PCB-GCode tips and tricks for full isolation

My PCB milling techniques are getting better at each trial-error experience.

Going to the SMD area there are a few tricks and adjustments that will improve the overall quality of the work.

By the way I'm now using some 0.1mm @ 60º V-bit for the PCB echting process instead of the 10º I was previously using. The results are a lot more even. I'm now going at 0.02mm of depth instead of the 0.05mm in my last config. Actually my new config has changed quite a bit.

I'm now using these settings:

Milling depth: 0.02mm
Tool size: 0.4mm (I moved the compensations and safety margins to this field. Run-out, vibrations and all unknowns are in here instead of being in the default isolation margin.)
Default isolation margin: 0.05mm. Reflects the changes above.
I still use the double passage method for best results. Maximum and Set Margin should reflect that has explained in an early post.

Also as I stated in early considerations the DRC tool in eagle is very important. And should reflect the given formula (Minimum clearance = Tool size + 2xDefault isolation margin) for all clearances.

Ensuring full PCB routing trick

Some times enough clearance between track simply can't be achieved or is too difficult. Here is a technique to overcome that limitation. (Remember this will ignore the clearance rule so your machine may not be capable of reproducing a good route/via/pad because it is just bellow the resolution it withstand).
You clould "lie" to the pcb-gcode plugin about the size of your tool to achieve until path was achieved, but this would result in poor final qualitty since all routes/pads/vias would become thinner than expected. This should be avoid.

Here is an example.

Check your clearances. Try to fix as many has you can. Remember that if you can't guarantee the given clearance the gcode generated will also reflect that and route isolation will not be fully achieved.
In the following circuit I used the DRC tool and my failed clearances were highlighted like in this image.

Eagle after DRC tool

Generated echting gcode

As you can see the the milling route in the areas without enough clearance is not generated.
To overcome this manually add some milling routes in the Milling Layer (layer 46 of eagle)

Manually added route

Generated milling gcode

Merged gcodes (milling + echting)

Has you can see the highlighted gcode and track are actually the milling gcode. The final result is a single pass routing to perform the desired isolation.
If the echting tool is not too big and the routes are not that thin the achieved result is very acceptable. The resulting route will be slightly thinner but it wont be that bad. This will in almost every situation yield best results.

Here is the output of the above circuit with those tips applied

Milled board with SOIC28, mini USB and SMD parts

NOTE:

I detected a small bug in pcb-gcode plugin. The first routing of the mill gcode file those not go to the default milling depth (the G01 Z-X.XXX FXXX instruction is not being generated). You must added it manually.

Cya next time.