Skip to content

Panelising PCBs for Seeed – Eagle and Gerbmerge

The problem of panelising PCBs created using the free version of Eagle and gerbmerge is described in an instructible but I found a couple of issues when creating gerbers for Seeed Studio. This outlines the issues and my approach in brief; it is mostly a public note to myself to remember what  to do next time. The account that follows assumes the guidance in the instructible is followed by default.

The issues stem from use of the “.BOR” and “.GML” gerber layers. Seeed’s instructions do not mention BOR files and they do say that the board outline should be in a GML file, which is supposed to be the milling control. My guess is that if you do not send a GML file, Seeed will use whatever is in the silk layer to guess the board outline. My board had some milled slots for a power connector.

Step 1 – make sure the CAM file emits the right Eagle layers to the right Gerbers

Start the CAM processor and open the CAM file provided by Seeed. It would be silly not to!

Click the “Add” button to create a new job section. Change Job|Section to (e.g.) Board Outline and change the output device to GERBER_RS274X. Style should have only “pos.coord” and “Optimize” ticked. Change the file name to %N.BOR

Select layer Nr 20 (Dimension).

That defines the .BOR file that gerbmerge needs to lay out the panel.

Next, select the “Slot drills/holes” tab. Note the file is %N.GML. Layers 20 and 46 should be selected. De-select layer 20.

Save the file (with a new name) and execute the CAM processor. Here is my variant CAM file: Seeed_Gerber_Generater_v0r95_DrillAlign + BOR and GML separated for gerbmerge ONLY.

Note that this should probably not be used for creating gerbers for a board that will not be panelised because the GML file does not contain the board outline as Seeed request.

Step 2 – edit the panel.cfg file for Gerbmerge

Note the existing lines “BoardOutline=%(prefix)s.bor”, one for the merged output and one for each sub-board. These stay as they are.

If there is any milling (check by looking at the GML in a gerber viewer, if you don’t already know), add “*Milling=%(prefix)s.GML” on a separate line in each of the sections where “BoardOutline=%(prefix)s.bor” appears.

Make sure the line “OutlineLayerFile = %(mergeout)s.OLN” does not begin with a “#” character.

Step 3 – panelise and hack

Run gerbmerge as normal.

Note that if there is no milling, is should work fine to rename the merged output OLN file as GML.

Otherwise… a bit of cut and paste hackery is needed to get the final merged board outline and the in-board milling into the GML file. Copy the section from just below the line with only a % character to the end of the OLN file and paste this into the merged GML file just below the same point, making sure that the last line from the OLN does not get merged with an existing line in the GML.

Now check all the panelised gerber files in a viewer!

This information is provided without warranty; if your boards come back wrong its your fault, not mine.

Post a Comment

Your email is never published nor shared. Required fields are marked *