Offset question.


Results 1 to 12 of 12

Thread: Offset question.

  1. #1
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Offset question.

    When I reference my machine I expect I would have to set the X and Z on 1 tool and then the rest should follow. Once they have all been setup of course.


    Well when I E-stop or restart machine I have to reference the main tool (turning tool) then I have to set the Z of every single tool.

    The X seems to be fine once I take surface cuts and setup main too, but Z I have to set every time for every single tool after referencing the machine, is this normal?

    Similar Threads:


  2. #2
    Member
    Join Date
    Oct 2010
    Location
    USA
    Posts
    670
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Hey digibbs,

    Keep in mind that I've only had my Slant Pro for about a month......

    I set up a boring bar block as my initial tool to use for all my setups. I think I numbered it something like tool 99. I used the face to set my zero (using the tool offset page zero, not the zero on the main screen), I then set the edge of my block to set an approximate X value (again, in the offset tab). Once this is done, I run through and add my tools using the offset tab and set everything up.

    Now, when I go to chuck up some new stock I throw back in my boring block, type in tool 99 or M6 T9999 in the MDI, jog it over to the face of the stock and hit the zero button on the main screen. From that point on all my other tools are good to go with the new reference.

    Just me newbi $0.02 worth.

    Later,
    Awall

    Awall - The Body Armor Dude
    CoolCNCStuff_ on Instagram - CoolCNCStuff.com


  3. #3
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Hey smokedriver, thanks for the reply.

    I have a turret but it should still be the same I would guess.

    What I'm doing is a little different and maybe wrong?

    So I use T8 for my main offset tool, It is a OD turning tool.
    I face the part with T8
    WORK OFFSET - Z0.
    TOOL OFFSET - 0 then hit touch z
    Turn down OD and take measurement.
    Set WORK OFFSET OD to the correct measurement AND then I set the TOOL OFFSET X to the same measurement and hit touch X.

    So now Tool 8 reads OD of part as X offset and Z set to the 0 end of part.

    Switch tools to parting tool Tool 6
    T6 touch OD then go to TOOL OFFSET and hit touch X.
    T6 touch end of part TOOL OFFSET and hit touch Z.

    It will now work fine until I restart or Estop.

    After restart doing the exact same thing above with T8, T6 now is perfect on X but Z is way off.
    Every tool I do this way is off in Z only.



  4. #4
    Member
    Join Date
    Mar 2013
    Location
    Canada
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Once you use the Offsets tab to set the tools, you don't go back in there after E-stopping; the offsets are all relative to each other now (based on absolute machine coordinates).. When you restart (or E-stop/restart) you use the Main page; first home the machine, then put in a tool and type T1 (or your tool number) in the MDI to set it, then touch off and set Z and X for that tool. You've already set all your tools relative to your touch-off tool so you don't need to reset them all.
    Explained really well here on John Grimsmo's channel:



  5. #5
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Thanks, that is actually the video I learned from and the X works exactly as described. He doesn't go into the Z much and that's the only problem I have.

    I guess I'm doing the Z wrong somehow.
    Forget the X as its working as expected.

    On your 1st tool you face the part and then set the work offset to 0 OR the tool offset to 0?

    After that you would switch to say a brand new tool and set the Z in work offset of tool offset?



  6. #6
    Member
    Join Date
    Mar 2013
    Location
    Canada
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Once you have set your tool offsets in the offsets tab you don't ever go back in and change those settings (unless you change the tool holder or buy a new tool, etc.). Everything is done from the Main panel. So, yes, when you turn on your machine or reset from E-stop, home X and Z axis using the buttons, then use MDI to enter your tool number, make a facing cut, set the Z (probably to zero for example) and then make a cut to skim the profile of the part so you can measure the diameter, set the X to the measured diameter of your part after taking the cut. Now, switch to a different tool, enter its tool number in MDI, and as soon as you hit Enter you will see the X and Z values change, and they should now be correct for the installed tool.. that is assuming the actual tool offset set-up you did to start with was correct.
    The Z isn't talked about much because it changes every time you put in new material - so there is an assumption you will always be resetting the Z once you install new raw stock. But, regardless, you still put in a tool, enter it's tool number in MDI, move the axis in Z and set (or zero) it, and all other tools should have correct Z if you mount them and enter their tool number in the MDI.



  7. #7
    Member
    Join Date
    Mar 2013
    Location
    Canada
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    I guess one other confirmation is, if you look at your offsets page, do you have values for Z that make sense? (i.e. they are not all one value, and the longer tools (in Z) have relatively larger values than shorter tools, etc.); just to confirm that when you measured your tool offsets that the Z was done correctly?
    This is a shot of my tool offsets (note I use QCTP and gang tooling though, so some X's offset negative), but Z shows longer and shorter tools relative to each other.

    Offset question.-lathetooloffsets-jpg



  8. #8
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    I won't be able to be in front of the machine until tomorrow will look then.

    Wait am I supposed to set the Z 0 in the work offset or tool offset on the 1st tool (T8 for me)?

    I have been setting the work offset to 0 then the tool offset to 0 as well for T8. Then setting the Z via the tool offset for everything else. I mean I feel like I'm doing it right but its not working lol.



  9. #9
    Member
    Join Date
    Mar 2008
    Location
    USA
    Posts
    82
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Here's how you do it:

    When setting up your tool table the first time:
    - choose which tool will be your reference tool (T8 in your case) and advance the turret to T8 (or set the tool selection to 8 if not using the turret)
    - face the part and without moving the carriage, set Z to zero in the WORK offset (main DRO) AND set Z to zero in the TTOL table for T8.
    - take a light cut and then measure diameter set X to that diameter in the WORK offset (main DRO) and X to that diameter for T8 in the tool table.
    - for each tool you want to set up, do the same thing BUT only set the Z and X in the tool table

    Now, when you use the machine:
    go to your reference tool (T8 for you)
    face the part and set the MAIN Z DRO to zero - do not touch the tool table
    take a skim cut, measure and set the MAION X to the diameter - do not touch the tool table
    All your other tools will be correct.



  10. #10
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Thanks Dannirr,

    I think that's what I needed, I was updating the T8 tool table not just the Work offset every time I restarted the machine.

    Hopefully this has fixed the issue will report back tomorrow eve.



  11. #11
    Registered
    Join Date
    Jul 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Update.
    Dannirr that is exactly what I needed, I was updating tool 8's tool table every time instead of updating just the DRO and that was jacking it all up.

    Thanks everyone for pitching in to help me understand.



  12. #12
    Member
    Join Date
    Mar 2008
    Location
    USA
    Posts
    82
    Downloads
    0
    Uploads
    0

    Default Re: Offset question.

    Glad I could help



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

Offset question.

Offset question.