need help milling large dia
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default need help milling large dia

    hey all, im making a section of a 60" dia "L" shaped bracket. ive triple checked my mastercam drawing and tool parameters. the issue is the outside dia is coming in .231 undersize and the inside dia is .353 undersize. ill post the program, the math doesnt seem right

    N2 G0 G17 G40 G49 G80 G90
    ( 1/2 ENDMILL SHARP CORNER FINISH OUTSIDE )
    N3 T3 M6
    N4 G0 G90 G54 X-7.6686 Y.5384 S1350 M3
    N5 G43 H3 Z.2 M8
    N6 G1 Z-.78 F50.
    N7 G41 D3 X-7.5476 Y.0533 F8.
    N8 G2 X7.5476 I7.5476 J-30.2718
    N9 X7.7297 Y-.2498 I-.0605 J-.2426
    N10 G1 X7.5991 Y-.7737
    N11 G2 X7.296 Y-.9558 I-.2426 J.0604
    N12 G3 X-7.296 I-7.296 J-29.2627
    N13 G2 X-7.5991 Y-.7737 I-.0605 J.2425
    N14 G1 X-7.7297 Y-.2498
    N15 G2 X-7.5476 Y.0533 I.2426 J.0605
    N16 G1 G40 X-7.6686 Y.5384
    N17 G0 Z.2
    N18 M5
    N19 G91 G28 Z0. M9
    N20 G28 Y0.
    N21 M30

  2. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,021
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2600

    Default

    probably a tool dia comp issue. line left and line right that is G41 and G42. obviously if using D3 what is the value in D3 ?? usually you compensate for radius / dia of cutter or you use wear comp from theoretical max size of cutter. that is selected in mastercam usually. also is D3 in radius or dia and what is needed. that is does D3 need to be .250 or .500 for a 1/2"dia end mill. different machines expect radius and others in diameter
    .
    or you somehow messed up selection arc or circle

  3. #3
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    916
    Post Thanks / Like
    Likes (Given)
    390
    Likes (Received)
    284

    Default

    can you post the mastercam file?

  4. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,021
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2600

    Default

    i have also seen where G17 G18 G19 or plane selected when incorrectly given messed up tool comp. usually G17 is used but 5 axis machines often G18 or G19 is used

  5. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,496
    Post Thanks / Like
    Likes (Given)
    4101
    Likes (Received)
    2663

    Default

    What is your comp set to in Mastercam? Control? Wear?

  6. #6
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    D3 is wear comp..should start at zero. they are undersized by different amounts which is perplexing, but all the other dims are in besides the bolt circle which is also .375 too small. it may be my cmm having a hard time on such a small portion of the dia. i making a section that is 28 deg of the whole circle(about 15" long)

    my program has the same noemclature they have had for 10 years, nothing differnt.

    the way i drew my drawing was creating the 60" circles then segmenting 28 deg then moves everything to origin in mastercam. ive check the dias in the mcam file thay are spot on.

    N8 G2 X7.5476 I7.5476 J-30.2718-----this here is where the tool makes the arc on the outside. the J-30.2718 should be 1/2 dia(61.897/2=30.9485+.250(1/2 tool)=31.1985..Right????? but the starting Y is not zero tho it shoudnt matter??

  7. #7
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    tab.jpg this is after backplot

  8. #8
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,042
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    1015

    Default

    When I plot the end points of your OD arc along with the center of the arc I get R31.25
    For your ID arc I get R29.232

  9. #9
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,021
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2600

    Default

    might be more a measuring problem.
    .
    but also cnc dro calibration that is have you measured when you moved 10.0000 using a gage block against stop and indicator and zero dro and remove gage block to travel til indicator is zero at stop what does dro say ?
    .
    that is you can move 9.995 but dro says you moved 10.0000. better machines have a calibration mode to fix dro errors. just something to check too.
    .
    also higher feed rates a cnc does not always track or move as accurately as when you travel at slower feed rates
    .
    just saying i have seen dro needing calibration before on each axis X and Y and Z

  10. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,496
    Post Thanks / Like
    Likes (Given)
    4101
    Likes (Received)
    2663

    Default

    Quote Originally Posted by tay2daizzo8 View Post
    tab.jpg this is after backplot
    I can draw it here at work and post my code for cutting the shape to see if mine is different, what is your OD,ID and angle per side if the segment?
    And the dia of the cutter you're using?

  11. #11
    Join Date
    Sep 2016
    Country
    UNITED KINGDOM
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    2

    Default

    We had a similar problem, we needed to put a linear move on as you put the comp on.
    Its under the lead-in lead-out settings. Worked for us.

  12. #12
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,637
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1426

    Default

    Quote Originally Posted by Booze Daily View Post
    When I plot the end points of your OD arc along with the center of the arc I get R31.25
    For your ID arc I get R29.232
    Hello Booze,
    How do you get those numbers? I get:
    OD = 31.1985 (30.9485 corrected for 0.25 Tool Rad)
    ID = 30.1585 (30.4085 corrected for 0.25 Tool Rad)

    Regards,

    Bill

  13. #13
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    Quote Originally Posted by Mtndew View Post
    I can draw it here at work and post my code for cutting the shape to see if mine is different, what is your OD,ID and angle per side if the segment?
    And the dia of the cutter you're using?
    .500 dia endmill 61.897 OD 60.817 ID 28 de total segment

    also shifted the center of the arcs down in Y -30.2185

  14. #14
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    Quote Originally Posted by Paul Hope View Post
    We had a similar problem, we needed to put a linear move on as you put the comp on.
    Its under the lead-in lead-out settings. Worked for us.
    i have a perpendicular lead in of .500.

    N7 G41 D3 X-7.5476 Y.0533 F8.

  15. #15
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    531
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    186

    Default

    Quote Originally Posted by tay2daizzo8 View Post
    i have a perpendicular lead in of .500.

    N7 G41 D3 X-7.5476 Y.0533 F8.
    Try this

    N2 G0 G17 G40 G49 G80 G90
    ( 1/2 ENDMILL SHARP CORNER FINISH OUTSIDE )
    N3 T3 M6
    N4 G0 G90 G54 X-7.6686 Y.5384 S1350 M3
    N5 G43 H3 Z.2 M8
    N6 G1 Z-.78 F50.

    G41 Y0.300 D3 F8.0 (LEAD BEFORE THE START POINT OF ARC)

    N7 G01 X-7.5476 Y.0533 F8.(TOOK OUT G41 HERE AND PUT IT ABOVE)
    N8 G2 X7.5476 I7.5476 J-30.2718
    N9 X7.7297 Y-.2498 I-.0605 J-.2426
    N10 G1 X7.5991 Y-.7737
    N11 G2 X7.296 Y-.9558 I-.2426 J.0604
    N12 G3 X-7.296 I-7.296 J-29.2627
    N13 G2 X-7.5991 Y-.7737 I-.0605 J.2425
    N14 G1 X-7.7297 Y-.2498
    N15 G2 X-7.5476 Y.0533 I.2426 J.0605
    G1 Y0.3 (LEAD OUT AFTER ARC)
    N16 G1 G40 X-7.6686 Y.5384

    N17 G0 Z.2
    N18 M5
    N19 G91 G28 Z0. M9
    N20 G28 Y0.
    N21 M30

  16. #16
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    531
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    186

    Default

    when your using a d offset as 0(tool centerline) instead of the tool dia you only need a few thousandths of lead in and lead out.
    if you use your D offset as a tool dia some machines you have to put the amount of tool offset and a tad more in the lead in.
    Hass and fadal you can get away with .01 .05 or what ever if your programing tool centerline ie tool offset 0

    your problem appears to be your g41 was right to the start point of the arc. you need a lead to the start point of the arc in which you didnt have.

  17. #17
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    i changed the program and added the extra move. ill let you know how it worked when its done in 3 hours.

  18. #18
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,042
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    1015

    Default

    Quote Originally Posted by angelw View Post
    Hello Booze,
    How do you get those numbers? I get:
    OD = 31.1985 (30.9485 corrected for 0.25 Tool Rad)
    ID = 30.1585 (30.4085 corrected for 0.25 Tool Rad)

    Regards,

    Bill
    Oops. I accidentally used J as the absolute coord of center instead of incremental distance to center.

  19. #19
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    762
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    288

    Default

    I was wondering what the material is and how big. Is it like in that screenshot you posted, made out of a solid bar? Is the material cold rolled?

    I didn't calculate radii or pay enough attention to whether it was indeed your cutter comp lead-in that may be causing it. But I do know that if you are cutting cold-rolled stock, it tends to go all wonky when cutting all around like that, especially something so long and thin.

    I'd make sure that you're leaving enough stock between roughing and finishing cycles. You will also want to make sure you strategically unclamp and reclamp the part after roughing, to allow it to spring/bow whichever way it wants to so when you finish it, it is more stable unclamped.

    I hope your issue is more cutter comp lead-in related and can be fixed by suggestions above. Otherwise you may want to look into this.

    I think that with any bowing issue on such a short segment of a large diameter like this, your CMM may throw you all kinds of wonky readings.

  20. #20
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    428
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    128

    Default

    right now the material is aluminum to set up on, but will eventually be a duplex stainless. Im beggining to think its my CMM some how because even the holes on the bolt circle are off

    yes im making it out of solid plate


Tags for this Thread

Bookmarks

Posting Permissions

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