Re: [PEDA] Panelise several designs
I am currently trying to create an A3 panel of 10 PCB designs I have created using Protel99SE. This saves cost by prototyping several PCB boards at once. When I try to copy and paste the PCB designs using Protel99SE the designs lose their connections to the Internal Plane (which I am using as a Ground Plane). Is there any way around this? (I did ask the PCB manufacturers to place these for me as they will have the correct tools but they refused as this design is a prototype only.) If anybody has any suggestions I would be very greatful to hear them. Kevin Blackmore From the PCB Menu, select Edit/Paste Special In the resulting Paste Special dialog box, check the checkboxes with captions of Keep net name and Duplicate designator. (The Add to component class checkbox will automatically be checked as well after doing this, and that is OK.) When you are subsequently asked if you want polygons to be repoured, answer No. Doing this should work, but check your Gerber files afterwards (which you should do in any case, even when you are not producing a panellised PCB). Camtastic can be used for this, but I am long accustomed to using GC-Prevue for this purpose (and this has the advantage of being *totally* independant of Altium/Protel). Let me know if you continue to have problems. 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] Panelise several designs
At 01:08 PM 7/09/01 +1200, you wrote: Hi I am currently trying to create an A3 panel of 10 PCB designs I have created using Protel99SE. This saves cost by prototyping several PCB boards at once. When I try to copy and paste the PCB designs using Protel99SE the designs lose their connections to the Internal Plane (which I am using as a Ground Plane). Yep - this will happen as when you copy and paste you do not bring over the design rules or the plane assignments. You may get a better result by taking one of the boards and using the Copy-As function to create a new PCB which will become the panelised PCB. This preserves the design rules and other stuff not copied by the Copy and Paste. But it doesn't help if the other boards in the set have wildly different design rules or layer stackup. The potential for incorrect rules causing problems with connections to internal planes is very real. You can export a set of rules from one of your designs (use the Menu button on the Design rules dialog) and then import this rule sset into all the other designs and re-run DRC and confirm that each design is OK. Then this same rule set can be used in the panelised board and you should/might/may be OK. Make sure in the new design the GND net is tied to the internal plane (Layer Stack manager), and you keep the nets (and allow duplicates) using the Paste Special command (rather than Paste) when you do the pastes. Is there any way around this? If all the boards are similar in construction it may be possible to do but is not for the faint-hearted (panelising the same PCB over and over is simpler). A detailed knowledge of the program and the PCBs and the manufacturing process is required. You could use Camtastic to do the panelising as this is the sort of thing it is good at. It deals with the Gerbers, so doesn't try to get too smart with rules and layer stack-ups. This is what I'd do, I think, even though I have been panelising in Protel for years. Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
