> -----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.


(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

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

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

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:
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to