522,226 active members*
2,001 visitors online*
Register for free
Login
IndustryArena Forum > Other Machines > PCB milling > How to avoid premature tool failure
Page 1 of 2 12
Results 1 to 25 of 39
  1. #1

    Join Date
    May 2020
    Posts
    12

    How to avoid premature tool failure

    Hi all,

    I own a desktop 6040 CNC router that is made in China. I have managed to make some good test boards I designed for evaluating the capabilities of my setup. However, I noticed that the tool I use (Stepcraft's V-Router 45°) has gone bad too early. The milling quality was OK for three really small test boards and one larger 40x50mm board (please see the attached pictures). Also, I am unable to use the classic cheap V-bits (30°/0.2mm) because I get rough edges from the first run. I was pretty sure that my cheap spindle was the main problem and I was going to buy a more powerful spindle (2.2kW 24k rpm 4 pole spindle) since I would like to try cutting aluminum in the future. But, other users state in some posts that it is possible to mill PCBs even with spindle speeds as low as 7k rpm if the feeding speed is kept really slow (I use 20mm/min).

    So what you think is the problem here? The spindle and/ or something else? If the spindle is the main problem which cheap alternative would you recommend if you took into account that I would also like to mill soft metals in the future? Is the 2.2kW/24k rpm Chinese spindle OK for this purpose? Should I buy a separate 60k rpm spindle only for PCB milling?

    I would appreciate any advice! Here is the current setup:

    Machine:
    CNC 6040 with SFU1605 ball screws.
    TB6560 motor drivers
    Backlash must be small as shown in the results (when the tool is new and sharp). I am waiting for a digital dial indicator to verify.

    Spindle:
    Cheap FitSain-ER11 Collet chuck CNC Spindle 24V 8000RPM (12-36V). Tried feeding it from 20 V up to 36V but I got the same results. In the attached pictures I use 30V (noticed less vibrations). Actual RPM has not be verified yet.

    Tools used: Genuine Stepcraft's V-Router 45° (success but premature tool wear) and classic cheap V-bits 30°/0.2mm (can't mill at all).

    Software and settings:
    Flatcam & GRBL.
    Feeding 20mm/min.
    Rapid travel speed 100mm/min.
    No auto leveling used until now. I manually verify the board's level before starting the milling process.
    Milling depth 35 ?m.
    4 passes and 40% overlap.

    If you need further information/ pictures please don't hesitate to ask.

  2. #2
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    I think you are cutting to much fibreglass and dulling the tool.

    Leveling of the PCB blank IS EXTREMELY CRITICAL. Its needs to be level to within 0.05mm otherwise you will
    have to command your machine to cut so deep that the tool dulls rapidly.

    I use Autleveller, a software utility that probes the board then modifies the gcode to accommodate any warp, bow of the board.

    On 1oz copper board the copper is 0.035mm (35um) thick. I cut 0.06mm (60um) deep, but even a small board say 50mm x 50mm
    board can have 0.1mm (100um) variance across the board. Autoleveller accounts for and corrects that variation.

    I use 0.5mm two flute endmills because I really like the cut quality and I get 10 hours cutting on each one, assuming I don't break them, they are
    very fine and break extremely easiliy. I also use engraving bits for very fine featured boards and I swap them out after about 10 hours. So it is possible
    to make tools last provided you don't cut too much fibreglass.

    Spin the tools as fast as you can. I have a 24000 rpm spindle, only because I cant afford a 600000 rpm one. I cut at 400mm to 600mm/min
    and plunge at half that.

    Craig

  3. #3
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    I have a 3020 with the standard spindle (I understand it goes up to not-quite-10K RPM, I have never measured) and I usually cut at 100mm/min just fine, at 0.06mm depth (without auto-leveling but on a HDF board pre-leveled with the mill itself). I'm using exactly those cheap 0.2mm v-bits (30 degrees I think) and yes the result is definitely on the burry side, but I've found a quick scrub with a standard kitchen scotch-brite pad removes them like magic. I need to clean the board anyway, since I'm also using a bit of oil on the surface of the PCB while cutting - may or may not help with the actual cutting but it sure traps the dust. Granted, this is not exactly a production-scale method (for any scale at all), but I find it's quite fine for occasional PCB work. I'm considering testing a thin cylindrical endmill too simply due to the width variations inherent in v-tip tools, but I'd prefer something thinner than 0.5mm - I understand one can get even 0.2mm ones for about ten bucks; no idea of course how long they'd last, even on "occasional small simple PCB" scale...

  4. #4
    Registered
    Join Date
    Nov 2012
    Posts
    862

    Re: How to avoid premature tool failure

    I will add my 2 cents...

    If you are feeling vibration at 8000RPM, your spindle is probably not balanced well. You may get better results if you reduce the RPM further (and lower the feedrate proportionally). It will be painfully slow, but the quality and tool life may improve.

    Also check the tool runout with a dial indicator if you have one. Cheap "spindles" (which are really just motors with ER11 collets slapped on) often have problems in that department too.

    Watch your cutting depth. Cutting into the fiberglass substrate too deep will dull the tool quickly. With larger boards, simply levelling the board may not be enough. You may have to use software levelling (such as Autoleveller already mentioned above) or a mechanical depth limiter.

    Narrow (15 or 30-degree) V-bits are not always better. Sometimes you can get better results with wider (45 or 60-degree) bits.

    Even 60-degree V-bit tips are very fragile. Watch your plunge feedrate (I usually set it at half the X/Y feedrate). Avoid straight plunges, try spiral lead-ins if your CAM software supports them.

    The board on the 1st photo looks pretty good, what RPM and feedrate did you use for it?

  5. #5
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,

    'm considering testing a thin cylindrical endmill too simply due to the width variations inherent in v-tip tools, but I'd prefer something thinner than 0.5mm - I understand one can get even 0.2mm ones for about ten bucks; no idea of course how long they'd last, even on "occasional small simple PCB" scale...
    0.2mm is too incredibaly fragile, you'll break them before they wear out.

    With 0.5mm (also fragile) I design my boards to have minimum 0.6mm intertrack/interpin spacing which allows SMD devices down to SOIC,

    https://www.ebay.com/itm/10-0-50mm-0...72.m2749.l2649

    $38 for ten is or $3.80 (plus shipping) is pretty good. The same company supply smaller endmills but I suspect you'll find them too fragile.

    Craig

  6. #6
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    also to use 0.2mm tools will require a spindle with very VERY VERY low runout otherwise you'll break the tool the moment it comes
    in contact with the board.

    Craig

  7. #7

    Join Date
    May 2020
    Posts
    12

    Re: How to avoid premature tool failure

    First of all I would like to thank all of you for spending your time to help me address this issue.

    1) Craig I found your advice really helpful and today I tried for the first time the auto bed leveling functionality given by bCNC. The results are outstanding (see the attached pictures). Bed leveling is for sure a really important step I was missing. I have already milled one small test board with one of my cheap V-bits 30°/0.1mm (better results) and now I am milling the "larger board". I will post the results probably tomorrow.

    2) Blinkenlight I used your idea with the scotch-brite and the board shown in "cheap_v_bit.jpg" looks much better. However, the quality is not good enough for what I want. Right now I am trying with the 30°/0.1mm and it works better.

    3) CitizenOfDreams thank you for your reply. Unfortunately I have not received my dial indicator yet. The runout on these cheap spindles must be incredibly high. Maybe this is the reason why I noticed the worst results with the V-bit 30°/0.2mm as Craig mentioned already.

    For all the boards uploaded till now I use 20mm/min feedrate and 30V (~10-12k RPM but not verified yet) to the terminals of the spindle.

  8. #8
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    while I use 0.5mm endmills mostly, I do use engraving bits when I require finer intertrack spacings than can be achieved with an endmill.

    My experience is those cheap 10-15-30 degree 0.1mm engraving tools are rubbish, the tip breaks almost instantly and the cut is rubbish.
    Try 45 or 60 degree bits, say 0.2mm, they are much more robust.

    I get these from the same supplier of my 0.5mm endmills. Note they are actually double the price of the endmills, but they have proven to have good cut
    quality and last for 10-12 hours cutting.

    https://www.ebay.com/itm/60-DEGREE-M...72.m2749.l2649

    Craig

  9. #9

    Join Date
    May 2020
    Posts
    12
    Quote Originally Posted by joeavaerage View Post
    Hi,
    while I use 0.5mm endmills mostly, I do use engraving bits when I require finer intertrack spacings than can be achieved with an endmill.

    My experience is those cheap 10-15-30 degree 0.1mm engraving tools are rubbish, the tip breaks almost instantly and the cut is rubbish.
    Try 45 or 60 degree bits, say 0.2mm, they are much more robust.

    I get these from the same supplier of my 0.5mm endmills. Note they are actually double the price of the endmills, but they have proven to have good cut
    quality and last for 10-12 hours cutting.

    https://www.ebay.com/itm/60-DEGREE-M...72.m2749.l2649

    Craig
    The first milling I tried was with something like this one:

    https://m.aliexpress.com/item/2037306745.html?trace=wwwdetail2mobilesitedetail

    I had a pretty clean cutout. For the first 15 secs... Then it just broke.
    The one you mention seems really good and it looks similar to the one we use in the LPKF milling machine we have in our university. They call it micro cutter and has a variable cutting width 0.2-0.5mm. I am going to order one for 14€ but this is almost twice the price I gave for the Stepcraft's V-router with which I had these great results shown in the first picture I posted. I hope that from now on, with autolevelling step added before milling, the bit's life will substantially increase.

    I will continue the tests and report the results.

  10. #10
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,

    I am going to order one for 14€ but this is almost twice the price I gave for the Stepcraft's V-router with which I had these great results
    Yes they are expensive, the only reason I got them was because I was already ordering a bunch of other stuff from the same supplier and just added a few of them
    to try them out. I'm impressed, but that is not to suggest that they are the only good ones out there. I suspect any decent 60 degree cutter would outperform
    the cheap 30 degree ones I had been using.

    Craig

  11. #11
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    Quote Originally Posted by joeavaerage View Post
    Hi,
    0.2mm is too incredibaly fragile, you'll break them before they wear out.
    Oh, I expect there might be trouble like that, but I'd still like a test. The V-bits I'm using are already 0.2mm at the tip after all and they don't break all _that_ often - and these cylindrical ones are basically V-bits too except for the absolute last half a millimeter or so: https://www.ebay.com/itm/0-2MM-Diame...torefresh=true
    I mean they might still break more often, but it seems to be worth a try. Those who scorn PCB milling never fail to point out how I can order some oh-so-very-cheaply (at about $10 cost plus another $10 shipping) so if one of these lasts more than half a PCB I've already broken even.

  12. #12

    Join Date
    May 2020
    Posts
    12

    Re: How to avoid premature tool failure

    First results with bed leveling. Here you can see a "test_board" milled with a cheap V-bit 30°/0.1mm. The spindle is running at 26V (~9000 rpm) with less vibrations. Feeding speed remains at 20mm/min. The board is actually good enough for what I want (test_board_06.jpg) but probably it is not a 0.1mm V-bit as advertised and/ or my spindle has a pretty high runout.

    In the following experiments I will set the V-bit tip diameter in FlatCAM to 0.15 or 0.2 mm. Yesterday I stopped the milling process of the "larger_board" because the cutting depth was inconsistent throughout the board area. I believe that was due to the lack of decoupling capacitors in my z-probe circuit. I added 10nF and 100pF decoupling capacitors and now the auto leveling process seems more accurate. Right now I am milling the "larger board" (cheap V-bit 30°/0.1mm | 26V ~9000 rpm | Fixed auto leveling) and I will post the results later.

    Blinkenlight what type of oil you use on the surface of the PCB while cutting?

  13. #13
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    how are you holding the PCB blank down? If you use clamps or screws around the peripherary of the board
    you will 'pull' a bow or warp into the board. When the tool cuts the board the board will move, negating the effort you
    took to probe the blank.

    Try double sided tape to hold the board down.

    Craig

  14. #14
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    Quote Originally Posted by mantalos View Post
    Blinkenlight what type of oil you use on the surface of the PCB while cutting?
    Oh, nothing special - some sort of generic, quite thin and runny "light machinery oil" or whatever it's called. The label fell off long ago...

    I'm a bit puzzled by your pics though - I seem to be getting better results than that (with the method I described) on my bog-standard 3020 and bog-standard cheap Chinese 0.2mm v-bits; one of my older pics: https://www.cnczone.com/forums/attac...0&d=1484955533

    Okay, these are post-scotch-brite, but still, wtf...

  15. #15

    Join Date
    May 2020
    Posts
    12
    Quote Originally Posted by joeavaerage View Post
    Hi,
    how are you holding the PCB blank down? If you use clamps or screws around the peripherary of the board
    you will 'pull' a bow or warp into the board. When the tool cuts the board the board will move, negating the effort you
    took to probe the blank.

    Try double sided tape to hold the board down.

    Craig
    I use a hot glue gun to attach the board on a larger piece of mdf which is also glued down to the cnc bed.

  16. #16

    Join Date
    May 2020
    Posts
    12
    Quote Originally Posted by blinkenlight View Post
    Oh, nothing special - some sort of generic, quite thin and runny "light machinery oil" or whatever it's called. The label fell off long ago...

    I'm a bit puzzled by your pics though - I seem to be getting better results than that (with the method I described) on my bog-standard 3020 and bog-standard cheap Chinese 0.2mm v-bits; one of my older pics: https://www.cnczone.com/forums/attac...0&d=1484955533

    Okay, these are post-scotch-brite, but still, wtf...
    Hmm interesting... What is the trace width in your boards? I used 8 mil (up) and 10 mil (down) traces respectively.

  17. #17
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi
    the issue is not trace widths but rather intertrack spacings.

    I commonly use 0.4mm (10 mil) as signal trace widths and have used 0.2mm (5 mil). One advantage of using two flute endmills
    is the clean cut and no trace thinning with depth that happens with a V bit. Thus I can use 0.2mm quite reliably but still prefer 0.4mm
    as being easier if PCB space is not constrained.

    Using 0.5mm endmills however means the intertrack spacing must be at leat 0.5mm (12.7 mil), and I allow 0.6mm (15 mil)
    as it allows the software to generate a tool path that passes as a minimum twice between pins/traces.

    0.6mm between traces is adequate for SIOC IC's but insufficient for finer pitches like quad flat packs. Then I am constrained to
    use a V bit.

    Having said that I've got my procedures down pat and very seldom do I break a 0.5mm endmill and I guess now that I have the
    experience to use even smaller endmills. I had and used and eventually broke 10 of 0.4mm endmills, and I have and use some
    0.3mm carbide drills. The drills being longer are very VERY fragile, I don't like using them much as they break almost by looking at them.

    Craig

  18. #18
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    Quote Originally Posted by mantalos View Post
    Hmm interesting... What is the trace width in your boards? I used 8 mil (up) and 10 mil (down) traces respectively.
    The traces are 16mil (0.4mm) and the tightest inter-track clearance is 8mil (0.2mm) which means that at ideal cutting width my 0.2mm v-bit can just about pass once between tracks (can't be less, or the software freaks out not being able to pass through there and just leaves stuff connected). In real life the milled slot is wider of course due to the v-tip, making the trace narrower - it's easily visible that the slot is more than half as wide as the trace...

  19. #19
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    Quote Originally Posted by joeavaerage View Post
    I commonly use...
    There's... something wrong with those conversions. Which numbers are the real ones?

  20. #20
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    my apologies, my conversion to mil was incorrect.

    0.2mm trace= 8mil
    0.4mm =16mil
    0.6mm=24mil

    tightest inter-track clearance is 8mil (0.2mm) which means that at ideal cutting width my 0.2mm v-bit can just about pass once between tracks (can't be less, or the software freaks out not being able to pass through there and just leaves stuff connected).
    That is my point, its the minimum inter-track or inter-pin spacings that determine the success or otherwise of your board.
    While its possible to end up with a track thinner by virtue of a V bit, it would have to be pretty poor cutting procedure to thin a track
    that much that it was discontinous. On the other hand if you are not careful the it is VERY possible for two tracks to NOT be isolated.

    For this reason I tend to decide right a the outset of my PCB design what my minimum inter-pin (inter-track) spacings have to be to use
    the IC's I want. That will determine the tool and procedures to be followed.

    If at all possible I use SOIC IC's that have 0.6mm inter-pin spacings which in turn allows me to use 0.5mm endmills for which I have
    a good supply and many hundreds hours experience in their use.

    Craig

  21. #21

    Join Date
    May 2020
    Posts
    12

    Post Re: How to avoid premature tool failure

    Hello,

    I finished milling the "larger_board". You can see the results in the attached picture.

    Settings:

    1) Feeding speed = 20mm/min
    2) Spindle at 22V (~7333 rpm)
    3) Tool: Cheap V-bit 30°/0.1mm
    4) Milling depth 50 um
    5) In FlatCAM I set the tool tip to 0.2mm to get good results. Probably this is needed because my tool is not actually a 0.1mm tool and/ or my spindle has a huge runout.
    6) 4 passes 40% overlap
    7) Auto leveling using bCNC.
    8) Added some sunflower oil on the blank pcb board. This was just an experiment because I didn't have any cutting fluid and it seems that it helped!

    In this board I use 10 mil tracks. The smallest isolation distance is 0.2 mm (pad to pad for the TSSOP chip).
    I edited the gcode and removed 3 out of the 4 board outlines to accelerate the milling. However, I forgot to remove a gcode command for the z axis and the machine milled a huge straight line throughout the board.
    Other than that, the improvement is obvious with respect to the "cheap_v_bit.jpg?" I uploaded in the first post. What is your opinion?

  22. #22
    Registered
    Join Date
    Nov 2012
    Posts
    139

    Re: How to avoid premature tool failure

    Yup, that looks pretty good... Results look quite nice for the TSSOP chip - I don't even go below SOIC typically (which I know for sure I can mill without issues) or preferably even use DIP - size tends to not matter that much for me and DIPs either let me pass a track between pins (very useful on a single-side PCB) or offer a free "via" (if I decide to bother with double-side registration).

    I'm sure there's room for experiments with other milling bits or even another spindle, but it looks like you've reached what a 3020/6040 should be able to do.

  23. #23
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    that is a marked improvement but is still pretty raggedy.

    I suspect your spindle has too much runout to do a good job. I would suugest you look to improve your machine with a 24000 rpm
    spindle. They (usually) have angular contact bearings and will bring the runout down to 5um or so. You don't need alot of power
    for PCB's, 750W is more than enough. If you want to do wood or aluminum then consider 1.5 -2.2kW.

    The Chinese made spindles are pretty good....for the money.

    I use this one from Germany:

    https://www.mechatron-gmbh.de/filead...08-24-ER11.pdf

    Craig

  24. #24

    Join Date
    May 2020
    Posts
    12

    Re: How to avoid premature tool failure

    Quote Originally Posted by joeavaerage View Post
    Hi,
    that is a marked improvement but is still pretty raggedy.

    I suspect your spindle has too much runout to do a good job. I would suugest you look to improve your machine with a 24000 rpm
    spindle. They (usually) have angular contact bearings and will bring the runout down to 5um or so. You don't need alot of power
    for PCB's, 750W is more than enough. If you want to do wood or aluminum then consider 1.5 -2.2kW.

    The Chinese made spindles are pretty good....for the money.

    I use this one from Germany:

    https://www.mechatron-gmbh.de/filead...08-24-ER11.pdf

    Craig
    Craig, you are right the results were not perfect. I will consider buying a new spindle. The one you suggested seems really good but it is too expensive for me right now. Do you think this one from aliexpress would be OK for milling aluminum?

    https://www.aliexpress.com/item/3280...175b2e0e5X0dtn

    Today I milled another "larger board" and I think the results are much better (see the attached pictures). Here are the settings:

    1) Feeding speed = 20mm/min
    2) Spindle at 22V (~7333 rpm)
    3) Tool: Brand new cheap V-bit 30°/0.1mm. The one used in the last board was also used for three other failed milling jobs and it seems it wasn't as sharp as a new one.
    4) Milling depth 60 um
    5) In FlatCAM I set the tool tip to 0.2mm to get good results. From the results in this board probably a value of 0.15mm would be better.
    6) 4 passes 40% overlap
    7) Auto leveling using bCNC. In this case I used a much more dense auto level grid. Auto level probe speed set to 5mm/min.
    8) Sunflower oil on the blank pcb board.
    9) Used a single sided blank board of better quality.

    Also, I didn't have to scrub the board. Total milling time of 4 hours. The results are actually comparable (quality not speed of course) with the $20k LPKF's ProtoMat S64 that we have in our university. What do you think?

  25. #25
    Registered
    Join Date
    Nov 2013
    Posts
    872

    Re: How to avoid premature tool failure

    Hi,
    yes that spindle has enough power to cut aluminum, but is your machine rigid enough?

    Many have tried cutting aluminum and other metals only to find that their machine is not rigid enough and
    therefore cant cut metals worth a damn.

    Can you post your code for the test board an I'll try to cut it and post the pics.

    Craig

Page 1 of 2 12

Similar Threads

  1. how do you avoid tool pull out ?
    By deadlykitten in forum Okuma
    Replies: 13
    Last Post: 07-07-2017, 02:20 PM
  2. Premature pinion wear
    By MechanoMan in forum CNC Router Parts
    Replies: 4
    Last Post: 03-27-2015, 04:29 PM
  3. Replies: 2
    Last Post: 10-17-2013, 07:33 PM
  4. Replies: 2
    Last Post: 04-03-2012, 08:59 AM
  5. Premature Ebay-ulation?!? (single Z axis linear rail)
    By braidmd in forum Linear and Rotary Motion
    Replies: 4
    Last Post: 11-06-2007, 05:08 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •