Generating a cutting line from a Gerber outline

Question

Our PCB fab has decided to charge us extra for our PCBs unless we provide them with a cutter tool path on a Gerber layer. Amazingly, Altium doesn't seem to have a tool to automatically generate this cutting path. Does anyone know of any software which can generate this, with tabs?

Answer 1

I cannot think of any easy way to do this automatically.

There are multiple issues with regard to how many tabs you need to mechanically support the PCB while the outline is being machined. This would be heavily dependent on your PCB thickness and substrate type, and I can't really see any way to automatically generate tab-route tool-paths without a fair amount of mechanical engineering knowhow.

Also, end-mill allowances and a number of other machining complexities make this something that requires a fair amount of knowledge about the actual board-house tooling.

I guess it should be possible to manually set tab width and quantity, and have an automated process place them equidistantly, but that seems a lot of work for little return, when manual tool-path generation is quite easy.

That said, doing it manually shouldn't be any trouble.

I've had board houses that needed tool-paths for PCB v-grove scoring. I just added another mechanical layer, and drew the tool-path with schematic primitives(Place -> Line or Place -> Arc). As long as you remember to export the additional layer during Gerber generation, it should work fine (though putting a note on the layer re what it is for is probably a good idea too).

There are a few intricacies here, such as whether you need to allow for the end-mill width. This could mean that you would either need to draw the tool-path 1/2 the end-mill width away from the real board outline. You will have to ask the board house for how they want the tool-path.

---

As an aside, the Altium File -> Fabrication Outputs -> NC Drill File dialog actually has a "Generate Board Edge Route Paths" option. Have you looked at that?

Answer 2

I use the Diptrace PCB software. But I have not tried the cutout Outline in it. What I do is to use the ISOCAM software from MEGA UK. I generate the gerber files and send them to the ISO CAM. With the ISOCAM software I can do wonders with the gerber files (with which milling is just one) before sending to the CNC for drilling. So I simply create the PCB cutting outing with the ISO-CAM, and then generate the Milling file from the cut-outling. Check out the MegaUK site http://www.megauk.com/cnc_production_centre.php. The ISOCAM costs about 1153GBP, which is quite expensive. You can check out other means, but this is one that I know of and sure of.