At 10:29 AM 2/12/01 -0500, Bryan Bernesi wrote:
>Also, each module has to be placed and wired the same way. No problem, or so
>I thought. I placed the components and wired the first module; ran the DRC
>no problems. I Copied it, and pasted it (using >>EDIT>>PASTE SPECIAL>>PASTE
>ARRAY), great.... no problems so far, once I had all 24 modules placed I ran
>a DRC again and I get clearance and short-circuit constraints. why????
I'm going to take the opportunity to ask writers to the list to do two things:
(1) Ask one question per post with an appropriate subject line. Yes. I
numbered it as one thing, but it really is two....
The reason I do this is that we are making efforts to compile a support
database from the archives of this list and someone looking to copy PCB
sections is *not* going to look under "complex multi-level schematics." So
"appropriate" means something which as clearly as possible refers to the
problem. In this case the problem really has nothing to do with Schematic
but with how PCB operates.
Now, I know that Mr. Bernesi is probably facing a deadline, and, besides,
he's a newcomer and newcomers deserve special treatment; this is not aimed
at him, but is merely a request to all writers.
Now, as to the question, the first one (there is another question in the
post which is completely unrelated to the first question, which I'm not
answering here), when a block containing components is copied in PCB, the
net attributes are normally not copied. So all those 23 other modules have
no net assignments, which is why they generate DRC errors; there are free
no-net primitives in contact with pads, and no-net pads are not allowed
contact with *any* other copper primitives.
So how to get from A to B. There are many methods which have been described
in this list from time to time by various authors. But here is a rough
outline of one:
In one module, on the schematic, make all the reference designators such
that they can be generically edited to represent each of 24 modules.
Perhaps the ICs would be numbered UX1 instead of U1, etc. Place the module
on the PCB and route it as usual. On schematic, copy the module 23 times so
you now have 24 modules. Edit each module to globally replace, within the
module, X with NN, where NN is the module number. This, of course, assumes
that X has not been used anywhere in a reference designator except as
described herein.
In PCB, copy the original module to a scratch PCB. You could edit the
reference designators on the original PCB to replace the X with 01 at this
point. Be sure to save the scratch PCB, then edit it to replace X with 02;
copy this back to the original PCB in the place of the second module.
Reload the scratchPCB, edit X to 03, copy, etc., etc.
There will be DRC errors on all the copied modules. To get rid of them,
generate a full netlist from the schematic; load this netlist into PCB, and
run Update Free Primitives from Component Pads (under Design/Netlist
Manager/Menu). Any errors left are presumably real errors.
Now, if Mr. Bernesi has already got the proper numbering of all the
modules, both on his schematic and on the PCB, he only needs to run that
Update command to fix the net assignments on the track he copied.
Abd ul-Rahman Lomax
LOMAX DESIGN ASSOCIATES
PCB design, consulting, and training
Protel EDA brokering (resale) services
Sonoma, California, USA
(707) 939-7021, efax (419) 730-4777
[EMAIL PROTECTED]
[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* This message sent by: PROTEL EDA USERS MAILING LIST
*
* Use the "reply" command in your email program to
* respond to this message.
*
* To unsubscribe from this mailing list use the form at
* the Association web site. You will need to give the same
* email address you originally used to subscribe (do not
* give an alias unless it was used to subscribe).
*
* Visit http://www.techservinc.com/protelusers/subscrib.html
* to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
________________________________________________________
To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'
More Information : http://www.dolist.net
