504,508 active members
3,556 visitors online
Register for free
Login
IndustryArena Forum > CAM Software > MadCAM > problem with 5 axis indexed toolpaths
Page 1 of 2 12
Results 1 to 12 of 13
  1. #1
    Registered
    Join Date
    Dec 2014
    Posts
    55

    problem with 5 axis indexed toolpaths

    hello all,
    i am really having a hard time to generate 5 axis toolpaths. the other day i tried all day and could finally manage to generate toolpaths for machining a three sided pyramid with pockets. (see attached example" dreiseitige pyramide..."). today i milled it but there is a problem with the pocket toolpaths, they are 180° in the wrong direction. the tip of the pocket is at the base of the triangle. the blue arrow is facing always down when choosing direction in the window which occurs when you press the forth button from the left.

    today i wanted to redo the generating of the toolpath and it is not working at all!!! i wrote exactly down when i did it the other day, and today it does not work again

    maybe there is somewhere a setting wrong that i am not aware of. i am not really very good with rhino and madcam so there might be a beginners mistake. (or more...)

    could someone show me how to generate a very simple 5 axis trunion toolpath on a very simple objekt, like a cube with a cut off edge? i attached the rhino file. i think then i can find out the rest myself. the files are in the zip attachment.

    i would really appreciate any help.

    thank you very much,
    michael

  2. #2
    Moderator Dan B's Avatar
    Join Date
    Apr 2003
    Posts
    1314

    Re: problem with 5 axis indexed toolpaths

    See if this video helps. Please forgive the crude production. I'm new to Camtasia, so I'm still learning.

    Indexed machining in madCAM - DanBayn's library
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    dan,
    thank you very much for that example. but there is still a problem, i just dont know why. i did exactly the same setup as you, but in my case when i use the 3d toolpath, i get an error that that the toolpath cannot be put into rhino.
    if i do the 2d toolpath face milling it works.
    again i am looking for hours what the mistake could be but i dont find it.
    attached is the simple cube model, and a screenshot.

    thanks,
    michael

  4. #4
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    i think i got it now.
    i describe what i do from scratch. i have the german rhino version so i might not get the original english rhino terms.

    when i modelled the cube with 2 cut off corners,

    1. join, get the outside lines of the plane, so i get a curve.
    2. make a plane out of that curve.
    3. define c plane on object. pick the plane then the blue z arrow will stick 90° out of the plane.
    4. enlarge the plane a little bit and move it away from the part.
    5. define part for madcam, choose the cube.
    6. select tool
    7. select stock material, the plane which is away from the cube.
    8. in the 5 axis functions, choose set direction. leftclick twice on the plane away from the cube.
    9. click on region curves and select the original curve on the cube on the side you are milling.
    10. do the 3d toolpath.

    when doing the next side, do all these stepps again, from 1 to 10.

    is this now correct how i am doing it? if yes maybe others can benefit from this description (for idiots) ;-)Click image for larger version. 

Name:	success.jpg 
Views:	1 
Size:	145.0 KB 
ID:	260192

  5. #5
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    now another problem occured when milling these toolpaths. i added a roughing operation to cut out the whole cube from above. i have a trunnion xyz ac setup. my center of rotation of the a axis is at 100mm, so i set z100 to my z zero point. the zero point of x and y is in the center of the turning table of the c axis.

    when milling the roughing path from above the part hight is correct. when the a axis rotates then -90°, the end mill chrashes into the c table. in the gcode, the y values are -20 with a part hight of 25mm. Shouldnt the y values go just in positive direction? if i understand correctly the center of rotation of the part should be in the bottom plane in the center at 0/0/0. so the y values should maximum go to the end mill thickness, right?

    so what is wrong here?

    thanks again for your help,
    michael

  6. #6
    Moderator Dan B's Avatar
    Join Date
    Apr 2003
    Posts
    1314

    Re: problem with 5 axis indexed toolpaths

    If you run RTCP on your machine, you don't need to worry about the center of rotation, although it's still good practice to keep it close to the center. On Heidenhain controllers I use M128 or CYCL DEF 19 depending on whether I'm drilling or milling. When you get into indexed machining, it's important that your post-processor is correct. Do you retract the tool to a safe location when rotating the table?
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  7. #7
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    dan,

    now everything is working. the mistake was in the madcam machine setup and mach3 motor outputs, the rotation axis moved in the wrong direction, so i got the negative y values.

    the retract i have to do manually i suppose. i changed the postprocessor line

    *RAPID_RETRACT*
    G00 "x""y""z""a""b"
    *END_SECTION*

    to

    *RAPID_RETRACT*
    G00 Z50
    *END_SECTION*

    but then every time also during milling the end mill goes to z50.

    so i guess changing it by hand in the editor is no big deal. i added a reminder line with M0 (Z Retract changed?) at the beginning of the code that i dont forget.

    so thank you again for your help.

    michael

  8. #8
    Moderator Dan B's Avatar
    Join Date
    Apr 2003
    Posts
    1314

    Re: problem with 5 axis indexed toolpaths

    This is how I do it:

    *FIRST_MOVE*
    "lnbr" L Z1. FMAX M92 <<<<< this is the max Z height of the machine coordinate system
    "lnbr" L X324.Y0. FMAX M92 "coolant_on" <<<<<<this is a safe corner where the part will never rotate into the cutter
    "lnbr" L Y-595. FMAX M92 <<<<<I approach the cuts from the right front corner of the machine envelope.
    "lnbr" L "a" "b" FMAX M126
    "lnbr" M128 ;TCPM ON
    "lnbr" M26 M28 ;LOCK THE TABLE
    "lnbr" M3
    "lnbr" M23
    "lnbr" L "x""y""z" F30000
    *END_SECTION*

    Then after the machining is done, but before the table rotates I do this:

    *TOOLPATH_CHANGE*
    "lnbr" M129 ;TCPM OFF
    "lnbr" M25 M27 ;UNLOCK THE TABLE
    "lnbr" L Z1. FMAX M92 <<<<<back up to a safe height
    "lnbr" L X324.Y-595. FMAX M92 <<<<back to the safe corner before the table rotates
    *END_SECTION*

    And when it's all done:

    *TOOL_STOP*
    "lnbr" M129 ;TCPM OFF
    "lnbr" M25 M27 ;UNLOCK THE TABLE
    "lnbr" M9
    "lnbr" L Z1. FMAX M92
    "lnbr" L X324.Y-595. FMAX M92
    "lnbr" L C+0 A+0 R0 FMAX M126
    "lnbr" L Y0. FMAX M92
    *END_SECTION*

    If I'm doing production (which is rare) I will skip the safe moves because I know where my material is on every block. However, if you are machining one-of-a-kind details you want to play it safe.

    Dan
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  9. #9
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    thanks for your example. the cutter runs during operation in the part, so i guessed i would have to change the retract moves. i am using the mach3 5 axis mm postprocessor. very simple machine, no extras ;-) in the mach3 post there is no option "toolpath change".

    michael

  10. #10
    Moderator Dan B's Avatar
    Join Date
    Apr 2003
    Posts
    1314

    Re: problem with 5 axis indexed toolpaths

    You can add sections to the posts. Refer to the help file for a list of all the sections that are possible.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  11. #11
    Registered
    Join Date
    Dec 2014
    Posts
    55

    Re: problem with 5 axis indexed toolpaths

    so i add
    *TOOLPATH_CHANGE*
    "lnbr"Z50 F1000 <<<<<back up to a safe height
    *END_SECTION*
    and the tool goes up to z50 before it rotates a or c axis?

    i just need to go up, that enough for my case.

  12. #12
    Moderator Dan B's Avatar
    Join Date
    Apr 2003
    Posts
    1314

    Re: problem with 5 axis indexed toolpaths

    Yes, the TOOLPATH CHANGE section was added to give the user some options when one path finishes, but before the next one starts. Without it, two paths using the same tool lacked control between paths.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

Page 1 of 2 12

Similar Threads

  1. which cam program to use full 5 axis machining no indexed
    By encex in forum Uncategorised CAM Discussion
    Replies: 11
    Last Post: 09-30-2014, 08:48 PM
  2. Solidcam transform toolpaths around 4th axis problem?
    By jsclark in forum SolidCAM for SolidWorks and SolidCAM for Inventor
    Replies: 1
    Last Post: 02-01-2014, 10:44 PM
  3. Replies: 12
    Last Post: 09-06-2013, 01:02 PM
  4. Replies: 10
    Last Post: 06-04-2012, 12:35 AM
  5. Madcam - 4 axis indexed ring machining
    By etzz in forum MadCAM
    Replies: 3
    Last Post: 08-28-2008, 06:54 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
  •