Exporting the right Gerber Files from Altium6 or Protel99SE

Archive BatchPCB
1

Hi All,

Could someone please help me with a technical answer regarding how to cleanly and correctly export the specific Gerber files that batch pcb ask for from my software.

I have access to both Altium 6 and Protel 99SE at my educational institution. I’m not really keen on learning Eagle just so I can apply the supplied tutorial.

I would prefer the instructions to be given for Altium 6, but 99SE would be cool too I guess.

In Altium6 I know I create the cam document and then I can use a wizard to export the excelon drill files, and the gerbers. I don’t have a particularly good understanding of the Gerber or Drill formats, so I’m not so sure what some of the options mean. Especially so when the Eagle tutorial uses different names for everything (relative to Altium).

I did notice in particular the example on the main page for batchpcb stating that the drill file is bad if there is only 1 coordinate supplied. I checked my drill exports and it seems some only have 1 coordinate.

I must admit I am quite daunted by this whole process, but it is something that I am very interested in learning. I hope someone can help me out.

Thanks for reading my long winded message,

Joshua

2

Hi Jobro,

Nobody replied to this, and I didnt’ see it earlier… Sorry this reply is a month late :slight_smile:

Designer 6 gerber/excellon output

File->Fabrication Outputs->NC Drill Files

-Set to Inches 2.4 (or mm 4.3)

-Keep leading and trailing zeroes (probably easiest for all)

-Reference to absolute origin (relative origin is probably OK too)

-The options at the bottom can all be unchecked, though you may

want to generate separate files for plated/unplated holes.

-Click OK and the drill file will be created.

A .DRR file will also be created with potentially useful information.

File->Fabrication Outputs->Gerbers

tab: General

-Set to Inches 2.4 (or whatever)

tab: Layers

-Check the layers you want to export.

-This should include the border layer.

-Leave everything else unchecked. (ie: no mirroring, etc.)

tab: Drill Drawing

-Uncheck all

tab: Apertures

-Check the RS274X box

tab: Advanced

-You may need to increase film size. Maybe to 40000, 40000

-Check “Separate file per layer”

-Check “Reference to Absolute Origin”

-Check “Unsorted (raster)”

-The others probably dont’ matter too much.

Now click OK and the gerbers will be generated. This will open a camtastic window too, but you can just close that. On the other hand, you can check the layers while you’re there.

I won’t tell you how to do the export from Protel99se unless you need to know, because it is a little different and strange.

Steve.