being able to produce a report, at any time, as to which components are currently mirrored. The alternative scenario would be to prohibit mirroring of components altogether, but that would mean that the use of the X or Y key would
Re: [PEDA] PCB Move-Component selection filter doesn't stick
Yeah that's great and would fit in just fine with what I requested. If the field is maintained between accesses to that dialog, it would do what I want, and in your case the user would have to change the R* to a C* anyway, so there is no difference to them. If they want to randomly pick various part types, just leave it as *. Late for Phoenix? They haven't even started beta testing. I think a little change like this would take a programmer 10 minutes. At least that's how fast my programmers change little features! :) Tony -Original Message- From: Geoff Harland [mailto:[EMAIL PROTECTED]] Sent: Sunday, December 09, 2001 5:41 PM To: Protel EDA Forum Subject: Re: [PEDA] PCB Move-Component selection filter doesn't stick When I tried the M-C command and click on a blank area of the PCB, it brings up a handy dialog box allowing me to choose from a list of components placed on the board. I want to just see the resistors, so I enter R* for the filter and it works as expected. The problem is when I want to do this AGAIN, the R* reverts back to * which causes all components to show up again. I have to type R* AGAIN and AGAIN. I think to make this more useful, the filter should persist between access to this dialog. Does anyone else disagree?? Tony There could be times when the user wants to select a resistor (say) on one occasion, then a capacitor (say) on the next occasion. As such, I would see merit in providing an user-selectable setting so that either the current behaviour or the requested behaviour could be selected (as desired). And given that the provision of such a feature *shouldn't* be too difficult to implement (either in the originally requested form or in the more refined form which I suggested above), I would not oppose it on the grounds of it being a relatively frivolous request (which could divert Altium's programmers from providing fixes or enhancements of a more important nature). I suspect it would be a bit late in the piece to incorporate within Phoenix, or at least in the initial version of this. But perhaps it could be incorporated in a followup SP (depending upon whether or not it would have a significant impact upon the database structure of PCB files or system settings)... Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] PCB Move-Component selection filter doesn't stick
Yeah that's great and would fit in just fine with what I requested. If the field is maintained between accesses to that dialog, it would do what I want, and in your case the user would have to change the R* to a C* anyway, so there is no difference to them. If they want to randomly pick various part types, just leave it as *. Late for Phoenix? They haven't even started beta testing. I think a little change like this would take a programmer 10 minutes. At least that's how fast my programmers change little features! :) Tony The code itself shouldn't take too long, but there could be database implications; if so, it could be far less straightforward to add this feature. I haven't been asked to be a beta tester for Phoenix (or at least not yet), but that doesn't mean to say that nobody else has been approached in this regard. So for all I know, there could be other users beta testing this already Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] PCB Move-Component selection filter doesn't stick
I have vague recollection about some of us being asked to participate and I know *I* haven't started yet. I hope they are serious about testing or are planning to slip the release date. Tony -Original Message- From: Geoff Harland [mailto:[EMAIL PROTECTED]] Sent: Sunday, December 09, 2001 6:54 PM To: Protel EDA Forum Subject: Re: [PEDA] PCB Move-Component selection filter doesn't stick Yeah that's great and would fit in just fine with what I requested. If the field is maintained between accesses to that dialog, it would do what I want, and in your case the user would have to change the R* to a C* anyway, so there is no difference to them. If they want to randomly pick various part types, just leave it as *. Late for Phoenix? They haven't even started beta testing. I think a little change like this would take a programmer 10 minutes. At least that's how fast my programmers change little features! :) Tony The code itself shouldn't take too long, but there could be database implications; if so, it could be far less straightforward to add this feature. I haven't been asked to be a beta tester for Phoenix (or at least not yet), but that doesn't mean to say that nobody else has been approached in this regard. So for all I know, there could be other users beta testing this already Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Beta testing (ex PCB Move-Component selection filter doesn't stick)
I have vague recollection about some of us being asked to participate and I know *I* haven't started yet. I hope they are serious about testing or are planning to slip the release date. Tony The websites for Protel and PCAD invite their visitors to apply to become beta testers for Altium products (which I have done). ISTR that a message was also posted to the Protel and PCAD mailing lists advising users to apply to become a beta tester (if they thought they were suitable for that task). However, other postings to this forum suggest that being accepted as a beta tester doesn't imply that such users will necessarily be asked to test *all* releases of beta software. The last I heard, Phoenix is supposed to be released during Q1/2002. As such, it could be released as late as late March next year without slipping from that schedule. If nobody is beta testing as of yet, that suggests a reasonably tight schedule, but for all I know, there could be some users beta testing already (possibly with NDAs requiring them to refrain from disclosing that they actually are beta testers). It could be argued as to how long is suitable for beta testing. A long test period *should* result in more bugs being found (hopefully all of them), but the counter argument is to ship product ASAP. As I suspect that some bugs will in fact slip through (regardless of how long the beta testing period is), what will be at least as critical is how long it will take to release followup SPs (and how many of these there will be)... Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
