On 12:21 PM 22/05/2001 -0700, Rimas Avizienis said:
>hello again,
>
>i am wondering if there is an easy way to merge two completed board
>designs (so as to have them manufactured as one board). i have designed
>two smallish (2" x 4") boards that are designed to be connected to one
>another and stacked. i currently have two separate protel layouts for the
>two boards and i was wondering if i could somehow merge them into one set
>of gerber files so i could have the two boards built as one big board
>which i could then cut in half. each board is six layers, on one of the
>boards 4 layers are power planes and on the other 2 are power planes and
>two are internal signal layers. anyone have any advice on how to do
>this/whether its possible? maybe i could somehow merge the completed
>gerber files outside of protel? or maybe convert the power plane layers
>into signal layers with big polygon pours on them and somehow merge the
>files within protel?
>
>thanks for any help!
>
>-rimas
Rimas,
I would not merge two boards in Protel with different lay-ups. I might
consider doing it in Camtastic - using the gerber files.
If it only for a prototype, I would probably quickly determine that my time
was more valuable and the saving not worth it.
If it is indeed a production issue, as it sounds like it might be - to
simplify or cheapen a production process - then I would probably try to lay
both boards out using the same layup (same number and order of positive
signal and negative power planes issues) and the same design rules.
Can you manage the two designs as one schematic? This can be a little
messy when doing the sch, as you try to manage all the net names including
the power nets, but it does make the PCB design task easier and you do not
need to do any mucking about with gerbers that often rely on someone
remembering what, how and why something was done. If you do accidentally
use the same net on both designs you will know about it as there will be a
DRC warning(s) or a track(s) crossing the board boundaries. I did one
design were I deliberately ran tracks across the boundary on an unused
layer to remove the supply and GND broken net connections as I used the
same net name for power/gnd on both sub-designs.
If you can't do this sensibly then you might consider doing a photo-merge
of the coinciding signal and plane layers. You would place a large fill
voiding the power planes (removing all copper from the power planes) under
the region of the other board *for * those plane layers that correspond to
signal layers - extend the fills well beyond the edge of the other
board. So for your six layer board you would provide 8 copper gerber
layers and request that the PCB maker merge relevant pairs (as a
positive/negative) merge.
You could use poured poly pours for two of the 4 plane layers on one board
and then the merging can be done easily in Camtastic - or mark accurately
and clearly where the other board should be in one of the designs and let
the PCB maker do the merge.
I would not do such a post-layout merge in Protel without *very* careful
thought - and based on years of experience in using Protel for producing
production panels (something I dislike greatly, but is appropriately done
in some cases - less so now with the availability of Camtastic). Watch out
for issues such as rules not being brought across when you copy and paste a
design (so rule based mask and paste expansions are not carried over), use
Paste Special to avoid getting duplicate designators renumbered, you can
forget doing a DRC once you have modified the board in this way (so save
originals of both individual boards) which then raises the problems of
doing changes in one or both boards requires updating the combined file
which is an error prone process. When I do all this in Protel I always
have a lump in my throat as it is at the final stages of the PCB design
and, so by definition, late. You are under pressure doing an error prone job.
I am not sure what I would do - depends on the complexity of the designs, I
think, and the number of voids and holes in the power planes. I am not a
great fan of large poly pours as it slows redraw rate, increases DRC time,
and I was bitten a number of times years ago by the phantom poly pour
problem of previous versions. Maybe though that is the simplest method for
you in this case - and then you can do the merge either in Protel or
Camtastic yourself or get the PCB manufacturer to do it.
Ian Wilson
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
