> -----Original Message----- > From: Aaron McFarland > Sent: Wednesday, April 10, 2002 1:59 PM > > I have a module within my PCB that I need to replicate two or four > times. So far I have been doing this by copying this module's footprint > layout into my PCB library and creating a new part... <snip>
(This reply is a copy of my post from 5/12/2001) The protel faq, http://groups.yahoo.com/group/protel-users/files/protelfaq.html, started & maintained by David Cary, has a section on this; search for "repetition" (it's under Layout). Also, the following is a post from June 4, 2000, from Pat Nystrom, which gives a good, detailed, procedure. [Mr. Cary -- how about adding this to the FAQ?] The particular method that would be best for you will depend on where you are in this process, how the schematic is arranged, whether or not you want to copy track layout, etc. Dwight (copy of)-----Original Message----- From: NCE Sent: Sunday, June 04, 2000 10:41 AM Subject: RE: [PROTEL EDA USERS]: PCB Step & Repeat In the following discussion, 'channel' means one section of duplicate circuitry. This process assumes you have a schematic for one channel entered, and also that each channel only occupies one schematic page. The method would have to be altered in the annotation phase if a channel occupies more than 1 page. 1. Annotate channel 1. The idea is to make this channel easy to duplicate with new designators on each channel, so a suffix is set on the parts. Go to the schematic page with channel 1. Choose Tools|Annotate, choose 'All Parts', 'Current Sheet Only', and in the 'Advanced Options' tab, put a check mark next the page number (there should be only one page there, as you've checked 'Current Sheet Only'). Enter '1' in the from column, and '999' in the to column. Put _1 in the suffix column, so channel 1 parts will take the form xxx_1. 2. Update the PCB with the new designators (Design|Update PCB). 3. Place channel 1 on the PCB, and route it (if you want to copy routing as well as placement). Now, for each new channel, do the following: 1. Make a new schematic page for the new channel. 2. Link it to the master sheet (place a sheet symbol with the correct filename). 3. Go to the page for channel 1. 4. Select all on the page (SA). 5. Copy to the clipboard (ctrl-C and choose a reference point). 6. Go to the new page and paste (ctrl-V and choose reference point). 7. Right click on any component on the new page and edit its properties. In the Designator field, change the '_1' to '_x' where x is the channel you're creating. Click 'global', and in the copy attributes field for Designator, type {_1=_x}, again where x is the new channel number. This will change all parts on the page to their correct designators. The root designator will remain the same, but the suffix will indicate the channel number. Now the schematic portion has been duplicated. 8. On the PCB, select all components for channel 1. An easy way to do this is to go to the schematic page for channel 1, hit 'SA' (Select All), and then 'TS' (Tools|Select PCB components). 9. Hit Ctrl-C (copy), and choose a reference point. 10. Choose 'Edit|Pase Special', and select 'Duplicate Designators'. Paste the channel 1 components into the location for the new channel. 11. You now have two groups of components selected, the original channel 1 and the new channel, with channel 1 designators. Deselect the original channel 1 components, leaving only the new channel's components selected. 12. Right click on any component in the new channel, and edit its designator suffix to match the new channel number, as was done on the schematic. Click Global, and set the copy attribute for Designator to {_1=_x} where x is the new channel number, and set the 'Selection' drop-down to 'same'. This will re-suffix all components in the new channel to match the schematic. 13. Finally, go back to the schematic and choose 'Design|Update PCB'. If you've copied routing information, make sure and check 'Assign Nets to Connected Copper'. You should have a matching schematic and PCB containing the new channel(s). Regards, Pat Nystrom > problem is that > when I copy the module's layout into the library all the part > designators are lost (because it is now considered a single part by > Protel). Is there an altogether easier way to replicate a module both > on the PCB and in the schematic? * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
