Spline probing


Page 1 of 2 12 LastLast
Results 1 to 20 of 22

Thread: Spline probing

  1. #1
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default Spline probing

    I have an Okuma 5 axis MA 600 HMC with an OSP200 controller.I have a part that I need to probe a tooth on an outside of a gear to find true C position to drill holes in the root. It is timed by the fixture but can be off slightly so I will have a close approximation of the tooth root I will be trying to find. Does anyone have some code to help me and be able to explain it to me? Thanks in advance!

    Similar Threads:


  2. #2
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Maybe I don't know enough about 5 axis HMC. I am having a difficult time trying to figure out how you will use C axis (rotation around Z) to find the center. I would have set this up to use the B axis (rotation around Y). Upload a picture of your set up.



  3. #3
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    I don't have a picture of it handy. Here is a link to a manual with a picture of the rotary that sits on the B table http://www.cnc1.com/images/customer-...tion_Guide.pdf. but it is a horizontal with a B table and a tombstone with a Rotary C. With B at 0 the rotary is pointing at the spindle, therefore a C not an A rotary. From the way is was explained to me years ago. So I have this gear fixed on center of the rotary but need to check the tooth angle and adjust the C in the offset. Sorry for no pic but I couldn't find one even on the net.



  4. #4
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Ok, try this. Find the center of the C axis. Then position the gear to probe between two teeth and find center line of the gear. Calculate the angular difference. Rotate C to adjust and probe again to verify.



  5. #5
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    I will give this a shot but it will take me awhile because I haven't programmed many probing routines. Thanks



  6. #6
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Basically you will be aiming to pick up the pitch diameter of the spline. So your Z location will be approximately the radius of the pitch diameter above center line. Initial C axis rotation will be whatever is needed to get you in the zone. Y axis will be near the center of the spline. X axis should be on center line. If you can rotate the C axis and capture positive rotation of C at the skip signal and write it to a variable. Then repeat for negative C axis rotation, there will be no need to calculate angular value. You can just add 1st and 2nd C values and divide by 2. This will be the C value to write to your work offset. Take care on your formula if you are crossing C0. during the rotating of the C axis.



  7. #7
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Thank you sir! I will keep these things in mind as I attempt this. I am going to look at the 90 deg spot as that is where the timer is and most likely no other tooth is at or really near a known angle. Though I could calculate that. I don't follow you on one (if not more as I get into it) point and that is not needing to calculate the angle. Thanks again and I will try and get this moving so I can give feedback on how it is going.



  8. #8
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Finally getting to look at this. After looking at some macros finally I am not sure I can pick up the C rotation. Do you know if the OSP 200 with renishaw is capable of doing this? This would simplify things alot. Right now I am looking to pick up the highpoint of the tooth and calculating for rotation. This is slow and a pain.



  9. #9
    Member Algirdas's Avatar
    Join Date
    Mar 2009
    Location
    United Arab Emirates
    Posts
    1982
    Downloads
    2
    Uploads
    0

    Default

    maybe you need to engage C axis first? M109?



  10. #10
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Algirdas View Post
    maybe you need to engage C axis first? M109?
    Al, its a mill, not a friggin lathe

    Shags, have you thought of just using a pointer, bring the pointer in along the centreline in so that it touches both sides of the tooth valley, & then tighten the part ?



  11. #11
    Member broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    822
    Downloads
    0
    Uploads
    0

    Default

    Yep... the statement "I have an Okuma 5 axis MA 600 HMC " kind of gives it away...
    HMC = Horizontal Machining Centre
    oh and the fact that he stated 5 Axis also!



  12. #12
    Gold Member
    Join Date
    Aug 2011
    Location
    Fordaville
    Posts
    2517
    Downloads
    0
    Uploads
    0

    Default

    we do a similar thing at my work on a horizontal mill where we do some extra machining on the face of a shaft with splines on the outside diameter that are cut on a different machine.
    our alignment accuracy between spline and face machining is not that tight so we simply put a digital spirit level across the top of the spline and manually rotate C to get the level to 0 degrees then we set the workshift of C to 0 degrees and then go.

    Last edited by fordav11; 04-05-2013 at 11:52 AM.


  13. #13
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    We already time it by a fixture but the drill is so near the size of the root that if off at all it drills the side of the tooth. So I have been searching through that manual and found O9821. It writes to some variables but looks like only x y z. I would need something to pick up the C rotation angle when it triggers. Does anyone know of a renishaw cycle that does that? Preferably with the calibration comp in it? Thanks for the responses!



  14. #14
    Gold Member
    Join Date
    Aug 2011
    Location
    Fordaville
    Posts
    2517
    Downloads
    0
    Uploads
    0

    Default

    if I was doing that alignment manually I would position the probe at X0 and between the gear tooth. Then rotate C until the probe touches one side. Then origin C. Then move C to touch the other tooth then take the C coordinate divide by 2 and move back that amount and that is your middle. Set workshift to C0 and you're done.

    You should be able to automate that in a macro pretty easily by doing the same steps....
    1. position in middle X0 then feed in Y until probe is inside the gear tooth.
    2. probe to left using C rotation. set C workshift to 0
    3. probe to right using C rotation. write C position to a temp variable
    4. divide temp variable by 2 to get the C middle position
    5. rapid C to that position
    6. set C workshift to 0
    7. drill hole at X0 C0



  15. #15
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Dave's post seems to trigger dark memories
    - the probe could only trigger while on linear movement, so you may not be able to probe features using a rotating action
    ( probing can only be done using the XY or Z axes, usually only one axis at a time )


    I remember creating a probe cycle to square a face on a MX40-HA ( horizontal )

    it probed (equi-distance) each side of the rotation axis (B axis is not moved)
    & calculated the difference in Z between the 2 ( but has a decision part to skip further adjustment if Z is within a certain tolerance)
    - there is a triangle with an angle that is obtained from that calc (Tan)....... ( probe distance in Y divided by Z distance = Tan Θ )
    - incremental rotation is 1/2 that angle
    - re-probe to check if it is in tolerance
    - then write the current position of the rotary axis to the work origin

    If the gear is large enough, you may have to use other tooth walls, as to get a larger Y probing distance, to gain accuracy
    ie ...the 4th tooth on either side of the valley that needs the hole

    Last edited by Superman; 04-06-2013 at 09:48 AM. Reason: made clearer -- hopfully


  16. #16
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Went out to the machine and in mdi tried doing a G31 C3 f100 just to see if it would do it and it wouldn't. Seems C only rotates in G0. I was just wanting to know if the probe would even stop the C rotation when it got bumped. So unless I can find a parameter to make the Rotaries move in a feed move I don't think this will work.

    I am not sure I understand what you are saying Superman. Which is no real surprise considering my experience with probing.

    Please correct me if I am wrong but since my timer is at 90deg then if I position the probe inside the tooth and just bump X side to side and find the difference, calculate the angle, this would be close but not really accurate because it may be hitting higher on one side, therefore not an equal X, which would skew the calculation to set the angle? I don't know. It would be nice if the manual would at least tell me for sure if the probe would trigger if bumped while moving C and if there is a cycle that would set some variable to what C is. Seems there is a lower level cycle O9726 that sets some system variables VSAPAX,Y,Z,A,B,C. That would normally lead me to believe that this would do what I need if my c would rotate in a feed move. Hope this makes sense to someone.

    The Manual I got for the Okuma probing is way less detailed than one for a Mazak that I have seen.



  17. #17
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Finally got the probe to work in C on a skip move! I am probing at C0 and rotating each way recording each touch of the probe. Now I have to come up with the system variables to get the calculations going. I tried the following VC38=VSAPC-VMOFC-VZOFC[VACOD]. This isn't working. A confusing thing is that VSAPC is around 144... and VMOFC is 500. I used this calculation set to get X Y AND Z positions and it works great. Any ideas?



  18. #18
    Member Algirdas's Avatar
    Join Date
    Mar 2009
    Location
    United Arab Emirates
    Posts
    1982
    Downloads
    2
    Uploads
    0

    Default

    VSAPC is around 144... and VMOFC is 500
    do variable/360° and use only the part less, than 1. In other words, use only values not exceeding 360°



  19. #19
    Registered
    Join Date
    Oct 2012
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    I don't understand Algirdas. What variable do I divide by 360?
    Both of the VSAPC's are +144. something which is not what I really expect. VMOFC (which I thought was machine offset) is 500. It would be so much easier if I could just get the 2 C values when the probe touches then I just add them together and that is my offset.



  20. #20
    Member Algirdas's Avatar
    Join Date
    Mar 2009
    Location
    United Arab Emirates
    Posts
    1982
    Downloads
    2
    Uploads
    0

    Default

    wait a moment. isn't C axis a rotation axis one? Full circle must be either 359,999 (comma decimal separator) what means 360°
    or
    199,999 if full circle is set as 200 units by parameter.
    The "500" value is strange here. I guess, it's the same as 500-360 in degrees or 500-400 in "200" units. Check that.
    what is VSAPC and VMOFC description in your manual?



Page 1 of 2 12 LastLast

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

Spline probing

Spline probing