[PEDA] On the SCH but not on the PCB
Hello all, I was wondering how I would go about placing a part on the schematic but not have it appear on the PCB. For example, I would have 3 resistors in parallel labeled 100, 200, 300 and I would only want one of those three to appear on the PCB when I updated it. Is there a way to set if a part is to appear on the PCB or is that not possible? Afshin Salehi DPS Telecom * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] On the SCH but not on the PCB
When using the update pcb command from the schematic choose to preview changes then remove the resistors you don't want from the change list. But you might have to create a rule for the missing resistors. Brad Jaurique Pelco Clovis, ca -Original Message- From: Afshin Salehi [mailto:[EMAIL PROTECTED]] Sent: Thursday, January 17, 2002 10:36 AM To: Protel Forum Subject: [PEDA] On the SCH but not on the PCB Hello all, I was wondering how I would go about placing a part on the schematic but not have it appear on the PCB. For example, I would have 3 resistors in parallel labeled 100, 200, 300 and I would only want one of those three to appear on the PCB when I updated it. Is there a way to set if a part is to appear on the PCB or is that not possible? Afshin Salehi DPS Telecom * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] On the SCH but not on the PCB
At 10:47 AM 1/17/2002 -0800, Jaurique, Brad wrote: When using the update pcb command from the schematic choose to preview changes then remove the resistors you don't want from the change list. This would work, but is unnecessarily cumbersome. One could accomplish the same thing by deleting the resistors after they were loaded. In another post, however, I suggested assigning a non-existent footprint with a name that made it clear that the error was intentional. This would be self-maintaining. But you might have to create a rule for the missing resistors. No rule is necessary for missing parts. Net information is carried in two places in the Protel database, if I am correct. One place is a list of nets, which does not contain assigned pins; the other is the net field in the primitive records. Unlike Tango, Protel does not create dummy pads for unplaced components. If a component is not loaded because the footprint does not exist, the pad simply does not exist. This is an important point: DRC will *not* inform you about missing components, that is, components on the schematic that are not on the PCB, either because load failed or was interrupted, or because the component was later deleted. If it is deleted, it's gone, except, of course, for the undo buffer. So it is highly advised to *always* update PCB from schematic before releasing a board, to verify that no macros are created, or that any macros which are created are intentional deviations between schematic and PCB. [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] On the SCH but not on the PCB
At 10:35 AM 1/17/2002 -0800, Afshin Salehi wrote: Hello all, I was wondering how I would go about placing a part on the schematic but not have it appear on the PCB. For example, I would have 3 resistors in parallel labeled 100, 200, 300 and I would only want one of those three to appear on the PCB when I updated it. Is there a way to set if a part is to appear on the PCB or is that not possible? If the footprint assigned to the part is one which does not exist in any library, such as DO_NOT_USE, then no part will be created in the PCB, and any nodes for that footprint will be ignored. You will get a macro error telling you that footprint DO_NOT_USE was not found, which you will immediately recognize as intentional You can thus control which of the three resistors is used by controlling footprint assignment. I would display the footprint fields, I think you can do that, on the schematic. [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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
