Re: [PEDA] 99SE: 2 of every net name?
> I had that one once too. > It turned out to be a not-so-obvious typo in the net and port names that > prevented P99 top correctly link the nets up. That still happens to me once in awhile. 1 thing I still wish for is a font which better visually defines the difference between 0 & O. Like the old days of the zero with the slash through it. _ Brian Guralnick - Original Message - From: "Leo Potjewijd" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Thursday, March 18, 2004 4:42 AM Subject: Re: [PEDA] 99SE: 2 of every net name? > At 18-03-2004 07:26, Laurie Biddulph wrote: > >I have found this to be caused by the fact that my schematics do not > >correctly link the nets across multiple pages. Check if your scope is set > >to Ports & Net Labels and/or make sure your nets are clearly marked on all > >relevant pages. The overall block diagram using sheets is useful here as well. > > I had that one once too. > It turned out to be a not-so-obvious typo in the net and port names that > prevented P99 top correctly link the nets up. > Found it by checking the 'add sheetnumber to local nets' checkbox in the > synchronizer > > > Leo Potjewijd > hardware designer > Integrated Engineering B.V. > > [EMAIL PROTECTED] > +31 20 4620700 > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
At 18-03-2004 07:26, Laurie Biddulph wrote: I have found this to be caused by the fact that my schematics do not correctly link the nets across multiple pages. Check if your scope is set to Ports & Net Labels and/or make sure your nets are clearly marked on all relevant pages. The overall block diagram using sheets is useful here as well. I had that one once too. It turned out to be a not-so-obvious typo in the net and port names that prevented P99 top correctly link the nets up. Found it by checking the 'add sheetnumber to local nets' checkbox in the synchronizer Leo Potjewijd hardware designer Integrated Engineering B.V. [EMAIL PROTECTED] +31 20 4620700 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
I have found this to be caused by the fact that my schematics do not correctly link the nets across multiple pages. Check if your scope is set to Ports & Net Labels and/or make sure your nets are clearly marked on all relevant pages. The overall block diagram using sheets is useful here as well. Best Regards Laurie Biddulph http://www.elby-designs.com - Original Message - From: Ray Mitchell To: [EMAIL PROTECTED] Sent: Thursday, March 18, 2004 8:58 AM Subject: [PEDA] 99SE: 2 of every net name? I've never seen this before. In 99SE (Win2K) I've created a schematic and am starting the PCB layout. When I double-click on a pad and look at the net attached to it, as well as all the available nets, I noticed that there are two of every net. For example, there are 2 A5 nets. Some of the A5 pads are connected to one of these nets while others are connected to the other, even though they all have the same A5 name. My manually going through all the pads and selecting, for example, the first A5 of the pair I can get all A5 pads to connect together, etc. Any ideas? Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
Ray Very simply put there is a bug in the netlist load routing with Protel. The netlist load works fine on the first load, subsequent loads will yeild varied and unpredictable results. If you wish an error free board 100 percent of the time you must >>1. 1. Clear all nets, 2 Load the netlist 3 Connect copper to pads 4. Run DRCs Repetitive netlist loads can yeild double net problems like you are seeing ( providing your the problem is not in your schematic driven netlist). Go to Design, and look at the menus under netlist manager Mike Reagan -- Original Message -- From: Ray Mitchell <[EMAIL PROTECTED]> Reply-To: "Protel EDA Forum" <[EMAIL PROTECTED]> Date: Wed, 17 Mar 2004 16:32:47 -0800 >Mike, > >I don't understand what I need to do to clear all nets. I told it to >un-route (although nothing had been routed). From within the PCB editor I >then told it to load all nets. It indicated that there were many redundant >nets. I told it to execute and it proceeded to remove all nets and all >parts. It's a good thing that the UNDO works! I've placed many of my >components already. Does this mean I must redo all of that? If anyone can >tell me the format of the offending portion of the .DDB file I'm not >adverse to using a binary editor on it. This approach is probably way too >complex for the average person, though, since it's obviously too complex >for the Protel developers themselves. > >Thanks, >Ray > >At 05:29 PM 3/17/2004 -0500, you wrote: >>Ray, >> >>If the problem is not in your netlist meaning nets A5 are not showing up >>twice: >>you must do this to avoid double nets in PCB >> >>1. Clear all nets, >>2 Load the netlist >>3 Connect copper to pads >>4. Run DRCs >> >>I am saddened to report this problem still exist in 2004 >> >>Mike Reagan >> >> >> >>-Original Message- >>From: Ray Mitchell [mailto:[EMAIL PROTECTED] >>Sent: Wednesday, March 17, 2004 4:58 PM >>To: [EMAIL PROTECTED] >>Subject: [PEDA] 99SE: 2 of every net name? >> >> >>I've never seen this before. In 99SE (Win2K) I've created a schematic and >>am starting the PCB layout. When I double-click on a pad and look at the >>net attached to it, as well as all the available nets, I noticed that there >>are two of every net. For example, there are 2 A5 nets. Some of the A5 >>pads are connected to one of these nets while others are connected to the >>other, even though they all have the same A5 name. My manually going >>through all the pads and selecting, for example, the first A5 of the pair I >>can get all A5 pads to connect together, etc. Any ideas? >> >>Ray Mitchell >>Engineer, Code 2732 >>SPAWAR Systems Center >>San Diego, CA. 92152 >>(619)553-5344 >>[EMAIL PROTECTED] >> >>* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * >>* 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/[EMAIL PROTECTED] >>* * * * * * * * * * * * * * * * * * * * * * * * * * * * * >> >> > >Ray Mitchell >Engineer, Code 2732 >SPAWAR Systems Center >San Diego, CA. 92152 >(619)553-5344 >[EMAIL PROTECTED] > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
That did it! Thanks for all the help. Ray At 11:44 AM 3/18/2004 +1100, you wrote: Ray, The Menu Design, Netlist Manager, then right click and select clear all nets. No, you don't need to remove any components. There is nothing you can do in the ddb file. Darren Moore > -Original Message- > From: Ray Mitchell [mailto:[EMAIL PROTECTED] > > Mike, > > I don't understand what I need to do to clear all nets. I told it to > un-route (although nothing had been routed). From within the > PCB editor I > then told it to load all nets. It indicated that there were > many redundant > nets. I told it to execute and it proceeded to remove all > nets and all > parts. It's a good thing that the UNDO works! I've placed > many of my > components already. Does this mean I must redo all of that? > If anyone can > tell me the format of the offending portion of the .DDB file I'm not > adverse to using a binary editor on it. This approach is > probably way too > complex for the average person, though, since it's obviously > too complex > for the Protel developers themselves. > > Thanks, > Ray Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
I don't know how DXP does the "clear all Nets" command in the PCB editor, however, in 99SE, its under the main toolbar "DESIGN" menu, The "Load nets" which pops up the net list load dialog. Bottom left corner has "Advanced. Click that and you get taken to another dialog screen. At the bottom right, there is a button called "Menu". Click that and a drop down panel with several options appears, one of these is "Clear all nets" (or, chose "Netlist manager" from the "Design" main menu, and the Menu dialog button is the one on the bottom left. Again, chose "clears all nets". I suspect that when you then reload all the nets, components still on the sheet will remain connected. If you have any pre-routes already on the sheet, you will need to go through yet another step to get the PCB package to propagate the Net names to the track primitives . (I gratefully acknowledge that this was pointed out to just last week, in answer to my first question on this forum. Complements of Matt Van De Werken on this forum) Cheers Harry -Original Message- From: Ray Mitchell [mailto:[EMAIL PROTECTED] Sent: Thursday, March 18, 2004 11:33 AM To: Protel EDA Forum Subject: Re: [PEDA] 99SE: 2 of every net name? Mike, I don't understand what I need to do to clear all nets. I told it to un-route (although nothing had been routed). From within the PCB editor I then told it to load all nets. It indicated that there were many redundant nets. I told it to execute and it proceeded to remove all nets and all parts. It's a good thing that the UNDO works! I've placed many of my components already. Does this mean I must redo all of that? If anyone can tell me the format of the offending portion of the .DDB file I'm not adverse to using a binary editor on it. This approach is probably way too complex for the average person, though, since it's obviously too complex for the Protel developers themselves. Thanks, Ray At 05:29 PM 3/17/2004 -0500, you wrote: >Ray, > >If the problem is not in your netlist meaning nets A5 are not showing up >twice: >you must do this to avoid double nets in PCB > >1. Clear all nets, >2 Load the netlist >3 Connect copper to pads >4. Run DRCs > >I am saddened to report this problem still exist in 2004 > >Mike Reagan > > > >-----Original Message- >From: Ray Mitchell [mailto:[EMAIL PROTECTED] >Sent: Wednesday, March 17, 2004 4:58 PM >To: [EMAIL PROTECTED] >Subject: [PEDA] 99SE: 2 of every net name? > > >I've never seen this before. In 99SE (Win2K) I've created a schematic and >am starting the PCB layout. When I double-click on a pad and look at the >net attached to it, as well as all the available nets, I noticed that there >are two of every net. For example, there are 2 A5 nets. Some of the A5 >pads are connected to one of these nets while others are connected to the >other, even though they all have the same A5 name. My manually going >through all the pads and selecting, for example, the first A5 of the pair I >can get all A5 pads to connect together, etc. Any ideas? > >Ray Mitchell >Engineer, Code 2732 >SPAWAR Systems Center >San Diego, CA. 92152 >(619)553-5344 >[EMAIL PROTECTED] > >* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * >* 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/[EMAIL PROTECTED] >* * * * * * * * * * * * * * * * * * * * * * * * * * * * * > > Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
Mike, I don't understand what I need to do to clear all nets. I told it to un-route (although nothing had been routed). From within the PCB editor I then told it to load all nets. It indicated that there were many redundant nets. I told it to execute and it proceeded to remove all nets and all parts. It's a good thing that the UNDO works! I've placed many of my components already. Does this mean I must redo all of that? If anyone can tell me the format of the offending portion of the .DDB file I'm not adverse to using a binary editor on it. This approach is probably way too complex for the average person, though, since it's obviously too complex for the Protel developers themselves. Thanks, Ray At 05:29 PM 3/17/2004 -0500, you wrote: Ray, If the problem is not in your netlist meaning nets A5 are not showing up twice: you must do this to avoid double nets in PCB 1. Clear all nets, 2 Load the netlist 3 Connect copper to pads 4. Run DRCs I am saddened to report this problem still exist in 2004 Mike Reagan -Original Message- From: Ray Mitchell [mailto:[EMAIL PROTECTED] Sent: Wednesday, March 17, 2004 4:58 PM To: [EMAIL PROTECTED] Subject: [PEDA] 99SE: 2 of every net name? I've never seen this before. In 99SE (Win2K) I've created a schematic and am starting the PCB layout. When I double-click on a pad and look at the net attached to it, as well as all the available nets, I noticed that there are two of every net. For example, there are 2 A5 nets. Some of the A5 pads are connected to one of these nets while others are connected to the other, even though they all have the same A5 name. My manually going through all the pads and selecting, for example, the first A5 of the pair I can get all A5 pads to connect together, etc. Any ideas? Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
Ray Mitchell wrote: I've never seen this before. In 99SE (Win2K) I've created a schematic and am starting the PCB layout. When I double-click on a pad and look at the net attached to it, as well as all the available nets, I noticed that there are two of every net. For example, there are 2 A5 nets. Some of the A5 pads are connected to one of these nets while others are connected to the other, even though they all have the same A5 name. My manually going through all the pads and selecting, for example, the first A5 of the pair I can get all A5 pads to connect together, etc. Any ideas? Yup, this is the out-of-sync synchronizer bug. I think you want to clear the entire netlist in PCB, close all files and exit P99SE, and then re-open the DDB and files, and then try to sync again. The worst case is to clear the netlist, generate a Protel netlist in the SCH tools, and load the netlist. But clearing, closing and the re-syncing may put it all back to normal. Jon * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 99SE: 2 of every net name?
Ray, If the problem is not in your netlist meaning nets A5 are not showing up twice: you must do this to avoid double nets in PCB 1. Clear all nets, 2 Load the netlist 3 Connect copper to pads 4. Run DRCs I am saddened to report this problem still exist in 2004 Mike Reagan -Original Message- From: Ray Mitchell [mailto:[EMAIL PROTECTED] Sent: Wednesday, March 17, 2004 4:58 PM To: [EMAIL PROTECTED] Subject: [PEDA] 99SE: 2 of every net name? I've never seen this before. In 99SE (Win2K) I've created a schematic and am starting the PCB layout. When I double-click on a pad and look at the net attached to it, as well as all the available nets, I noticed that there are two of every net. For example, there are 2 A5 nets. Some of the A5 pads are connected to one of these nets while others are connected to the other, even though they all have the same A5 name. My manually going through all the pads and selecting, for example, the first A5 of the pair I can get all A5 pads to connect together, etc. Any ideas? Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] 99SE: 2 of every net name?
I've never seen this before. In 99SE (Win2K) I've created a schematic and am starting the PCB layout. When I double-click on a pad and look at the net attached to it, as well as all the available nets, I noticed that there are two of every net. For example, there are 2 A5 nets. Some of the A5 pads are connected to one of these nets while others are connected to the other, even though they all have the same A5 name. My manually going through all the pads and selecting, for example, the first A5 of the pair I can get all A5 pads to connect together, etc. Any ideas? Ray Mitchell Engineer, Code 2732 SPAWAR Systems Center San Diego, CA. 92152 (619)553-5344 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
