Cadence Allegro (OrCAD) PCB Editor ~ Gerber & Drill Output

[Terri Miller]

Hello all!

To generate Gerber & NC Drill files from OrCAD (Cadence Allegro) PCB Editor, Open the native file (.BRD) in OrCAD PCB Editor;

Gerber Files: From the Editors window, go to Manufacture > Artwork; on the Artwork Control Form, click on the General Parameters tab to make active and then confirm the following settings:

Device Type ~ Gerber RS274X
Film Size Limits ~ 14 x 16

Leave remaining default settings to keep outputs consistent. Now, click on the Film Control tab and choose Select all from the bottom of the Available Films section and then Create Artwork. Choose OK to close this window. The artwork (Gerber files) should now reside in the originating folder (where your .brd file is located).

NC Drill File : From the Editors window, go to Manufacture > NC > NC Drill. The NC Drill dialog box will open. Confirm that the root file name is present (board name.drl) and choose 'Auto Tool Select'. Leave remaining default selections. Click on the Drill button to generate the NC Drill file. The NC Drill file should now reside in the originating folder.

Please review attached document Allegro OrCAD PCB Editor_Gerber-Drill Output.pdf for screenshots and easy reference.

If you have any comments or suggestions about this post or any other, please leave a reply here on our forums or contact one of our Customer Service Representatives and we will do our best to assist you!

Terri Miller

***

[JasonG]

For 4 layer boards the website PCB Express states that the inner layers are to be negative artwork: Inner layer exposed copper Required: draw .050 mil trace back set/keep-out areas for processing. (See sample picture A.) This results in a negative plot where our film will flood the empty area with copper. The pads, backsets keep out areas will be clear of copper.(See sample picture B.) I've tried to do this in Allegro by selecting 'negative' on the layer dialog and also when generating the artwork, but I don't get proper clearances on vias or holes. Can I submit positive artwork for inner layers? Or can you tell me the correct way to generate negative artwork? Also, there is a nice tutorial for generating artwork from Allegro on http://www.referencedesigner.com/tutori ... page_9.php

Thanks

[Terri Miller]

Hello Jason,

This section is referring to the inner layer exposed copper area. For processing we want to keep this area clear of copper. See sample picture A... the outline around the image will be the backset (sample picture B) and will keep the area around the board copper free.

We do accept postive polarity for inner layers as well. For our Quick Turn products we only accept positive polarity for outer layers.

And thank you for the link! I really like the tutorial too... it looks like videos will be posted soon as well. There is a lot of helpful information there.

However, for Quick Turn orders we do prefer that the 'Auto Tool Select' option is chosen for the NC Drill file - this way each tool has it's own number and there isn't an end of program command with every tool size listed.

I hope this answered your questions about the inner layers. Let me know if you need further information.

Terri