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/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *