Problems with cnc while making PCB

Hi, i am having trouble making PCBs with my CNC, the Router bits breaks so often(1 or 2 for each pcb) that makes the PCB(pertinax) very expensive.

I am using 0.1mm and they break very often, and when i use 0,4mm router bit, they makes a hole of 1mm more or less..

I am using mach 3 software while generating the code with pcbtogcode from eagle.

Is there same software configuration i should check up? or are the router bits i have are not that good? Which brand is better in that case?

Thanks i am new in the cnc stuff i bought one with a friend few days ago

Experiment with feed rate, rpm, and depth of cut.

If a 0.4mm tip makes 1mm groves, you dig far too deep. You just need to get past the copper.

Bits should never break, but wear out.

Jakob E.

I agree... In my experience, the copper was so thin, that even a 0.2mm cut was deep enough.

However, added to that difficulty with mine was that it took a lot of force to "pierce" the copper at the start of milling.

That meant I had to specify 0.4mm, then have deep traces.

Annoying!

Thanks jakob and Rochey for quick answers

I cant change RPM, its set to 28000. Is it a good value? Or should i make a trimmer to the spindle(or motor, sorry, my english is not very good)?

About the 1mm, sorry, it looks like the tip wears out very quickly, and start digging 1mm.

Thanks again

28000 rpm is probably a good speed for the small routers.

The tip on the 0.1's should NOT wear out quickly - specially not when running in pertinax/copper (glass fiber is much tougher on them)

Make sure to use a full-carbide bit (DE: Vollhartmetall) - HSS won't do.

I use these bits for engraving - http://www.sorotec.de/shop/index.php/cat/c164_Gravierstichel--Standard--Gravierstichel--Standard-.html - and they do an occasional PCB fine as well. It seems the only thing that dulls them is anodized front panels.

(If you post your location in your profile, sourcing questions are easier answered)

Jakob E.

What kind of spindle is it?

Any "runout" would cause these problems. On my first router I put a cheap router as the spindle, and snapped bits all over the place. Then some time later for I put a dial gauge on it and found that the runout was 0.25mm.

If you were to have a spindle with runout of 0.1 with a bit of 0.1mm cutting diameter, that would be like a spoon whipping around in a bowl of cake batter, as opposed to spinning on its axis like it should.

Just another possibility......

Tim

Thanks for the info, i will try those bits.

The spindle came in the CNC assembled, i dont know much about it, i will tell you when i go to the lab

And i will check about any run out problem, maybe is something related to that.

Sorry i am from argentina, no problem with shipping anyways, most of the time i buy these from ebay.

I have broken two bits in a month of owning a CNC machine. There is a lot if trial and error in getting up to speed with all the aspects of milling.

From a noobies perspective... What depth and plunge rate are you using in pcb2gcode?

If you type "run pcb-gcode --setup" (no quotation marks) in the command line in eagle it will bring up the setup menu with all the finer details of control. I don't have eagle in front of me at the moment, but if you hit the 3rd or 4th tab long it will bring up 5 different setting choices for your CNC software. Make sure you select the appropriate line for Mach 3.

Once you have generated the gcode and have loaded it into mach3, make sure you properly zero the z axis of the machine. Jog the z axis down until it just touches the top of your pcb blank.

If in doubt, remove the endmill from the machine and install a sharpened pencil instead (with the spindle off obvious). Zero your axes, run the program and watch closely. If the pencil get rammed into the pcb, either the z axis isn't calibrated/zeroed properly, your plunge rate is too quick or the cutting depth is too deep. If it starts off fine but gradually lowers the pencil deeper and deeper till it snaps, you might have incremental depth set somewhere. Pcb milling doesn't need it. Incremental depth gradually increases the depth of cut over multiple passes - I have found it quite handy when cutting deeper profiles and cutouts in aluminium and such.

Also, reduce your feed rate right down before you start milling. There is a + and - arrow in the program screen of Mach 3. It increments the FRO up and down by 10%. Once milling has started and you are confident it is going as plan, gradually increase it back towards your target rate.

I had a problem related to mach3 losing my stepper motor tuning settings as well. Generally I leave my CNC machine running all the time, but occasionally I'll come back to it and it will be off (probably a result of it being in a damp, cold of garage). It appears that mach3 can lose the motor tuning settings if it crashes. The right settings for your machine should be listed in your CNC machines manual.


Good luck! Report back on how you go!

I will report you back when i go back to the lab.

BTW the cnc model is:
http://www.cnc-sable.nl/sable-2015-p-21.html?language=en

But the feed rate applies to all axis, not just z, if its too slow it will take some hours per pcb

As soon as i got there i will try and send you the values, and try again, the depth is 0.1mm

Thanks for all the information, its really helpful

Edit:

Feed rate is: 800mm/minute xy and 250mm/minute z, is it to high? se z the same, but i noticed the spindle is vibrating a bit, may be this the problem who is breaking my bits?

I read a saying about CNC machines when I was looking at which one to buy. It goes like this:
Time, value and quality. Pick any two of those.

I am using a CNC6040, which is a decent sized machine and works really well for a variety of tasks... but because it is an entry level machine (even at $2000...), it does have some drawbacks. One of them is time. It will take longer to complete some tasks than more expensive, higher quality machines. I can't cut PCB's of excellent quality at 800mm per minute on my machine. At 800mm per minute it will snap bits and generate runout on the spindle. I usually run it at around 450mm per minute, but then again my spindle has a maximum RPM of 9000, not 28000 like yours. Your spindle could be shuttering and vibrating because your feedrate is too fast. It might be moving the spindle faster than the endmill can cut the copper.

My suggestion to reduce the feedrate right down is to determine what the best feedrate for your machine is when cutting PCB's. Start slow (like 100mm per minute) then increase it gradually as it is cutting. Keep increasing it gradually (maybe by 10% each minute) to the point where the machine is cutting nice clean traces quickly. If the machine starts shuttering, or the endmill snaps, or you get run out where your 90degree turns look like larger arcs, you have increased the feedrate too far.

The machine you are using, the material you are cutting, the speed of the spindle and the type of endmill you are using will all alter the required feedrate. Using a 0.1mm V bit will probably require some slight changes to the feedrate compared to an 0.4mm ballnose bit for example. It is all about experimentation.

Once you determine the best feedrate for the task, you can alter the settings in pcb-gcode in eagle for both the feedrate and plunge rate (how quickly the z-axis moves). Set the feedrate to your optimal setting. The plunge rate is usually best set to 20%-30% of your feed rate.

Trial and error my good man. Its all about trial and error. 

Thanks for all the info, it really helped me out!

I broke like 13 bits, but i bought 30 more.. but they are lasting more time, with propper adjustment.

One last question, which i couldnt find on the forum or google

Is there a way to use a pdf for cnc routing? i know eagle can take images and trace the tracks, but i dont know about pdf. And somebody told me once that it was used for vinnyl plotting.

Thanks!

We never worked from pdf but it is a standard format for sign cutting etc. In fact I use an outside shop for laser cutting and he works with pdf.

Agggggggh ....  I have never understood why people want to machine PCBs., just look at the comments in the posts
above. Chemical etching is a very accurate method, a greater track density and doubled sided boards are no problem. Even
professional manufacturers use chemical etching irrespective of board size and quantity.
The echant ... Ferric Chloride is relative safe taking normal and simple precautions, otherwise why is it sold is suppliers
catalogs ???? The etching process takes 10 minutes. The etchant can deposed of easily.  CNC has better uses.


Frank B.

12volts said:

Agggggggh ....  I have never understood why people want to machine PCBs., just look at the comments in the posts
above. Chemical etching is a very accurate method, a greater track density and doubled sided boards are no problem. Even
professional manufacturers use chemical etching irrespective of board size and quantity.
The echant ... Ferric Chloride is relative safe taking normal and simple precautions, otherwise why is it sold is suppliers
catalogs ???? The etching process takes 10 minutes. The etchant can deposed of easily.  CNC has better uses.


Frank B.

Click to expand...

Its not just making the pcb, drilling, cutting and some process which finished units looks better.

Its not the only thing i use it i personally have some problems with etching and the pcb tracks doesnt always etch propperly, its cheaper, of course.

One thing that's needed when milling boards is either a vacuum table or a foot on the spindle to hold the board perfectly flat as you mill, otherwise the bit will dig in (when set low enough to mill the low areas) or miss (when set high enough to just mill the high areas).  You will notice that all dedicated circuit board milling machines have this feature. You could try milling a bunch of straight cuts across the material with a tapered bit and measuring the width of the cuts to see if they are even. You could also mount a dial indicator on the spindle and run it across the board to check for flatness. 

Another problem may be that you need to have a dwell time set when you plunge into the material.  The bit should drill in at a stationary point and dwell for a moment to make sure that it has plunged all the way to the full cut depth before proceeding to make the cut.  It also needs to delay moving to the next location long enough for the bit to raise clear of the board at the end of the pass.

When routing large holes or the board outline, make sure to use the correct bit for that purpose and to adjust the feed rate.  Even if these bits are a lot less likely to break, a feed rate that is too high will make the cut inaccurate at the end of the cut or when cutting curves, because the bit will lag behind.  For a straight cut the dwell time at the end of the cut will let the bit catch up.

Make sure that the board is free of debris by using air, vacuum, or both.

When you get it all working well, I'd be interested in how well your software is choosing the tool path.  I have some dedicated machines that have really bad software when it comes to the tool path.  Could be 2-10x faster if it was smarter.

A last tip:  Think about tool change delays when choosing hole sizes.  Drill vs route...

Actually, I'd like to use my CNC to drill the holes post etching.

But I have no way of telling Mach3 where the fiducials are, and if the board has rotated etc.

/R