Electronics > Altium Designer

I can't get the board outline to gerber

(1/2) > >>

brianbange:
I can't seem to find how to output the board outline in:
FILE - FABRICATION OUTPUTS - GERBER FILES - Drill drawing tab

Does anyone know how I can get the board outline in the gerber of the drill drawing.
I'm really wasting my day on this and have better things to do.

Thanks in advance,

Brian

free_electron:
draw the outline on a mechanical layer. in the project outputs create a 'final' project. there you can add the board outline to the plot.

hesam.moshiri:

--- Quote from: brianbange on May 08, 2012, 10:31:42 pm ---I can't seem to find how to output the board outline in:
FILE - FABRICATION OUTPUTS - GERBER FILES - Drill drawing tab

Does anyone know how I can get the board outline in the gerber of the drill drawing.
I'm really wasting my day on this and have better things to do.

Thanks in advance,

Brian

--- End quote ---

I had the same problem, here you can consider the reason and solution.

https://www.eevblog.com/forum/altium-designer/altium-gerber-export-board-outline/

dfnr2:
Free_Electron gave you the exact answer.  Not knowing your level of experience with Altium, I'll spell out the steps a bit more explicitly:

1. Use "Design->Board Shape->Create Primitives from Board Shape".  Create the primitives in a mechanical layer, and make sure nothing else is in that layer.

2. You should be using an OutJob to create the Gerbers.  Right click the "Gerbers" line, select config, go to the "layers" tab, and check the mechanical layer containing your outline.

3. Document your convention, including the name of the outline Gerber, in your README file.

Dave

free_electron:
Here is another technique : i simply draw the outline on the keepout layer.

S-y. ( select all on layer )
Define board from selected objects.


Do design

In gerber. Export job , the keep out layer will automatically be injected as a separate plot.
If. You draw it on a mechanical layer , make sure the 'add to plot' is turned off, or it appears on every single gerber file.  Board houses don't like that as they have to remove it ...

Navigation

[0] Message Index

[#] Next page