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, here's a post from June 4, 2000, from Pat Nystrom, which gives a detailed
procedure.
[Mr. Cary -- how about adding this to the FAQ?]
Note, Rimas, that 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 Harm
Trax Softworks, Inc.
-----Original Message-----
From: NCE
Sent: Sunday, June 04, 2000 10:41 AM
To: Multiple recipients of list proteledausers
Subject: RE: [PROTEL EDA USERS]: PCB Step & Repeat
OK, here it is again - new and improved, more reliable than the last
method I posted. I also posted this to protel-users-misc at egroups,
as suggested - although I don't believe it 'strays from the primary
purpose' of this group.
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
------------------------------
-----Original Message-----
From: Rimas Avizienis [mailto:[EMAIL PROTECTED]]
Sent: Friday, May 11, 2001 11:46 AM
Subject: [PEDA] replicating component placement ?
if i have a circuit replicated eight times in a design, is there an easy
way to do the layout for one circuit and then replicate the layout for the
others? i believe this question has been addressed on this list before but
i am uncertain as to the conclusion that was reached. being able to do
this in an automated fashion would save me QUITE a bit of time on a board
i'm currently working on.
thanks for any help,
-rimas
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
