PCB prototype milling using CNC 3020

PCB prototype milling using CNC 3020

posted in: CNC | 6

Making your own PCB prototypes without all the messing around with chemicals sounds like a dream come true. The availability of low cost and seemingly high precision engraving / milling machines could provide the ideal tool for this, but in practice things are not as simple or as good as they appear.

Ebay has a number of vendors selling desktop CNC mills, commonly called CNC3020. I think the 3020 refers to the size 30 x 20 cm. These are also often referred to as engraving machines, which is probably nearer to the truth than them being a milling machine. Prices start at around $600 (USD).

If you are thinking of buying one of these please read this whole posting, as there are various bits of important information, which I’ve inserted in what I think are logical places in the description of the unit and how its assembled, configured and used.


The first thing to note with these machines, is at the time of writing there are two different variants available, the “old” and the “new” model.
The “new” / improved model has both different mechanics and different electronics to the “old” model.
This is an example of the “new” version.

The key difference in the mechanics seem to be a strengthened gantry on which the “spindle” / milling motor is mounted, with  a thick aluminum plate all the way across. I suspect there are other mechanical changes, but its hard to tell from the photos on eBay.

The other difference is the power supply / motor control unit. The “new” version seems to be housed in a black box, with a sloping front, where as the old version was in a blue box with vertical sides all the way around. The changes appear to be more than just the cosmetics of the box. The PCB’s in this box differ from the ones in the old model as well – however whether they are an improvement over the old version, or just an alternative set of boards, is hard to tell.

I’ve read a lot of postings about issues of the control unit “missing steps”. This is where the PC tells the control box to move the motor a certain number of steps, but the motor doesn’t turn as much as it is supposed to because the control unit has not passed the correct number of steps onto the motor. I’ve not personally experienced this issue, as it manifests itself with cutting head not moving as far as it should do in any particular direction. However I have found other issue where the cutting head was actually moving slightly too far. More on this later.


My CNC 3020 arrived as a partial kit, but without a mechanical assembly manual. My unit came with a CD that contained some software and a word doc explaining in pigeon English how to configure the software, again… more on this later.

I suspect all these units arrive partially assembled, where the motors were not attached to the frame, and their control / power wires were not attached. However its a relatively simple process to attach the motors using the bolts that are supplied, and the unit even came with Hex / Allen keys to tighten up the bolts. You also need to fit the flexible couplers on between the spindle of the motors and the lead screws, but this also just involves doing up some small Hex screws.
One thing that was slightly odd about my CNC 3020 was that the 3 couplers were not the same design, but all had the same internal diameter for the motor and lead screw shafts. As the unit didn’t come with an assembly manual, I made a guess that the odd one out, of the couplers, should go on the main, back to front / Y axis lead screw motor, however I suspect it does not make any difference.

Once the motors are bolted on, and you guess which control / power cable goes to each motor, (you can work it out from which cable will nicely reach each motor), you can connect the 4 circular control / power cables to the back of the control unit, and connect the control unit to a PC via a Centronics printer cable.

Yes… This unit needs your PC to have a old fashioned Centronics / parallel printer port. If your PC does not have one, you are out of luck.

Buying a USB to Centronics adaptor cable will not work, as the software that is supplied with the unit directly generates square waves on the Centronic port’s pins, using a special Windows driver, and this will not work with a USB to Centronics adaptor.


Anyway, assuming you have an old PC, even a laptop which has a proper Centronics / parallel printer port, you should be OK; but please note, I am also using Windows XP, and I can’t comment on whether Windows 7, or Windows 8 etc, work even if you have a machine with the correct hardware.

The software that came on the CD with the unit, is “Mach3” except it is a “demo” / limited version, which seems to be quite old.

Once installed, you have to enter the calibration numbers as stated on any installation documents supplied with the unit. This is basically the number of steps that each motor needs to take to move the cutting head 1mm

The limitation of the software is that it will only process 1000 lines of GCODE data. GCODE being the standard language for CNC machines and is generated by all sorts of design packages.

The 1000 line limitation is something which is likely to be an issue for most users fairly soon after they start to try to mill anything other than some demo files e.g. the outline of the “Roadrunner” cartoon character, and the best option for most people is to buy the full / official version of Mach3, which at the time of writing, retails for $175 (USD).

There are other options, including using Linux to control the mill, and also to buy a dedicated USB to CNC adaptor – which replaces parts of the electronics in the control box; however I have not investigated these options as yet.

Once you have connected it all up, and calibrated the software, you should be able to move all 3 axis motors and do a test mill of the “Roadrunner” icon to confirm that everything is working OK.

Tip:  One thing I do to test a new set of GCODE is to set the Z  zero position of the unit to about 5cm above the actual milling bed, and without a cutter in the chuck, then run the GCODE without the spindle / cutter motor running.

Finally after quite some time you are getting slightly closer to being able to mill your own PCBs.   Generating the GCODE for the PCB is relatively simple. An open source package called PCB-GCODE (http://www.pcbgcode.org/ ) can convert either Gerber files to GCODE, or there is a User Language Program (ULP) for Cadsoft Eagle which will generate the GCODE “tap” files from within Eagle.

With the “etch” file loaded into Mach3, you can attempt to mill your first PCB, but first there are a few more hurdles to overcome 😉

Securing the PCB to the milling bed

The main problem with milling a PCB is how to secure the PCB down onto the milling bed. As you will be drilling holes through the PCB as well as milling away the copper, you will need to mount something like a small sheet of wood onto the milling machine, and mount the PCB onto the wood. The best thing I’ve found so far to mount the PCB onto is MDF. The MDF needs to be thick enough so that the drill can completely penetrate the PCB and not drill into the aluminum bed of the mill. If you are careful, you can probably use 3mm or 5mm MDF, however these are likely to be too weak to attach to the bed using the bolts supplied with the machine, so I normally use 10mm or even 12mm MDF, as this feels really secure and robust. MDF has good dimensional stability as long as it doesn’t get wet or absorb a lot of moisture, but should work in most indoor environments unless you live somewhere very humid.

Initially I used masking tape to hold the PCB onto the MDF, however this doesn’t work particularly well, as the edges of the PCB soon start to lift off slightly, as most PCB I have appears to be not entirely flat.

If the PCB is not absolutely flat you will have major issues with the milling process. This is because the normal cutting head for milling PCB’s is a 20 deg or 30 deg V shaped engraving tool, hence the width of the section that is milled is dependent upon the depth that the point of the cutter is below the surface. So if your PCB lifts off by, for example 0.5mm, this is going to cause the cutter to penetrate into the board by an additional 0.5mm, which will mean it cuts a path which is approximately 0.25mm wider than you expect (assuming you are using 30 deg V cutter), this can be the difference between a track existing or getting milled away.

CNC with secured PCB
CNC with secured PCB

The way I hold the PCB in place is to clamp down at least 3 sides of the board using steel plates. I bought some steel fixing plates from a DIY store, which are about 15cm long by 3cm wide and about 4mm thick. I’m not entirely sure what use they have in building construction, but if you overlap them onto the edge of the PCB by a 5mm (or a bit less) them screw them down onto the MDF, the PCB is prevented from lifting on any of the sides. Of course if you have a PCB which bows up in the middle you will still have a problem, so you should try to use PCBs that are as flat as possible, and even possibly flatten them before hand by storing them flat under pressure e.g. between some heavy books.

I’ve seen some examples on the web, where people just used a small clamp in the middle of each side, and I think this would be equally effective; but either way its very important to clamp the PCB onto the MDF as flat as possible.

Cutting tool height adjustment

The next important thing is to set the exact height of the cutting tool. For a while I’d been using a sheet of paper as a feeler guage, and lowered the cutting head a little at a time, until it was in contact with a sheet of paper placed on top of the PCB, so that I could feel definite resistance, when trying to move the PCB, however this isn’t really accurate enough.

A better approach is to use the a continuity meter (buzzer / beeper) setting in a normal multimeter to determine when there is an electrical connection between the cutting head and the PCB. To do this I attach crocodile chips to the PCB clamps and to the cutting bit, and slowly jog the cutting head height down 0.01mm at a time until my meter beeps, I then raise the cutter a few 1/100 of a mm until it stops beeping, and I know its very very close to zero.

Even with the PCB clamped down, there can also be minor differences in its height, so its best to do this Z height calibration in the middle of the area you are about to mill. There is actually a program which will scan the PCB using this electrical connection and re-map the Z height of the milling to take account of minor fluctuations in the PCB thickness / height, however to use it you need to modify the control unit to accept the continuity as the Z zero limit, and so far in practice I have not found it necessary to go to this level of complexity.


When you have finally calibrated everything, you can start to mill the board, and hopefully you will not have too many problem with board thickness or warp.

After the “etch” path has been milled, you need to change your cutting bit to a 1mm or 0.9mm PCB drill, and load the “drill” tap GCODE file. Its important to not loose the X and Y calibration when you are changing the cutting bit for the drill bit, otherwise it will be very hard to get the machine re-positioned correctly to drill the holes in the correct locations.

I have attempted to use the same continuity technique to calibrate the Z zero on the drill, but I think perhaps the drills come pre-coated with some varnish, as they are not good conductors when they are new.

Its also very easy to snap the PCB drill, by applying downward pressure. So under no circumstances “jog” the drill down onto the PCB surface when its not spinning, otherwise you stand a very high chance of snapping it. Trust me, I have snapped one drill this way, and snapped a second drill trying to manually drill out some holes which the mill didn’t drill completely through a board.

As the depth of the drill holes isn’t that critical, as long as its completely through the PCB, its safer to use the paper technique, with some thicker paper, to get the Z height about right, even if its 0.5 or 1mm above the board, and set the drilling depth to 2,3 or even 4mm to ensure the drill goes completely though the PCB. (Assuming you have a decent thickness of MDF below the PCB).

After the board has been drilled, then and only then, should you release the clamps are remove the board.

Results so far…

So far I have only milled single sided boards. Milling double sided boards is technically possible, however I can see a number of possible problems around the re-registration of the zero point (X,Y), as after the board is flipped over, it would need to be repositioned to within about 0.05 of a mm in both X and Y of its original position. This can probably be achieved by adding a calibration drill hole at 0,0 in the board GCODE file. However the other problem is rotation. i.e 2 calibration holes would be needed to ensure the board is not slightly rotated. Or perhaps some sort of metal jig could be bolted to the MDF prior to milling the first side, to ensure that the board is refitted in exactly the same location.

I’m personally very skeptical about the feasibility of doing this. I know it can be done, but I think it would take quite a lot of practice and experimentation to develop a process to make reliable double sided PCB’s a practicality.

However overall, production of single sided prototype boards is entirely possible on the CNC 3020, it just takes some time and effort.

6 Responses

  1. matthias lichtenegger

    So I sum up:
    600USD for the machine
    150USD for the full version of mach3
    =750 USD
    + problems caused by parallel interface (Ok, on desktop pc’s you can buy a pci-parallel card) and problems with newer versions of windows (so I guess)
    So maybe it’s a cheaper/better solution to buy a (partial) set of a prusa i3 a rebuild it as cnc?

  2. Roger Clark

    Hi Matthias

    Yes. I totally agree. These CNC machines are useless to mill PCB’s

    The fundamental problem is the physics and geometry of milling insulation between the tracks of less than 0.5mm wide.

    The cutting head is a 20deg or 30 deg V shaped tool, and the width of the cut is proportional to the depth of the cut.

    In practice the PCB’s are not very flat, and even if you clamp them down with metal brackets on 2 or even 3 or 4 sides, the PCB is higher in the middle of the board furthermost away from the clamps.

    With the result that the cut depth changes far too much.

    I know that some people, use a pre-process, which uses uses the cutting head as a continuity tester and software takes point height measurements across the whole PCB (perhaps 100 points) then remaps the Z height of the routing file to match the high changes to the PCB, but this is a complex process, and it requires modification of the CNC controller hardware so that an additional input goes from the CNC router continuity detector into the PC (via the parallel interface), and I’m not convinced that even doing this would give perfect results.

    I think if it was possible to CNC mill boards, then prototyping companies would use this process, but as far as I know, they use etching.

    CNC machines like this are probably good if you have to drill lots of through holes, onto an etched PCB and good for other things like engraving plastic and wood.

    But I’d not recommend them for PCB production

  3. Chris

    Clamp a peace of wood to your bed mill it true with a end mill and stick the PCB with DS Tape to the board,

  4. Roger Clark

    The issue is not really the flatness of the bed, though I agree if I mill some wood flat it will be flat with respect to the milling head.

    The problem is that I’d need to glue the PCB to the wood to get it flat enough

    I’ve tried using double sided tape (very strong tape), but unless you cover the whole of the back of the PCB, the PCB will warp enough to affect the milling of the insulation between the tracks.

    I’m sure it would be possible to mill PCB’s for big SMD components e.g. 1206 resistors etc, but for me it would still be neigh on impossible to reliably mill the tiny tracks on quad flat package MCU’s etc


  5. Chris Bezuidenhout

    I agree with you, but for a proto board it is ok I still prefer the etching method because most of my designs are double sided and I do a lot of RF development then the track with is very importent and I do thru plating and with an engraved board it is just not possible. I still use Protel for my layout and I will only use the 3020 for drilling as soon as I find out how to convert the Protel gerber files to G-Code

  6. Roger Clark

    Thanks Chris

    Using the 3020 just for drilling is a good idea. I only use Eagle and more recently KiCad.

    I suspect there must be a script or macro to convert Gerber drill files to G-Code.

    Perhaps as described in this article


Leave a Reply