Re: [PEDA] Netlist error?
This is a new one for me. I have a heiarchical design with 8 pages. Everything passes the ERC and from the observation, looks fine but when I try to generate a netlist it seems to not connect one page. Even the power ports on that one page create their own nodes. So if the rest of the design has a net called GND, this page also has a net called GND which should be connected to the other GND net, but isn't. I'm scratching my head on this one. I tried to rejoin the page on the project sheet by using the -Tools-Create symbol from Sheet. This was not successful. The really weird thing is that the power ports which should be global aren't being connected. Any suggestions?! Lloyd Good Engineering Systems Co-ordinator GE Harris Energy Control Systems Canada Inc. 2728 Hopewell Place NE Calgary, AB, Canada T1Y 7J7 * +1 (403) 214-4777 * +1 (403) 287-7946 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Netlist error?
Lloyd, This has happened to me before. It occurred when I deleted one page and renamed another (simplifying the design and reducing the number of pages). All I had to do was save the project, close it, close Protel. then re-open everything. The troublesome sheet may still not be linked to the hierarchy, but by deleting the sheet symbol and then recreating again should workIt did for me. Hope this helps, but it still does not answer the question of WHY? Lawrence Regnier High Density Design Inc. 280 Dougall Road North Kelowna, BC, Canada V1X 3K5 ph: (250) 470-1109 fax: (250) 765-5817 email: [EMAIL PROTECTED] web: http://www.highdensitydesign.net - Original Message - From: [EMAIL PROTECTED] To: [EMAIL PROTECTED] Sent: Friday, May 04, 2001 3:19 PM Subject: Re: [PEDA] Netlist error? This is a new one for me. I have a heiarchical design with 8 pages. Everything passes the ERC and from the observation, looks fine but when I try to generate a netlist it seems to not connect one page. Even the power ports on that one page create their own nodes. So if the rest of the design has a net called GND, this page also has a net called GND which should be connected to the other GND net, but isn't. I'm scratching my head on this one. I tried to rejoin the page on the project sheet by using the -Tools-Create symbol from Sheet. This was not successful. The really weird thing is that the power ports which should be global aren't being connected. Any suggestions?! Lloyd Good Engineering Systems Co-ordinator GE Harris Energy Control Systems Canada Inc. 2728 Hopewell Place NE Calgary, AB, Canada T1Y 7J7 * +1 (403) 214-4777 * +1 (403) 287-7946 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Netlist error?
On Fri, 04 May 2001 15:57:07 -0700, Lawrence Regnier wrote: This has happened to me before. It occurred when I deleted one page and renamed another (simplifying the design and reducing the number of pages). All I had to do was save the project, close it, close Protel. then re-open everything. The troublesome sheet may still not be linked to the hierarchy, but by deleting the sheet symbol and then recreating again should workIt did for me. Hope this helps, but it still does not answer the question of WHY? Because the design manager didn't know what sheets were in the project after your changes? In the explorer bar did it show the all the sub-sheets as sub-sheets of the main project sheet? You need to right click and select refresh on the containing folder in the explorer bar - that causes it to re-scan the sheets and re-establish the hierarchy. I presume this happens automatically when a design database is loaded. You would think it would inspect the top sheet on netlist generation but I suspect it doesn't. I know when you generate (an old style at least) BOM for a project the BOM gets the name of the active sheet not the top sheet of the project (annoying). Cheers, Terry. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Netlist error?
Thanks all for your input. What I serendipidiously discovered was many short fragments of wires scattered throughout this particular sheet which created junctions between nodes that shouldn't have been connected. I went through the hard copy to see what connections were valid and eliminated the wrong connections. Viola.fixed. Apparently Protels ERC checker did not pick up the multiple connections for what ever reason. I even made sure the multiple net name check was on. It may have to do with the sheet not having many net labels on the connectionsnot sure. Thanks again, Lloyd Good Engineering Systems Co-ordinator GE Harris Energy Control Systems Canada Inc. 2728 Hopewell Place NE Calgary, AB, Canada T1Y 7J7 * +1 (403) 214-4777 * +1 (403) 287-7946 -Original Message- From: Terry Harris [mailto:[EMAIL PROTECTED]] Sent: Monday, May 07, 2001 10:19 AM To: Protel EDA Forum Subject: Re: [PEDA] Netlist error? On Mon, 07 May 2001 11:08:40 -0400, you wrote: I cleaned up this schematic from another designer who didn't realize power ports were global, so he placed ports on all the sheets routing GND, VCC etc. Now that it's all cleaned up, I get this disjointed GND net. The VCC net seems to be connecting as do all the other netshuh? Ahh, that could be a tricky area - I seem to remember something about using port connections to isolate power nets between sheets. Like supplying static RAM with a battery backed VCC by placing it on a separate sheet and connecting power with ports. There may even be an example in the handbook or somewhere. I don't know exactly how it was supposed to work or if it is still supposed to work like that. Make double sure you don't have any GND ports left on the sheet (or sheet symbols). Cheers, Terry. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Netlist error?
project only the GND net. All the GND power ports are only connecting to each other on the one sheet, while all the others are creating a seperate GND net for the rest of the project. I have seen something like what I think you have described. There were two nets in the netlist with identical net names. Each contained a subset of the nodes that were to be connected to the net in the schematic. There was no overlap between the two nets. All nodes that were to be connected appeared in one of the two nets. I fixed some other unrelated(?) ERC and this situation disappeared. That is, the two nets became one that contained all the proper nodes. I did not investigate further since the deadline for several PCB's was imminent. Regards, Phil So The contents of this E-mail may contain information that is legally privileged and/or confidential to the named recipient. This information is not to be used by any other person and/or organisation. The views expressed in this document do not necessarily reflect those of the company. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
