we panelize in PCB everyday (without going the gerber route) you have to be careful of course
As has been mentioned, P99SE is not the best tool for panelization. CAMtastic may be better, it is designed for that.
Some layers in Protel are called "calculated" layers. This means that the layer is not literally present in the database, but is calculated depending on, for example, solder mask expansion rules. Inner planes are also calculated layers. So if you are copying a PCB for panelization, you should realize that the resulting panel is not DRCable. And there could indeed be problems.
First of all, the copied primitives must have the correct net assignments, the copied components must have the same reference designators, etc. If you know how to do it, all this can be done.
(1) Generally fabricators prefer to panelize, since they can make the panels fit their process requirements. They don't charge for panelization, as far as I have seen.
(2) Sometimes designers panelize to produce more copies of a board being made by a prototype service that is cheap for, say, one or two or three copies of a board. These services typically panelize boards from different customers, that is one way they can make boards so cheaply. I know of one company, a major one, that explicitly prohibits such panelization by the customer.
(3) When the desired board to be stuffed is, for example, a breakaway panel with multiple boards, broken apart after it is populated, it may be desired to panelize for one's assembly requirements. This is the major good reason for panelizing. But it is still better done in a CAM tool.
(4) Because Protel is not really designed for panelization, it does not have tools for DRCing a panel; and because of the calculated layers, it is quite easy to have errors in the added board images. Note that if a fabricator does the panelization, it will be the fabricator's responsibility if there is an error in this process, not yours. (And I'm pretty sure you are not a fabricator or you would not be attempting to do panelization in Protel, you'd have a much more efficient CAM tool for doing it.)
(5) Your Protel database will become enormous, which can slow you down in many ways.
(6) Sending a single board's worth of gerbers plus a master panel layer (see below) to a fabricator with instructions to step and repeat everything but the master panel layer involves, for the fabricator, a few second's attention, it might literally be less than a minute. And the size of the transmitted data will be *much* smaller than for a complete panel. A file zip program is not going to notice that all those different numbers are actually the same data offset! Nowadays with high-speed lines, etc., we often forget the data transmission time issue. Until we try to put our plots on a floppy. Or we discover that the size of file attachments is limited by someone's mail system.
One way that I've done panels in Protel, on the rare occasion that the job required it, was to make a PCB file have only one copy of the final (smaller) board. On a mech layer, the "master panel layer," I place track and text that will become part of the final panel that is *not* to be multiplied up. This would be, for example, legends or the outlines of cutouts.
Then the gerbers are generated. In CAMtastic, the gerbers for everything except that master panel layer are imported and panelized, together with one copy of the master panel. If properly designed, it should all fit neatly.
Now, if one *must* do it in Protel, I'd recommend reimporting gerbers to a new board file, to make a free-primitive, explicit image of every item to be multiplied. The rules for this board should be set so that calculated layers do not create any altered plot primitives; this image can be copied and pasted into every position. Because they are generated from gerbers, they will be identical when plotted to the primary (original, single) board.
I'd set all solder mask expansions to a large negative number, for example. The reason is that the actual solder mask flashes should come from the original solder mask plot, which will have the correct aperture sizes according to the original design rule settings. The free pad primitives on, say, the bottom layer, would otherwise generate their own solder mask plots, which might differ from the rule-based settings in the original design.
And if one finds an error in the primary board, resist the temptation to try to correct all the individual copies; not only is it faster and easier, usually, to do it with one board, but the process will be error-prone and not DRCd. Fix the one board and then do all the multiplication again. Doing it again should be just a matter of deleting all primitives in the panel file, reimporting the corrected gerber, hiding the master layer, selecting all, copying to the clipboard,, and then copying it as an array with the first instance in the same position as the imported gerber. It should be that simple and fast. In this case, the primitives will be duplicated in the
So, again, as a lesson from the School of Hard Knocks, make sure the single board is correct before panelizing it! Consider panelization as part of the fabrication process rather than part of the design process (except that the panelization is itself designed....). When, for example, submitting the board for review by another engineer, don't make the full expanded panel!
The master layer I mentioned is the panel design, and the design reviewer should be able to readily understand that; the actual multiplication of the board primitives (in Protel) or of the gerber code (in CAMtastic or another CAM program) is simply the final step before the films go to physical fabrication. Yes, the completed panel should be checked, but at this step one would be looking only for copy failures, not reviewing other aspects of the design.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *