584,814 active members*
5,252 visitors online*
Register for free
Login
Results 1 to 8 of 8
  1. #1
    Join Date
    Nov 2019
    Posts
    8

    CNC cuts 0.4mm out

    Hello, I have a 3040 CNC machine, and I am cutting some CNC clamping plates 50 x 20 x 4.6mm acrylic. There is a slot in it, 20 x 6mm, starting 10mm from one end.

    The drawing was made in AutoCAD, imported into Aspire Ver 10.5, and the toolpath created with a brand new 1/8" milling bit with 2 flutes, fed 300mm/min and with 0.95mm depth of cut with 5 passes.The G.Code is sent to the UGS Platform on Win 10 64 bit running with 8 GB RAM and 2.5 -3.0 GHz CPU.

    When I cut it the overall result each time is the outer dimensions are 0.4mm too large in each X and Y direction, and the slot dimensions are 0.4mm too small.

    I have put my 0-10mm dial gauge on both the X and the Y axis, and when jogging the spindle 10mm, coming from 20mm out to eliminate backlash, the dial gauge readings give 10.05mm maximum in either direction.

    Can you please suggest how I can get these cuts more accurate? I need the slot to take a M6 bolt

    My kind regards,

    Jill

  2. #2
    Join Date
    Jan 2013
    Posts
    474
    Quote Originally Posted by JillB99 View Post
    Hello, I have a 3040 CNC machine, and I am cutting some CNC clamping plates 50 x 20 x 4.6mm acrylic. There is a slot in it, 20 x 6mm, starting 10mm from one end.

    The drawing was made in AutoCAD, imported into Aspire Ver 10.5, and the toolpath created with a brand new 1/8" milling bit with 2 flutes, fed 300mm/min and with 0.95mm depth of cut with 5 passes.The G.Code is sent to the UGS Platform on Win 10 64 bit running with 8 GB RAM and 2.5 -3.0 GHz CPU.

    When I cut it the overall result each time is the outer dimensions are 0.4mm too large in each X and Y direction, and the slot dimensions are 0.4mm too small.

    I have put my 0-10mm dial gauge on both the X and the Y axis, and when jogging the spindle 10mm, coming from 20mm out to eliminate backlash, the dial gauge readings give 10.05mm maximum in either direction.

    Can you please suggest how I can get these cuts more accurate? I need the slot to take a M6 bolt

    My kind regards,

    Jill
    So basically you have an 0.2mm positional error when circular interpolation and the opposite error if cutting the slot.

    It looks like a problem with cutter compensation. Have you tried test cuts with comp off ?

  3. #3
    Join Date
    Nov 2019
    Posts
    8

    Re: CNC cuts 0.4mm out

    Thanks for your reply, servtech. I am a newby to CNC. Where do I find cutter compensation please? I have never heard of it before

  4. #4
    Join Date
    Jan 2005
    Posts
    15362

    Re: CNC cuts 0.4mm out

    Quote Originally Posted by JillB99 View Post
    Thanks for your reply, servtech. I am a newby to CNC. Where do I find cutter compensation please? I have never heard of it before
    Cut / paste your Program as text here, if you are new, you won't be using cutter compensation, so don't get confused with it.

    To get you started so you can have a useable part, just trick the control, until you get this figured out, so in your cam program change the tool diameter, but use the same .125 cutter so when you select the tool in your cam program from .125, give it a diameter of .1094 and reprocess using this diameter, this should give you close to the correct size you are wanting, using the same tool.

    This could be a setup problem with your control or cam as to how it is seeing your cutter diameter.

    Another thing to check is you are using inch measurement for your cutter and mm for your control. it could be just a simple code missing if it is programed in inches and your machine is setup as metric, you will have to use a G20 at the start of an Inch program and a G21 for a metric program

    So, if you are using an inch postprocessor you will need a G20 at the top of your program. if you are using a metric post processor then you will need a G21 at the top / start of your program.
    Mactec54

  5. #5
    Join Date
    Jan 2013
    Posts
    474
    Quote Originally Posted by mactec54 View Post
    Cut / paste your Program as text here, if you are new, you won't be using cutter compensation, so don't get confused with it.

    To get you started so you can have a useable part, just trick the control, until you get this figured out, so in your cam program change the tool diameter, but use the same .125 cutter so when you select the tool in your cam program from .125, give it a diameter of .1094 and reprocess using this diameter, this should give you close to the correct size you are wanting, using the same tool.

    This could be a setup problem with your control or cam as to how it is seeing your cutter diameter.

    Another thing to check is you are using inch measurement for your cutter and mm for your control. it could be just a simple code missing if it is programed in inches and your machine is setup as metric, you will have to use a G20 at the start of an Inch program and a G21 for a metric program

    So, if you are using an inch postprocessor you will need a G20 at the top of your program. if you are using a metric post processor then you will need a G21 at the top / start of your program.
    He is using a post, inputting tool data. My point is the POST could be putting cutter compensation on and off in generating the program, confusing the newbie.

  6. #6
    Join Date
    Jan 2005
    Posts
    15362

    Re: CNC cuts 0.4mm out

    Quote Originally Posted by servtech View Post
    He is using a post, inputting tool data. My point is the POST could be putting cutter compensation on and off in generating the program, confusing the newbie.
    No, the software being used to generate the G-Code does not support Cutter Compensation, so it won't be posted in his program, it helps if you understand what the cam software being used is.
    Mactec54

  7. #7
    Join Date
    Nov 2019
    Posts
    8

    Re: CNC cuts 0.4mm out

    Thanks for the suggestions above. Today I cut the acrylic CNC clamp plate with a Conventional Cut ( not climb cut) as suggested above and the error reduced from 0.4 to 0.18mm. I.e, the dimensions of the inner slot were 0,18 too small in both length and width, and the dimensions of the outer rectangle were 0.18mm too big in both length and width.

    I checked the accuracy of the X & Y stepper motors by jogging 10mm and measuring the distance travelled. In each case the distance was 10.01mm, measured by a high quality dial gauge.

    Ooops , forgot to mention, the 1/8" ( 3.175mm) cutter actually measures 3.15mm

    Can anyone please suggest why the difference in climb cutting and conventional cutting?
    Also, is there anything else I should check for accuracy in the X and Y directions?


    Finally, how do I remove the 0.18mm error without cutter compensation? It would appear that I need to add cutter compensation of 0.18mm/2 =0.09mm

    Incidentally, Aspire Ver 10.5 certainly does have allowance for cutter compensation to make the cut bigger or smaller

    kind regards,
    Jill
    Attached Thumbnails Attached Thumbnails cncclamp plate.JPG  

  8. #8
    Join Date
    Jan 2005
    Posts
    15362

    Re: CNC cuts 0.4mm out

    Quote Originally Posted by JillB99 View Post
    Thanks for the suggestions above. Today I cut the acrylic CNC clamp plate with a Conventional Cut ( not climb cut) as suggested above and the error reduced from 0.4 to 0.18mm. I.e, the dimensions of the inner slot were 0,18 too small in both length and width, and the dimensions of the outer rectangle were 0.18mm too big in both length and width.

    I checked the accuracy of the X & Y stepper motors by jogging 10mm and measuring the distance travelled. In each case the distance was 10.01mm, measured by a high quality dial gauge.

    Ooops , forgot to mention, the 1/8" ( 3.175mm) cutter actually measures 3.15mm

    Can anyone please suggest why the difference in climb cutting and conventional cutting?
    Also, is there anything else I should check for accuracy in the X and Y directions?


    Finally, how do I remove the 0.18mm error without cutter compensation? It would appear that I need to add cutter compensation of 0.18mm/2 =0.09mm

    Incidentally, Aspire Ver 10.5 certainly does have allowance for cutter compensation to make the cut bigger or smaller

    kind regards,
    Jill
    You have to check the steps / per over a longer distance 10mm is not going to tell you much, you need at least 75mm or more is better I use 300mm when setting up axis Steps / per.

    If it cut better conveniently then you have some flex in the machine most likely the Z axis, to test this setup your dial gauge against the cutter then put some pressure on the Z axis in a twisting motion.

    Your cutter does not sound like it is very good quality, a poorly ground cutter will push away instead of cutting, try 3 flute also.

    To get the size you want adjust your cutter size in Aspire.

    Good to know Aspire now supports cutter comp. I knew they were working on it.

    You can also adjust your drawing size if you don't want to change the cutter geometry size or use cutter comp.
    Mactec54

Posting Permissions

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