584,842 active members*
4,196 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Mastercam > 5 Axis Positional Code questions. Have pictures and MCX file Inside.
Results 1 to 10 of 10
  1. #1
    Join Date
    Jan 2009
    Posts
    245

    5 Axis Positional Code questions. Have pictures and MCX file Inside.

    I had made a post last week, that sorta got confusing. So I decided to take another simular part and try it again. I drew up in SW the exact orientation of the machine so there is no confusion there. As you can see The machine is a tilting rotary table style of 5th. It is a B and C, with the B being the tilt, and the C being the rotary.










    You can see the Positive movment for each axis.

    Now lets look at the mcx problem.









    It is the RED face that I am starting with.

    Here is the begining part of the code it outputs:

    N102 G20
    N104 G0 G17 G40 G80 G90 G94 G98
    N106 G0 G28 G91 Z0.
    N108 G0 G28 X0. Y0.
    N110 ( 1/2 FLAT ENDMILL TOOL - 1 DIA. OFF. - 239 LEN. - 1 DIA. - .5 )
    N112 T1 M6
    N114 G0 G54 G90 X-5.2979 Y3.3719 C-81.765 B47.494 S3000 M3
    N116 G43 H1 Z7.1048
    N118 M8
    N120 Z6.9548
    N122 G1 Z6.2936 F5.
    N124 X-4.992 Y3.1204 F20.
    N126 X-2.0155 Y3.4114


    As you can see it is wanting to do a C-81.765. When I think it should be doing a Neg 8.235 Deg. And it is outputing a B 47.494 when It measures to be needing a B 47.2?

    I think I have something wrong in my MISC VALUES section of the Parameters of my toolpath. Can someone look to see what I am doing wrong?
    Attached Files Attached Files

  2. #2
    Join Date
    Mar 2011
    Posts
    1
    hello ,problem is in your plane are made wrong,check this file .

  3. #3
    Join Date
    Jan 2009
    Posts
    245
    It looks like you created a surface and then did a surface pocket. The problem is the surface is not parallel to the surface I am trying to cut if you look perpendicular on the view you created?.

  4. #4
    Join Date
    Apr 2003
    Posts
    3578
    What post are you using?
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  5. #5
    Join Date
    Jan 2009
    Posts
    245
    MILL 5 - AXIS TABLE - HEAD VERTICAL

  6. #6
    Join Date
    Dec 2008
    Posts
    3110
    Quote Originally Posted by blakemachine View Post
    MILL 5 - AXIS TABLE - HEAD VERTICAL
    My understanding for this description is :-

    a "MILL 5 AXIS" post, 4th axis is "TABLE" moving, 5th axis is "HEAD" tilting, Spindle normally "VERTICAL"
    your picture is for a "TABLE-TABLE"

    the concept of the X & Y positive table movement is OK for 2D work,.... but lose that thought when stepping up into 3D spacial machining....it's the tool that does all the moving & rotating around a fixed part. ( I hate it when manuals show Z+ to move the tool, & the other X/Y buttons to move the table )

    Your angles may not be correct as they are taken from intersecting face edges, the only true item to measure from is the hole axis line

    Try re-creating your planes by selecting the hole circle wireframe ( it cannot be a spline ), this should give you a couple of variants of Z axis direction/orientation ( select the one coming away from your red face ). This would place your red face perpendicular to the Z axis. It would be simple to then to rotate that new view around Z to get your best C/T plane, re-pick the origin to your tooling ball.

  7. #7
    Join Date
    Jan 2009
    Posts
    245
    Yea, thats what it is, is that to get the correct compound angle, you cant just move to the angles that are on the part, as the 5th table cant move in those axis, so it becomes a trig function. Turns out is that the code is somewhat output correct. The problem is that it is giving a C of -81.765 when it should be 90.0-81.765= 8.235. But the correct is -8.235 degrees. I dont know why its outputing the -81.765 and not the -8.235. What would be the correct post that I should be using?

  8. #8
    Join Date
    Jan 2009
    Posts
    245
    MILL 5 - AXIS TABLE - TABLE HORIZONTAL it still wants to spin C axis -81.765 instead of -8.235. I dont get why its referencing from 90 deg with the part orientated the way it is.

  9. #9
    Join Date
    Dec 2008
    Posts
    3110
    Quote Originally Posted by blakemachine View Post
    MILL 5 - AXIS TABLE - TABLE HORIZONTAL it still wants to spin C axis -81.765 instead of -8.235. I dont get why its referencing from 90 deg with the part orientated the way it is.
    You would need a TABLE-TABLE VERTICAL
    - with a CNC machine build having the C-axis on top of the B-axis. So that B-axis would tip 47.2°, & the C-axis would go to +8.2°

    The NC output would seem to be OK.... if a B-axis is on top of the C-axis ( C-axis rotates 81° CW, B-axis tips 47° CCW )

    Put up a pic of the TOP view of the red face, so I can see how it is seen by the tool.

    You'll also find that the angle ( the items you dimension the angles on ) are not 90° to each other.

    - create a line thru the bore, and angle dimension it in TOP & FRONT views to get the proper angles to have the red face flat for machining

  10. #10
    Join Date
    Mar 2016
    Posts
    3
    Hi Sir,
    The Mastercam post proceesor for 5 axis post C value not correct and B value correct
    but the sign miss up with + and -. The only way I do is to edit the post by calculate again the C and
    keep B always - and add under the G54 line (red line). The B-47.947 is correct( 90- 42.5056 = 47.494)
    because the part rotate C171.765 to another side.

    T1 M6
    G0 G54 G90 X-5.2979 Y3.3719 C-81.765 B47.494 S3000 M3
    C171.765 B-47.494
    G43 H1 Z7.1048
    M8
    Z6.9548
    G1 Z6.2936 F5.
    X-4.992 Y3.1204 F20.
    X-2.0155 Y3.4114

    Good luck.
    If you need something more, please reach me at [email protected]

Similar Threads

  1. Plasma bevel cutting burny 10LCD+ code inside
    By MrElder in forum Waterjet General Topics
    Replies: 2
    Last Post: 12-09-2021, 12:46 PM
  2. Simple 5 axis positional not correct.
    By blakemachine in forum Mastercam
    Replies: 14
    Last Post: 10-15-2013, 05:03 AM
  3. New on X5+. some questions and pics inside
    By okabum in forum Syil Products
    Replies: 5
    Last Post: 09-24-2011, 04:20 PM
  4. macro code inside of a subroutine
    By brockmo in forum Fadal
    Replies: 7
    Last Post: 03-13-2009, 04:32 AM
  5. Positional 5-Axis Machining
    By PrecisionD in forum Surfcam
    Replies: 1
    Last Post: 10-06-2008, 10:25 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
  •