593,377 active members*
8,119 visitors online*
Register for free
Login
IndustryArena Forum > WoodWorking Machines > DIY CNC Router Table Machines > Bobs CNC Evo 4 - Feed n Speeds problem
Results 1 to 16 of 16
  1. #1
    Join Date
    Oct 2024
    Posts
    6

    Angry Bobs CNC Evo 4 - Feed n Speeds problem

    Hello,

    I cannot get the feeds & speeds right on my Evolution 4 to save my life.

    I'm using a 1/4" 2 flute end mill and using the speeds directed exactly as the Bob's "Speed and Feed Calculator" describes. I've tried two different bits, thinking maybe one was dull (it feels sharp, though). I'm just on a piece of scrap that I believe is pine (chatgpt says the same).

    I'm exporting using the BobsCNC mm processor (machine is set to mm). The only thing I could think of is that somehow units are off, but I don't think so. I'm running the code with UGS to the machine. Zero'd on center of piece and using touch plate.

    See video:


    Have a closer-up pic of when I first started as well.

  2. #2
    Join Date
    Oct 2024
    Posts
    6

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    (Is there no way to edit threads?)

    UPDATE:

    I got it to work by forcing a 50% feed override (slow down by half) and bumping the speed up... but this is like 1/4th the proper chip load. I don't get it? Even then, it still sounds like it wants to catch once in a while, but it seems to work.

  3. #3
    Join Date
    Jul 2018
    Posts
    6664

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Hi JMS - what are your actual F&S? By the look of the cut your machine is not stiff enough to hold the cut. The tool is moving sideways which means the machine is flexing. No you have 60mins to edit I think then that entry its set in stone. Peter

  4. #4
    Join Date
    Dec 2003
    Posts
    1292

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    With that much depth of cut on a lightweight machine,the logical adjustment is to reduce the depth of cut drastically and compare the outcome.Maybe try conventional cutting instead of climb cutting as well.

  5. #5
    Join Date
    Oct 2024
    Posts
    6

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    I've tried a bunch of different settings at this point, but I believe I was running the following settings with the 40-50% override (see screenshot).

    The other difference being I bumped up the RPMs higher, thus why I think I was about 1/4th proper chip load. (2x feed slowdown and a little over 3 on the rpm's making it probably ~18000 so about a 50% increase there as well).

    If anyone has any recommendations on the "proper" way to test and figure it out, please let me know. The fact that the exact settings the manufacturer recommends even with the exact same equipment not working is driving me nuts.

  6. #6
    Join Date
    Mar 2010
    Posts
    622

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Have you checked the spindle rotation yet?
    Gecko G540, Rack and Pinion Drives-X and A axis, 1/2-10 5 Start Acme-Z Axis
    4-THK HSR 25 Linear Slides, KL23H2100-35-4B, Power Supply-KL-600-48 48V

  7. #7
    Join Date
    Oct 2024
    Posts
    6

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    It uses a Makita 0701c, so speed is set manually by a dial. I'm unsure how to check the rotation as it's not controlled by and doesn't report to software.

  8. #8
    Join Date
    Jul 2018
    Posts
    6664

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Hi JMS - Lets work thru this 1) the recommended feed is 186in/min (4700mm/min) this is fast - at 14500rpm and 950ft/min which is 289m/min. Its a 2F tool so the chipload is 0.16mm or 0.0064". This is too big a bite I feel for that small machine. Aim at 0.05mm The surface speed at 289m/min is OK I aim at 300m/min max. Now Chip size per tooth is = feed/rpm/N So to make the CL or Fz 0.05 you can run the feed at say 1500mm/min/14000rpm/2 teeth= 0.05mm or 0.0020inches. Start there. Once you find the max Fz that works stay there! do not fiddle with this number. Always set your F&S to achieve that bite size. Now the DOC is related to the power available from the spindle and the ability of the tool to expel the chip. Use the deepest DOC possible to minimise the bending of the tol and maximis tool life. The BOCBS chart recommends 0.5D which means you will wear out half of your tool fast. try 1D DOC or more and see how you go once you have sorted the Fz. Hope this makes sense. Peter

    do not randomly speed up or slow down feeds and speeds. Always understand what chip thickness you are cutting at. The chip thickness is the real deal.... Use a 1FR tool with a machine that is not rigid you are probably cutting on onje tooth rubbing on the other. A 1F tool means its always cutting... Then there's runout to consider. I always found the Makita to be pretty good but really noisy... Peter

  9. #9
    Join Date
    Dec 2003
    Posts
    1292

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    I believe we are using different words to describe matching the DOC to the rigidity of the machine as that is more of a weak spot than the spindle power available.I would be surprised if the spindle rotation isn't clockwise and the steppers appear to have sufficient power to move the machine.

  10. #10
    Join Date
    Jul 2018
    Posts
    6664

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Hi Routalot - No I think we understand what DOC is. The image published shows the tool moving sideways under the cutting loads. To me this says 1) the machine is not stiff enough to control that cut 2) If the cut is Fz-0.16mm then that's a heavy chip and the machine is digging into the material. hence the sideways moving tool. 3) deep DOC only exaggerates this digging in of the tool. Its either blunt, totally wrong Fz, tool is choking etc 4) I'm sure the Makita has enough power to do the cut given the right conditions, I abused a makita for a couple of years and was surprised by how well it did. You can't run a Makita backwards. I suppose you could program the feed the opposite way. So JMS what is the direction of feed in the sample image? Is the tool feed moving clockwise or anticlockwise? around the rectangle? Peter

  11. #11
    Join Date
    Dec 2003
    Posts
    1292

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    I have every faith in Makita tools,although I haven't found any small 1/4" router that isn't noisy!I agree with your analysis of the aspects that are leading to the misfortune and I have no doubt that if the tool is sharp,the weak link is the machine structure.Obviously there is a linear relationship between the forces imposed by cutting and the depth of tool engagement,which is whhy I suggested a major reduction until a good cut is achieved.At which point cautiously increasing the depth can begin.I'm always wary of hobby machines being loaded with the cutting parameters that would be ideally suited to high output commercial machines.Compromise may be necessary.

    In the video posted,which i had to view on youtube,the cut is clearly a climb cut and it seemed to be an oak,or similar,species being cut.The gantry beam was clearly flexing at the time of the most severe deflections and it seemed to be happening while the end grain was being cut.I'm not sure how you would reinforce the gantry beam and I suspect that it would be the first step in chasing a series of weak spots until the machine was coping with the loads that are being imposed by the chosen cutting parameters.A known sharp tool would be the easy first step.

  12. #12
    Join Date
    Jul 2018
    Posts
    6664

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Hi JMS - couldn't get the video to work before but it works now. Definitely lack of machine stiffness for that cut. If the machine was stiff enough the Makita would stall or burn the timber.... I have a small router that does exactly the same and had to rebuild it to improve the Z stiffness and the gantry stiffness. Reduce DOC as routealot (like Lancelot I suppose) has suggested and review Fz start small and work up... Peter

  13. #13
    Join Date
    Oct 2024
    Posts
    6

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    I appreciate the help, guys. I'm nearly at my wits' end.

    Today I took a scrap piece and ran back and forth with bits are varying speeds & depths to figure out what seemed to be the best settings. I first tightened down the Y-axis belts as well as a bit of adjustment to the gantry (has less wobble now). This is what I came up with... To be clear: these numbers still seem wrong to me. I feel like I'm having to move incredibly slow/very low depth of cut just to keep it from having problems.

    1/8th" 4 Flute Upcut EM: 1300 mm/min, 1.5mm DOC, 10K RPM
    1/16th" 4 Flute Upcut EM: 1300 mm/min, 1mm DOC, 12K RPM
    1/4th" 1 Flute Upcut EM: 1100 mm/min, 1mm (!!!) DOC, 10K RPM
    1mm radius ball: 1100 mm/min, 1mm DOC, 10K RPM

    After thinking I finally had "good" settings, I proceeded to try a small project on a clean piece, only for it to continue to catch and gouge the wood using the 1/4th" bit at only 1mm depth. This is driving me crazy. The pics below are from this run.

    I really am not sure what's wrong--I should be around 0.5 bit diameter for depth if I understand it correctly. I also feel like I'm moving too slow and the chips are too small, but if I try to speed up I immediately run into problems.

  14. #14
    Join Date
    Jul 2018
    Posts
    6664

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    looking at the 1/4" setting 1100/10,000/1= 0.11mm Fz. I think it's your machine stiffness or lack of it, try 0.05mm chip load so 600/10000/1=0.06mm
    1/8" tool 1300/10,000/4= 0.0325mm too small
    1/16" 1300/12000/4 = 0.027mm too small

    so if these don't work it comes back to machine compliance...

    If the chip is too small then the tool rubs vs cuts as the tool gets pushed away from the surface when it tries to cut. If the chip is too big the tool chokes. Surface speeds at 10-12k rpm are fine. If you try conventional cutting ie the chip is thin to start and gets thicker and its the same result then its definitely machine compliance. The machine has to be stiff to start a thin cut. Some images of your machine maybe helpful. Peter

  15. #15
    Join Date
    Dec 2003
    Posts
    1292

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    I will make a suggestion that isn't closely related to the machine;give some thought to getting hold of a USB microscope.The are quite inexpensive at the lower end of the market and these are quite good enough for taking a very close look at cutting edges.If you can see any kind of an edge-the tool is blunt.My more traditional test is to drag the tool along a thumbnail to see if a tiny shaving is lifted off but the ability to see is perhaps more useful.

  16. #16
    Join Date
    Oct 2024
    Posts
    6

    Re: Bobs CNC Evo 4 - Feed n Speeds problem

    Appreciate the feedback about the microscope--it's an interesting idea and I have to look into that. In the meantime, this is a brand new blade and seems plenty sharp.

    I may have at least narrowed down the problem:

    With all this cutting I was getting annoyed and decided to create something of a jig in which I place the work piece against each time. You'll know what I mean as soon as you see the screenshot. Anyways, while cutting this the following happened:

    - No problems with the circle pocket.

    - #1 is a climb cut and seemed OK, but once in a while I heard a slight sound that made me start to believe the X-position wasn't perfectly aligned as it ran north/south on the Y-axis. It seemed to me like it was rubbing slightly on the left-hand side as it went north (Y+).

    - #2. The east/west (x-axis) pocket is a conventional cut and where the trouble hit. It got about 50-75% or more through the depth without issues and then suddenly on a east (+x) pass it just completely rubbed against the north side. It obviously had a bunch of the bit engaged depth-wise and was bouncing/etc. You can see how that side is chewed up in the pic.

    So at this point I took a break, then cleaned all the rollers/rails/checked belts/etc. thinking that the x/y isn't being accurate and causing this problem.

    Now what's really weird... I have this zeroed on 25mm/25mm. I can home and then go to 25/25 and always be on zero for the jig, at least that's the idea. When I ran it again, the east/west pocket was being cut at the wrong diameter. It was a little thinner than expected. The board did not move. It wasn't off on the zero (for ex, Y-axis) because it would have cut too much into the south side, which it didn't. Both north and south sides of that channel are inwards more than expected.

Similar Threads

  1. Feed and Speeds for CNC Machine (Plywood)
    By maudib32 in forum WoodWorking Topics
    Replies: 6
    Last Post: 08-13-2023, 10:42 PM
  2. How CNC lasers manage such high feed speeds?
    By Nikolaguca in forum DIY CNC Router Table Machines
    Replies: 2
    Last Post: 06-01-2020, 01:54 AM
  3. New To cnc Routing. Part hold down? feed speeds?
    By troyerscnc in forum WoodWorking Topics
    Replies: 5
    Last Post: 05-23-2013, 05:41 PM
  4. Speeds and Feed rates for acrylic in a CNC mill
    By tremx in forum Glass, Plastic and Stone
    Replies: 8
    Last Post: 11-06-2012, 06:22 AM
  5. feed speeds cnc shark
    By vanstone in forum Commercial CNC Wood Routers
    Replies: 2
    Last Post: 12-24-2010, 03:08 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
  •