537,761 active members*
3,457 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > PlanetCNC > howto work with multiple work offsets G54 G55 ....
Results 1 to 7 of 7
  1. #1

    howto work with multiple work offsets G54 G55 ....

    I'm currently looking into working with different Work Offsets and I have a bit of a hard time understanding the differente and relations between Work Position and Coordinate System.
    I'm more or less sure that the confusion mainly is caused by me being an absolute novice in machining, so if someone could shed some light into this it would be greatly appreciated.


    I have two vices installed on my machine and I want to machine the same part in both of them to reduce tool change time. From my understanding I can achieve this by running the same gcode in different coordinate systems and switching between them on the fly. Machine Part 1 with tool 1 in G54, and repeated the same code a second time with G55.
    In general this seems to be working as expected, however I'm struggling with setting the Origin for G54 and G55 correctly.
    From a hierarchy point of view I always thought that I would have the Machine Coordinate Systems on top, followed by the G54/G55 Coordinate System. But it seems that with Planet CNC there is a third Work Position in between the two.
    When using the default buttons for "Work Position XY/Z" To zero it shifts not only the currently G5* but ALL of them.
    I figured that I need to use the Buttons
    Machine->Coordinate Systems->Axis To Zero..... to set the Origin for each G5* individually.
    Beside this I figured that switching in Settings->User Interface->Position->Command from Work Position to Coordinate System would change the behavior of the XYZ Buttons in the user Interface to change only the current active G5*

    So while ignoring the Menü buttons on the left menu and working with "Machine->Coordinate Systems->....." buttons seems to give me the desired result I don't really understand the benefit of the "Work Position" Coordinate system in between and I'm not sure if I'm going with the correct approach or if I do something fundamentally wrong.

    best Regards,
    Klaus

  2. #2
    Moderator
    Join Date
    Mar 2017
    Posts
    758

    Re: howto work with multiple work offsets G54 G55 ....

    Text below

    On this image CS sets distance between blue and green, WO sets distance between green and orange.
    Attached Thumbnails Attached Thumbnails IMG_20210216_114900[1].jpg  

  3. #3
    Moderator
    Join Date
    Mar 2017
    Posts
    758

    Re: howto work with multiple work offsets G54 G55 ....

    There are two important positions on CNC.


    1. Machine position - this is physical position of tool of your machine.
    This position is set during hoiming procedure where machine limits are detected.
    2. Work position - this is ad hoc position. It is set as needed to ease working with machine.


    CNC move commands almost always use work position (exception is G53).
    Because physical machine moves are in machine position. algorithm to calculate machine position from work position is needed.


    These are our options (I call them offsets):
    1. Axis offset, rotation and scale (AO)
    2. Tool offset (TO)
    3. Work offset (WO)
    4. Coordinate system offset and rotation (CS)
    5. Warp
    6. Transformation


    Formula for algorithm is:
    Machine position + AO + TO + WO + CS + Warp + Transformation = Work position


    As you see there are a lot of different ways to get same results.


    Which offset you use depends on your workflow because each offset has its own perks.
    In "multiple vices" case I would use CS offset for each vice.
    Within each vice I would use WO.


    In old days there was only one offset and perhaps it was easier to understand.
    But this gives much more flexibility.

  4. #4

    Re: howto work with multiple work offsets G54 G55 ....

    OK this matches more or less what I figured.

    The point that confuses me is that changing the Work offset while being in G54 has a influence on G55
    I had expected that the WO would be a "subset" of CS, not the other way around.
    As far as I can see from the reactions of the Programm CS seems to be set in relation to WO

  5. #5
    Moderator
    Join Date
    Mar 2017
    Posts
    758

    Re: howto work with multiple work offsets G54 G55 ....

    WO and CS are independent.

    Lets say machine position X=10 and all offsets are zero. Work position is X=10.
    Set CS to X=6. Work position is X=4.
    Set WO to X=3. Work position is X=1.
    Set CS again to X=1. Work position is X=6.

    G54, G55... just select which coordinate system offset you you use. Work offset remains the same.
    This is logical. You select coordinate system for each vice. With G54, G55,... you select which vice you will be using.
    Now put some material in all your vices. You only need to select "working zero" on one vice and will remain same for all other.

  6. #6

    Re: howto work with multiple work offsets G54 G55 ....

    Thanks for the explanation. I think I finally understand the logic behind this. It does not match by initial Assumtion on how this stuff would work but I think I can adapt to this ;-)

  7. #7
    Member
    Join Date
    Jan 2005
    Posts
    12068

    Re: howto work with multiple work offsets G54 G55 ....

    Quote Originally Posted by ScorpionTDL View Post
    I'm currently looking into working with different Work Offsets and I have a bit of a hard time understanding the differente and relations between Work Position and Coordinate System.
    I'm more or less sure that the confusion mainly is caused by me being an absolute novice in machining, so if someone could shed some light into this it would be greatly appreciated.


    I have two vices installed on my machine and I want to machine the same part in both of them to reduce tool change time. From my understanding I can achieve this by running the same gcode in different coordinate systems and switching between them on the fly. Machine Part 1 with tool 1 in G54, and repeated the same code a second time with G55.
    In general this seems to be working as expected, however I'm struggling with setting the Origin for G54 and G55 correctly.
    From a hierarchy point of view I always thought that I would have the Machine Coordinate Systems on top, followed by the G54/G55 Coordinate System. But it seems that with Planet CNC there is a third Work Position in between the two.
    When using the default buttons for "Work Position XY/Z" To zero it shifts not only the currently G5* but ALL of them.
    I figured that I need to use the Buttons
    Machine->Coordinate Systems->Axis To Zero..... to set the Origin for each G5* individually.
    Beside this I figured that switching in Settings->User Interface->Position->Command from Work Position to Coordinate System would change the behavior of the XYZ Buttons in the user Interface to change only the current active G5*

    So while ignoring the Menü buttons on the left menu and working with "Machine->Coordinate Systems->....." buttons seems to give me the desired result I don't really understand the benefit of the "Work Position" Coordinate system in between and I'm not sure if I'm going with the correct approach or if I do something fundamentally wrong.

    best Regards,
    Klaus
    This can be very simple in your programing with just having an X----- Y------ move to the next Vice start position still using the same work offset
    Mactec54

Similar Threads

  1. multiple work offsets
    By poster in forum Mastercam
    Replies: 4
    Last Post: 02-21-2013, 03:28 PM
  2. Using multiple work offsets in MC
    By Crashmaster in forum Mastercam
    Replies: 6
    Last Post: 08-25-2010, 04:18 PM
  3. Multiple Work Offsets
    By 9 1/2 in forum Mastercam
    Replies: 5
    Last Post: 11-15-2009, 11:28 PM
  4. Multiple Work Offsets
    By PinMan in forum BobCad-Cam
    Replies: 3
    Last Post: 06-06-2008, 10:41 PM
  5. multiple work offsets
    By rbest27 in forum Surfcam
    Replies: 2
    Last Post: 01-25-2007, 10:02 AM

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
  •