Problem with CNC 3018 Pro when milling pcbs

[ClemensU42]

Hi everyone,

I recently bought a CNC 3018 Pro to make PCBs because I'm not really comfortable working with acids and when receiving it, it worked fine milling a test image into a piece of wood.
But when I tried milling a PCB, the result is a mess. The rendered GCode on the computer is different than the actual result, for example the solder pads all have differents sizes. I have no idea what's wrong with the machine. I already checked the config of the cnc machine and it seems fine I also tried different programs to send the gcode over to the machine and the result is always the same. I attached an image of the gerber file and an image of the result.

I hope some of you could help me figure out, what the issue is.

[Kean]

Not sure of the size of those pads and traces, but you seem to be expecting a bit too much from a cheap machine.
You need to spend a lot of time tweaking things for such fine detail.  I'd guess mechanical backlash in the Y axis may be your biggest issue right now, but fixing that will probably just show other constraints.
Make your traces thicker wherever possible.

[thm_w]

Do you have a dial test indicator you can use to measure backlash?

You can find milder etchants if you want, I think these are relatively safe:
- https://en.wikipedia.org/wiki/Sodium_persulfate
- https://quinndunki.com/blondihacks/?p=835 (vinegar and hydrogen peroxide)

[E-Design]

(1) run the spindle as fast as it will go. Make sure it is tight in the holder. Machine should be as rigid as possible.
(2) Use the height map - your board isnt flat.  its a must to use this.
(3) You dont have the right feed and speed yet for your bit. You have to do some test patterns first before you try a board.
what is your depth of cut?  typical between 0.05mm and 0.1mm

Ive had issues like this early on with the 3018 and they can be resolved with some experimentation to dial in your settings.

[PlainName]

The cutter seems to be going in too deep. I suspect you're using one with a narrow angle to minimise the width variation with depth of tool but, counter-intuitively, the reverse is better - something at least 45 degrees and maybe even 90 degrees.

Flatness of the PCB is critical. A suggestion above is to use a height map, but when I set up my system that kind of thing was unavailable without a lot of hassle. Instead, I use a 15mm thick acrylic sheet (thinner is OK! I just wanted to be able to make threaded holes in it) which is bolted to the milling table and then made flat with a flycutter. I then use carpet tape to stick the PCB down and it is as flat as a very flat thing. Using LPKF cutters I can do 0.5mm pitch SMD devices.

The edges of the tracks are a bit rough in your photo, suggesting the cutter isn't really sharp. You can extend the life and have neater cuts by using a lubricant. I spread 3-in-1 oil across the entire PCB surface - it doesn't get flung off and is easy to clean up afterwards with a kitchen towel, plus it stops FR4 dust going everything. Except for milling out the PCB with a 2mm bit and then there is so much debris the oil can't possible cope, so I do that dry and use a vacuum to suck away the dust. (This is also where using carpet tape is useful - you can completely cut out the PCB and it won't move so there is no need for tabs. And the slight thickness of it means you can cut entirely through the PCB without leaving a mark on the (sacrificial) acrylic sheet.)

Also as mentioned above, you want to spin the cutter at a high speed - 20krpm at minimum. You can run at a lower RPM but then the cutter movement has to be slowed down to suit so it's not taking huge cuts.

Ultimately, you'll probably find that the successful way of doing it is different from all the suggestions here - whatever works is good! But taking note of some obvious stuff will give you a head start along the road of tinkering that will no doubt be required to perfect the process for you specific setup.

[Doctorandus_P]

I'm with Kean.

Your mill seems to be doing what it can do. You just can't expect 4 mill tracks from a cheap chinese mill.

Some things you can try:
May be you can (and should) add some radius compensation in your software. The center of the mill may be going over the edges of your Gerber files, and it should be the side of the mill.

Use coarser tracks. Adjust the feature size to match the capabilities of your tools.

If your machine has backlash, then you may have some success with a weight, rope and a pulley, to always pull the backlash to one side.

But there are many other variables. PRM, feedrate, quality form of the mill itself, ...