Build Thread Tree325 Retrofit Started - Page 28


Page 28 of 28 FirstFirst ... 1825262728
Results 325 to 329 of 329

Thread: Tree325 Retrofit Started

  1. #325
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    403
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    .
    I am not seeing the machine position (tip of the tool) 1.0" higher.
    Also, just to be sure you understand, the machine moves up 1.0". The tip of the tool should be in the same place as the previous tool. That is the whole point of tool length compensation, making the tip of the tools the same height for a whole bunch of different length tools of course.



  2. #326
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    171
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ....
    ...

    Quote Originally Posted by mmurray70 View Post
    Also, just to be sure you understand, the machine moves up 1.0". The tip of the tool should be in the same place as the previous tool. That is the whole point of tool length compensation, making the tip of the tools the same height for a whole bunch of different length tools of course.
    Maybe I am misunderstanding how this functions. On the machines I work with at my daily job, the operator can set the tool gauge length to the actual length of the tool ... set on a tool-setter.
    So, a tool is measured at 10.0".... this is what he enters into the Siemens 840D controller while setting up the tool in the controller
    Then he can run any NC program and it will cut the programmed size on Z-axis. However, if the operator chooses to stay up .010" on a Z-surface being cut .... he can change the tool gauge length to 10.010" instead of 10.0".
    Now when he runs the NC program ... it will cut at +.010" higher then the NC Z-Level programmed value.

    Wouldn't I expect this tool data in KMotionCNC to function the same was?

    So, I set tool #2 at Z0 on the top of the work piece via Z-Axis setting on the DRO.... then in the tool data table I set tool #2 at 1.0" .... wouldn't the G43 H2 position the actual cut (if programmed at Z0 via NC code) be at Z1.0" instead of Z0?

    ....
    ....



  3. #327
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    403
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    ....
    ...



    Maybe I am misunderstanding how this functions. On the machines I work with at my daily job, the operator can set the tool gauge length to the actual length of the tool ... set on a tool-setter.
    So, a tool is measured at 10.0".... this is what he enters into the Siemens 840D controller while setting up the tool in the controller
    Then he can run any NC program and it will cut the programmed size on Z-axis. However, if the operator chooses to stay up .010" on a Z-surface being cut .... he can change the tool gauge length to 10.010" instead of 10.0".
    Now when he runs the NC program ... it will cut at +.010" higher then the NC Z-Level programmed value.

    Wouldn't I expect this tool data in KMotionCNC to function the same was?....
    Yes, it will work the same way here. If you have some way to measure all your tools before you put them in the machine that will work fine.

    So, I set tool #2 at Z0 on the top of the work piece via Z-Axis setting on the DRO.... then in the tool data table I set tool #2 at 1.0" .... wouldn't the G43 H2 position the actual cut (if programmed at Z0 via NC code) be at Z1.0" instead of Z0?.
    Im not really sure what you mean here. If you are looking at your DRO to calculate what tool length offset to use, there may be a new offset already in there (since its a different tool) that may be messing up the calculation.


    Seems like theres always a lot of confusion on here about tool offsets. The easiest way to deal with tool offsets is to have a standard procedure of touching your tools off some common plane (Table, tool height setter, 123 block etc) and run this program i attached with a user button. This will set the machine position of the current tool when at that plane. Do this for every tool as soon as you load it and then they will all match up. You can simply zero the Z DRO for each new job (with any tool) and all other tools will move with it. You can use different fixture offsets (g54/g55/etc) and everything will still work. If you break a tool just touch it again with same procedure.

    Dont worry if the theory of all the numbers/offsets is confusing, Its really simple in practice. Just move to your tool setting point, run this program as a user button, do this for every tool, and everything will work out after. Only possible issue is with knee mills. If you move the knee you will need to re touch all tools again.

    Attached Files Attached Files


  4. #328
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    171
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ...
    ...


    Quote Originally Posted by mmurray70 View Post
    ......

    Seems like theres always a lot of confusion on here about tool offsets. The easiest way to deal with tool offsets is to have a standard procedure of touching your tools off some common plane (Table, tool height setter, 123 block etc) and run this program i attached with a user button. This will set the machine position of the current tool when at that plane. Do this for every tool as soon as you load it and then they will all match up. You can simply zero the Z DRO for each new job (with any tool) and all other tools will move with it. You can use different fixture offsets (g54/g55/etc) and everything will still work. If you break a tool just touch it again with same procedure.

    Dont worry if the theory of all the numbers/offsets is confusing, Its really simple in practice. Just move to your tool setting point, run this program as a user button, do this for every tool, and everything will work out after. Only possible issue is with knee mills. If you move the knee you will need to re touch all tools again.
    Thanks Mark ... I will give this a shot.

    I think I understand how this is working now. I was able to to get it to work like I wanted. I set tool #1 to the top DRO "Z" zero work piece plane and took the same tool raised it up .500" from the work piece top "Z" zero place and called tool #2 the loaded tool pull-down --> then edit and put in .500" on tool #2 and then I saw the DRO read zero while the Machine position read Z.500". This now makes sense to what you have explained above.

    Now I can run the NC code with tool #1 and it cut at the work piece "Z" zero place ... and if I run the same NC code with tool #2 ... it will run at Z.500" from the work piece "Z" zero plane.

    I will try your attached C-Program next.

    ...
    ...



  5. #329
    Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    3137
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Hi Peter,

    I think I understand how this is working now. I was able to to get it to work like I wanted. I set tool #1 to the top DRO "Z" zero work piece plane and took the same tool raised it up .500" from the work piece top "Z" zero place and called tool #2 the loaded tool pull-down --> then edit and put in .500" on tool #2 and then I saw the DRO read zero while the Machine position read Z.500". This now makes sense to what you have explained above.
    It may help to understand that when you "Zero" an axis what actually happens is a GCode offset is computed to make the GCode coordinate (DRO) be zero. The computed offset will be different depending on whether or not Tool Length Compensation is turned on with G43Hxxx or turned off with G49. And of course if Length Compensation is turned on the length of the selected tool will matter.

    If Tool Length Compensation is on (G43):

    DRO = Machine + Global Offset + Fixture Offset + Tool Length(Hxxx)

    otherwise (G49)

    DRO = Machine + Global Offset + Fixture Offset

    Regards
    TK http://dynomotion.com


Page 28 of 28 FirstFirst ... 1825262728

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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Tree325 Retrofit Started

Tree325 Retrofit Started

Tree325 Retrofit Started