584,860 active members*
5,065 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > G-Code Programing > Macro Programming for Taper Bore machining
Page 1 of 2 12
Results 1 to 20 of 31
  1. #1
    Join Date
    May 2008
    Posts
    157

    Macro Programming for Taper Bore machining

    I need to make macro program for machining a taper bore which also has a fillet at the top. Though this can be made with spiral option in many CAM softwares it does not yield desired results and i felt macro may be the solution as it has better control on such 2 1/2 D profiles. Can someone help ?

    thanks
    yaji

  2. #2
    Join Date
    Jul 2003
    Posts
    1220
    Is this for Mill or Lathe and what make is your controller?
    Would generating the code with a PC then downloading to the controller acceptable?

  3. #3
    Join Date
    May 2008
    Posts
    157
    This is a CNC milling machine and the controller is Mitsubishi M70 A. This accepts Fanuc type macros when it comes to trignometry. It is very much acceptable to generate the code on PC and then transfer it to the machine controller but the issue here is that there are 2 different tapers in a single bore and added to that is a fillet of R16 at the top of the bore. I guess one has to make 3 different programs for these 3 different regions of the bore.

    Another issue is that i have to use a bullnose type tool (16mm with 2mm corner radius). Is it possible to use such tools with a macro program as the contact point of the tool with the workpiece varies at each spiral point.

    thanks
    Yaji

  4. #4
    Join Date
    Jul 2003
    Posts
    1220
    Yaji
    I can only help with a G-Code file as I don't know either Mitsu or Fanuc.
    I'm sure what you want can be done with a Macro but with all requirements I believe it would be quite difficult.
    I have VBasic programs which will generate code you need.
    If you post the specs of the hole and the cutter, I'll generate code for you to try.

  5. #5
    Join Date
    May 2008
    Posts
    157
    How do you want me to post the specs of the hole ? It is a hole with two tapers and then a fillet on top like i mentioned to you. How will you generate a G code with a VB file for a profile like this ?

    Cutter is a 16mm tool with corner radius of 2mm.

  6. #6
    Join Date
    Jul 2003
    Posts
    1220
    Figures as shown in picture.
    Attached Thumbnails Attached Thumbnails TaperedHole.jpg  

  7. #7
    Join Date
    May 2008
    Posts
    157
    Here is the drawing as per your advice.

    I have already generated a G code program using a CAM software but i was looking whether a continuous spiral program can be generated for this profile with helical interpolation codes so that the machine lag if any does not spoil the profile. I do not know whether Helical interpolation is possible in a taper bore.

    Thanks
    Yaji
    Attached Thumbnails Attached Thumbnails Bore-Dwg.jpg  

  8. #8
    Join Date
    Jul 2003
    Posts
    1220
    Yaji
    Don't know if Fanuc has tapered helix feature.
    The path will not be helical interpolated.
    The path will be a continuous spiral made up of straight paths as short as you wish and the step-over as close as acceptable.
    Short increments makes a large file and small step over will take more time to machine.

  9. #9
    Join Date
    Jul 2003
    Posts
    1220
    Yaji
    Three files attached. These can be joined together to make one file.
    Check for step-over (cusp) and arc smoothness and advise if usable.
    Attached Thumbnails Attached Thumbnails R16 Fillet.jpg   CombinedFiles.jpg  
    Attached Files Attached Files

  10. #10
    Join Date
    May 2008
    Posts
    157
    Thanks for the codes ! What software did you use to generate these codes ? These look pretty smooth. I' am looking at a constant stepdown of 0.2mm, 0.15mm and 0.1mm. I will know which one to use only after i ascertain the cusp achieved on different surfaces. My only worry is on the radius surface which may have larger cusps with larger stepover / depth of cut.

  11. #11
    Join Date
    May 2008
    Posts
    157
    What is the chordal tolerance used in these programs when splitting into G01 codes ?

  12. #12
    Join Date
    May 2008
    Posts
    157
    Kiwi,

    I just checked the programs and the depth of cut seems to be varying a lot in the lower taper program and in the end it has gone even upto a depth of cut of 0.7mm which is pretty large for the given tool. Is there a was of maintaining a constant depth of cut of 0.15mm ?

    Yaji

  13. #13
    Join Date
    Jul 2003
    Posts
    1220
    Yaji
    The program I'm using is a VBasic program which I am writing.
    The Radius file has 30 revolutions and each revolution has 72 steps (haven't calculated the chordal lengths) This gives a step around the arc of 0.83 and a cusp of 0.049. A 400mm/m
    this will take 5.1min.
    The upper taper: 60 turns @ 72: Step 0.84 Cusp 0.045
    The lower taper: 38 turns @ 72: Step 0.74 Cusp 0.035

    The Radius cut with 0.1 Step along the path would give a Cusp 0.001. There would be 250 revolutions and at 72 chord per revolution the file would have 18000 lines.
    At 400 mm/m this would take 41min.

    My program does not have any way of giving constant depth.

    Quote Originally Posted by yaji63 View Post
    ... the depth of cut seems to be varying a lot in the lower taper program and in the end it has gone even upto a depth of cut of 0.7mm which is pretty large for the given tool...
    This comes about because the diameter is reducing but the step-over is constant.
    Like a 20mm X 1 thread looks fine and a 5mm X 1 thread looks coarse.

    I can reduce the step-over by increasing the turns which will give a better finish but take longer to machine.
    Advise what you think you may require.
    Kiwi.

  14. #14
    Join Date
    Jul 2003
    Posts
    1220
    Quote Originally Posted by yaji63 View Post
    ........My only worry is on the radius surface which may have larger cusps with larger stepover / depth of cut.
    My program doesn't Z step down, it steps around/along the profile.

  15. #15
    Join Date
    Jul 2003
    Posts
    1220
    Quote Originally Posted by yaji63 View Post
    I just checked the programs and the depth of cut seems to be varying a lot in the lower taper program and in the end it has gone even upto a depth of cut of 0.7mm which is pretty large for the given tool.....
    Picture shows spacing of the lower taper.
    As the helix changes its angle, does that make a heavier cut towards the bottom?

    Addition: I see the 0.7371 as the cut width, not the cut depth.
    The 0.7371 is made up of one full rotation of 72 movements and the feed rate will determine the cut depth.
    I agree the tool will only be able to cut properly at a certain helix angle. Don't know what that would be.
    Attached Thumbnails Attached Thumbnails LowerTaperSpecs.JPG  

  16. #16
    Join Date
    May 2008
    Posts
    157
    Kiwi,

    Since i tend to maintain the depth of cut (Z axis) t a max of around 0.2mm i do not look at the helix angle part when cutting taper bores. Hence the insistence on constant depth of cut considering the cutting tool behaviour when machining higher hardness die steels which is the case here.

    thanks
    yaji

  17. #17
    Join Date
    Jul 2003
    Posts
    1220
    I can generate code with small step-overs and short chords as you require.

    The file attached is for the Fillet only. Step-over 0.2mm with 360 chords per revolution.
    Chord Length Max. 0.4865 , Min. 0.2073 , Cusp Height 0.0028
    Chord to Arc Distance. Max. 0.00106 Min. 0.00045
    File has 45,000 blocks and at 400 mm/m time 20min 38sec.
    Attached Files Attached Files

  18. #18
    Join Date
    Jul 2003
    Posts
    1220
    Quote Originally Posted by yaji63 View Post
    ....I just checked the programs and the depth of cut seems to be varying a lot in the lower taper program and in the end it has gone even upto a depth of cut of 0.7mm which is pretty large for the given tool....
    Quote Originally Posted by yaji63 View Post
    .......Hence the insistence on constant depth of cut considering the cutting tool behaviour when machining............
    With reference to picture attached to post #15 do you agree the tool path shown has a constant depth of cut or as the helix angle increases do you believe the depth of cut has increased?

  19. #19
    Join Date
    Jul 2003
    Posts
    1220
    Attached file for Fillet Only
    Not sure if any better than the one your CAM program generated.
    Step-Over 0.1mm G03 Interpolated with cusp 0.001mm
    File has 501 blocks and at 400mm/m time to run 42min 33sec.
    Attached Files Attached Files

  20. #20
    Join Date
    May 2008
    Posts
    157
    It is almost the same as my CAM program and i have cut this job with leaving a stock of 0.1mm per side and the time was 16 mins for full bore at a feed rate of 525mm /min. I could not go at higher feeds as the machine was not a good one. This had a constant depth of cut of 0.15mm per pass. I' am not sure why you have said your fillet program takes 40 mins as per you as i verified them and i got a theoretical time of 20 mins + for this.

Page 1 of 2 12

Similar Threads

  1. Macro Programming
    By danhaskell in forum Fanuc
    Replies: 1
    Last Post: 05-07-2008, 08:04 PM
  2. Macro Programming
    By dapoling in forum G-Code Programing
    Replies: 4
    Last Post: 01-18-2008, 06:33 PM
  3. Jacobs Taper 3 Machining
    By pzzamakr1980 in forum MetalWork Discussion
    Replies: 2
    Last Post: 04-03-2007, 09:20 PM
  4. Machining short taper tooling.
    By davidmb in forum MetalWork Discussion
    Replies: 6
    Last Post: 04-07-2006, 11:25 PM
  5. Kia bore mill macro
    By WILLMC in forum MetalWork Discussion
    Replies: 0
    Last Post: 10-14-2005, 05:56 PM

Posting Permissions

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