584,849 active members*
4,466 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Uncategorised CAM Discussion > 4th axis, is this normal or should I be disappointed...
Results 1 to 14 of 14
  1. #1
    Join Date
    Apr 2012
    Posts
    0

    4th axis, is this normal or should I be disappointed...

    So,

    I just bought a hobby license for deskproto multi axis. I was super excited about using the 4th axis eventually. Well, a part I'm working on suddenly changed and 4th axis became something I needed.

    I started looking into it and noticed I can't use my Y axis... it only does X, Z, and A... that's not really 4th axis if I only have access to 3 of them is it? Is this normal for 4th axis machining? I'm having a lot of issues programming my part because theres an entire section that would be done entirely in X,Y,Z and the rest of it would be better done with X, Z, A. I have some off center pockets that it wont be able to cut because it can't move along the Y axis.

    This could be a newbie issue but it's looking like something I'd be able to do in a single job if I had access to x, y, z, and a, will require three jobs and re-alligning the part since one operation will be rotational and the other two will be basic 3ds with a flip.

  2. #2
    Join Date
    Feb 2010
    Posts
    62
    Hi Lance,

    DeskProto offers two ways of using the rotation axis:
    - continuous rotation, where indeed only X, Z and A move and the Y-axis is not used (the cutter stays at Y=0 which is exactly above the rotation axis).
    - indexed machining, where plain 3-axis machining (XYZ) is used, then the part is rotated, then again 3-axis machining, a rotation, etc. This is multi-sided machining, and can be done using the wizard "Two or mode sides, automatic rotation.

    Looks like for your part you need the second method (or a combination of both).

    Lex.

  3. #3
    Join Date
    Apr 2012
    Posts
    0
    well... that sucks =\

    My part has a square pocket and some round parts with grooves in them. The square pocket can't be cut with my tool from the side because of the depth and length but if it was face cut using XYZ it'd be fine and my o-ring groves and round parts can't be cut without rotation for obvious reasons so the loss of Y means I have to do the job in a minumum of 2 jobs with 2 operations each when I was really hoping I could do it in a single job with 2 operations =\

    Also, no simulation in rotation mode makes me a sad panda.

  4. #4
    Join Date
    Feb 2010
    Posts
    62
    The simulation not yet being possible for rotation axis machining makes us sad too... It is mighty complicated to get that done.

    For your project I prefer to look at the bright side: it can be done using DeskProto !! - combining rotational paths and normal XYZ paths in one project.

    Lex.

  5. #5
    Join Date
    Jul 2007
    Posts
    1602
    Can you do it in two toolpaths, one for the rotational geometry and one for the pockets?

    bob

  6. #6
    Join Date
    Feb 2010
    Posts
    62
    Hi Bob,

    Yes, in most cases two toolpaths is sufficient.
    That combination is in fact used quite often, for instance for a ring with a flat relief or with a seat for a stone.
    See the pictures on www.deskproto.com/gallery/sealring.htm

    I assumed that in this case the total of four jobs is needed to also have a roughing path, both for the rotation work and for the XYZ work.

    Lex.

  7. #7
    Join Date
    Mar 2003
    Posts
    35538
    Is this normal for 4th axis machining?
    Yes, if your CAM software was doesn't cost several thousand dollars.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

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

  8. #8
    Join Date
    Aug 2012
    Posts
    181
    I too noticed this shortcoming of DeskProto.
    Support suggest writing a postprocessor but couldn't name an api to do that, that has access to the model geometry and tool collision checks.

    So I wrote my own.
    https://code.google.com/p/simplemultiaxiscam
    It can read the tool files of DeskProto (however I didn't get to adding the dialog to enter the path yet. ).
    It's not fully featured but a nice companion to DeskProto.
    It can use the X axis to try and follow the surface normal while cutting in Y, A, Z (e. g. cutting a cube it degenerates correctly into 4 sided, indexed face milling).
    Try in an emulator first. It's still a beta.

  9. #9
    Join Date
    Aug 2012
    Posts
    181
    Another thing you'll soon notice in DeskProto using a rotational axis is,
    that the distance of parallel cuts are calculated only once on the outside of your blank.
    Thus I cuts for example at with d/3 on the outside but halfway in already at d/9 and even deeper at d/81 melting the material and blunting the cutter.
    I'm also not too sure that it corrects the feed rates correctly or at all (angular velocity vs. velocity on the surface of a circle at a changing radius)

  10. #10
    Join Date
    Feb 2010
    Posts
    62
    Hi Marcus,
    On the feedrate issue that you mentioned: DeskProto does not make any feedrate changes when coming closer to the rotation axis. In standard G-code the Feedrate is defined only in linear speed units (like mm/sec, inches/min, etc). The G-code definition does not supply a rotation speed command. This means that the controller needs to calculate the correct rotation speed that is needed to reach the prescribed linear feedrate: the closer to the rotation axis, the higher the rotation speed that is needed.
    Unfortunately many controllers do not conform to the ISO G-code specifications in this matter.
    Also see DeskProto >> support >> forum for DeskProto users
    Lex.

  11. #11
    Join Date
    Aug 2012
    Posts
    181
    I didn't know that was the machine controllers job. I was in the process of implementing that compensation in my tiny CAM.

    I'll have to see that standard (hope it's public) to see how movements with no linear motion of the tool tip (reorient on a corner) are supposed to be handled.
    ... And see if MACH3 is standard compliant in that regard.

  12. #12
    Join Date
    Aug 2012
    Posts
    181
    Found that MACH3 support link.
    Entering a constant diameter is no solution for me as maximum and minimum diameter are very different.
    Guess I'll have to implement a MACH3 specific postprocessor to compensate for that shortcoming.

    Does Deskproto have any documentation on how to add a postprocessor and what it has access to except the g-code to process ?

  13. #13
    Join Date
    Feb 2010
    Posts
    62
    Dear Marcus,
    This will be a difficult issue to solve, I am afraid. You will not be able to fix this using the postprocessor: a postprocessor only changes the format of the NC file. Compare the two lines "G1 X10.00 Y10.00 Z 10.00" and "MOVEABS 10000, 10000, 10000": both lines contain the same information, only the format is different. You will find full documentation on the DeskProto postprocessor in the Reference manual (DeskProto >> download >> downloadable manuals). The postprocessor cannot be used to change the actual toolpath and/or the speeds. Sorry about that.
    Lex.

  14. #14
    Join Date
    Aug 2012
    Posts
    181
    Thanks.
    Maybe I can work something out with subroutines.
    If not, I can always write a standalone program like I did to add a 10*10 height probe and linear interpolation of z coordinates plus subdivision of long movements to pcb2gcode.

Similar Threads

  1. Looking for good CAM software,disappointed with Esprit Cam
    By javed08 in forum Uncategorised CAM Discussion
    Replies: 15
    Last Post: 02-28-2015, 06:44 PM
  2. Axis not refed to normal conditions
    By Claude Boudreau in forum Mach Software (ArtSoft software)
    Replies: 14
    Last Post: 02-03-2014, 08:46 PM
  3. Lynx X axis noise normal?
    By fomaz in forum Daewoo/Doosan
    Replies: 1
    Last Post: 10-18-2012, 04:20 PM
  4. disappointed with Sherline and needing recommendation
    By brian257 in forum Benchtop Machines
    Replies: 18
    Last Post: 03-18-2012, 07:05 PM
  5. Axis not refed to normal conditions
    By Claude Boudreau in forum Machines running Mach Software
    Replies: 0
    Last Post: 02-19-2008, 05:34 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
  •