532,016 active members*
3,417 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Fadal > Spindle Touch Probe Programming Question(s)... 2007 VMC15
Results 1 to 16 of 16
  1. #1

    Spindle Touch Probe Programming Question(s)... 2007 VMC15

    I recently installed a spindle touch probe (I honestly don't know how I managed without one) and have written a bunch of programs/macros to run various probing scenarios and save x-y-z coordinates into the fixture offset table.
    I have written a program to probe either the ID or OD of a bore/shaft and calculate the center x-y coordinates (i.e., L9101). This works great. However, in the same program I would like to stop the program using M0, jog the machine and then continue running the program to probe z axis position.
    When I jog, the z probe touch movement is not correct. If I don't jog, the z touch is correct. Something about jogging then re-starting screws thing up???
    Here is the code for this z movement. It is probably something obvious, but I can't seem to figure out the problem. Any suggestions are appreciated.
    Thanks, Mark.

    N340 (STOP PROG FOR JOG TO Z POSITION)
    N345 #PRINT "JOG TO Z POSITION AND START"
    N350 M0

    N355 (Z PROBE TOUCH MOVEMENT)
    N356 G1 G91
    N360 Z-3.0 F15. G31
    N365 Z.50 F15. G31.1
    N370 Z.01 F15. G1
    N375 Z-3.0 F.1 G31
    N380 (M0)
    N385 #V5=AZ
    N390 #V6=(V5+10.4593)
    N395 #R3=V6
    N396 G1 G91 Z.5 F30.

    N405 (SAVE X Y Z TOUCH POSITIONS TO FIXTURE OFFSET TABLE)
    N410 G90 G10 L2 P+R9 X+R1 Y+R2 Z+R3

  2. #2

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    here is what's happening.
    when i run the program and probe 3 points of a circle (ID or OD) needed to calculate the center using L9101, the machine is at a constant z, say -5.8.
    i can then jog to any x, y position and as long as i return z to -5.8 when i restart the program, the the z touch position is correct.
    however, if the z is changed to say -6.0 when i restart the program the recorded z position is off by the 0.200 difference in the starting position.
    this happens using either restart from JOG Option 2 or 3.
    the z absolute display on the screen shows the correct value but for some reason the recorded z position is shifted?

  3. #3

    Join Date
    Aug 2019
    Posts
    295

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Any way to confirm if the control is correctly applying the calibration offsets/variables for all axes when manually probing an ID/OD?

  4. #4

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by Mecanix View Post
    Any way to confirm if the control is correctly applying the calibration offsets/variables for all axes when manually probing an ID/OD?
    the coordinate system shift is greater than calibration offsets, so i don't think that is the issue?

  5. #5

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    the z shift from a JOG is not being recorded by the axis position variable AZ.
    when i read the current position using variable AZ i do not get the absolute value as shown on the upper left corner of the display?
    some sort of coordinate shift is happening?

  6. #6

    Join Date
    Aug 2019
    Posts
    295

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    You believe in shop's ghosts? Gets worst when planets lines up, about this time of the year in fact ;-)

    In all seriousness, I'd get the macro out from the ctrl's file system and study its logic with a text editor while relaxed, I bet your answer is in there somewhere.
    (I'm on Siemens, can't help for your proprietary bits but still curious to know what went wrong, let us know)

  7. #7

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by Mecanix View Post
    You believe in shop's ghosts? Gets worst when planets lines up, about this time of the year in fact ;-)

    In all seriousness, I'd get the macro out from the ctrl's file system and study its logic with a text editor while relaxed, I bet your answer is in there somewhere.
    (I'm on Siemens, can't help for your proprietary bits but still curious to know what went wrong, let us know)
    yeah, some ghost...
    i will figure it out, it is probably something obvious, but still racking my brain with what's going on.
    i think i will write a simple program that does nothing but probe the z axis and stop, jog and restart and record positions at several lines in the code.
    hopefully it will shed some light on what's happening???

  8. #8

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    well.., i'm stumped.
    i run the simple program below.
    it records initial x y z positions, stops the program, i JOG x y z positions, rerecord x y z positions, then probe z axis and record final z position.
    the program is restarted using Option 3 and it does what it says it does which is to keep original coordinate system. this is correctly shown on the absolute coordinate display on the monitor.
    but when axis position is read using Axis Position Variables the absolute position is not recorded correctly.
    what is recorded is the position prior to the the JOG???
    at this point i will have to run two separate programs, one to calculate the center of the circle (x & y) and another get the z position. bummer...
    i suspect this is my error, but i just can't seem to figure it out...???

    Option 3 will cause the tool to remain at this current position, the tool
    coordinate system will remain at its original position, and execution of the
    program will continue.

    O0010 (PROBE.ZTEST)
    N5 #CLEAR
    N10 #PRINT "Z PROBE TEST WITH JOG"
    N15 #PRINT "SAVE IN FIXTURE OFFSET TABLE"
    N20 #PRINT "INPUT FIXTURE OFFSET #"
    N25 #INPUT V10
    N30 #R9=V10
    N35 M64 M66
    N40 (SAVE INITIAL X Y Z POSITION)
    N45 #V18=AX
    N50 #V19=AY
    N55 #V20=AZ
    N56 #R1=V18
    N57 #R2=V19
    N60 (STOP PROG FOR X Y Z POSITION JOG)
    N65 M0
    N70 (Z PROBE TOUCH MOVEMENT)
    N75 G1 G91
    N76 #V28=AX
    N77 #V29=AY
    N80 #V30=AZ
    N85 #V31=V20-V30
    N90 Z-3.0 F15. G31
    N95 Z.50 F15. G31.1
    N100 Z.01 F15. G1
    N105 Z-3.0 F.1 G31
    N110 #V5=AZ
    N115 #V6=(V5+10.4593-V31)
    N120 #R3=V6
    N125 G1 G91 Z.5 F30.
    N130 (SAVE Z TOUCH POSITIONS TO FIXTURE OFFSET TABLE)
    N135 G90 G10 L2 P+R9 X+R1 Y+R2 Z+R3
    N150 M0
    N155 M30

  9. #9

    Join Date
    Aug 2019
    Posts
    295

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Something with how the optional high speed skip behaves? that pos is saved "when retracted" (31.1), if I am not mistaken.
    Old fanuc stuff on top of my head...

  10. #10

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by Mecanix View Post
    Something with how the optional high speed skip behaves? that pos is saved "when retracted" (31.1), if I am not mistaken.
    Old fanuc stuff on top of my head...
    dunno...?
    initial position V18, V19 & V20 should differ from position V28, V29 & V30 after JOG. they don't.
    and, final z position V5 should be the absolute z position which is shown on the monitor. it isn't.
    essentially, the JOG is ignored? or, i screwed something up... which probably more likely.

  11. #11

    Join Date
    Aug 2019
    Posts
    295

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    You haven't screwed up anything, I'm sure you are just missing something simple somewhere, whether that is a clear or init command somewhere in the code I'm not sure.
    I bet the fanuc experts will chime in soon since you now have posted your routine code.

  12. #12

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by Mecanix View Post
    You haven't screwed up anything, I'm sure you are just missing something simple somewhere, whether that is a clear or init command somewhere in the code I'm not sure.
    I bet the fanuc experts will chime in soon since you now have posted your routine code.
    i will probably just manually probe the z if i can't get this figured out. it isn't that difficult :-)
    but, glad to hear from the programming experts if anyone has suggestions.

  13. #13

    Join Date
    Aug 2019
    Posts
    295

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by everettengr View Post
    but, glad to hear from the programming experts if anyone has suggestions.
    I'd list up your control type/make also, as much of the 31 & 31.1 are parametized, to my limited knowledge. Hopefully someone with a similar set-up could help out to compare those params with yours and get you going.



    Quote Originally Posted by everettengr View Post
    well.., i'm stumped.
    i run the simple program below.
    it records initial x y z positions, stops the program, i JOG x y z positions, rerecord x y z positions, then probe z axis and record final z position.
    the program is restarted using Option 3 and it does what it says it does which is to keep original coordinate system. this is correctly shown on the absolute coordinate display on the monitor.
    but when axis position is read using Axis Position Variables the absolute position is not recorded correctly.
    what is recorded is the position prior to the the JOG???
    at this point i will have to run two separate programs, one to calculate the center of the circle (x & y) and another get the z position. bummer...
    i suspect this is my error, but i just can't seem to figure it out...???

    Option 3 will cause the tool to remain at this current position, the tool
    coordinate system will remain at its original position, and execution of the
    program will continue.

    O0010 (PROBE.ZTEST)
    N5 #CLEAR
    N10 #PRINT "Z PROBE TEST WITH JOG"
    N15 #PRINT "SAVE IN FIXTURE OFFSET TABLE"
    N20 #PRINT "INPUT FIXTURE OFFSET #"
    N25 #INPUT V10
    N30 #R9=V10
    N35 M64 M66
    N40 (SAVE INITIAL X Y Z POSITION)
    N45 #V18=AX
    N50 #V19=AY
    N55 #V20=AZ
    N56 #R1=V18
    N57 #R2=V19
    N60 (STOP PROG FOR X Y Z POSITION JOG)
    N65 M0
    N70 (Z PROBE TOUCH MOVEMENT)
    N75 G1 G91
    N76 #V28=AX
    N77 #V29=AY
    N80 #V30=AZ
    N85 #V31=V20-V30
    N90 Z-3.0 F15. G31
    N95 Z.50 F15. G31.1
    N100 Z.01 F15. G1
    N105 Z-3.0 F.1 G31
    N110 #V5=AZ
    N115 #V6=(V5+10.4593-V31)
    N120 #R3=V6
    N125 G1 G91 Z.5 F30.
    N130 (SAVE Z TOUCH POSITIONS TO FIXTURE OFFSET TABLE)
    N135 G90 G10 L2 P+R9 X+R1 Y+R2 Z+R3
    N150 M0
    N155 M30

  14. #14

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    Quote Originally Posted by Mecanix View Post
    I'd list up your control type/make also, as much of the 31 & 31.1 are parametized, to my limited knowledge. Hopefully someone with a similar set-up could help out to compare those params with yours and get you going.
    good idea

    machine is a 2007 VMC15 with CNC88HS control. i believe it is the latest revision, 1400-5C for the main cpu.

  15. #15
    Registered
    Join Date
    Jan 2015
    Posts
    393

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    I assume you have the Fadal touch probe manual not sure if anything in there will answer your question https://itscnc.com/images/Sect_15_Touch_Probes.pdf

  16. #16

    Re: Spindle Touch Probe Programming Question(s)... 2007 VMC15

    thanks to @scubawes, who discovered the fix, i can now stop during a probe macro and JOG to a different x, y location and continue the macro to pickup my Z position.
    this is a huge help when probing IDs and ODs where the Z is likely the top or bottom of the hole or fixture, but a JOG is needed to position the probe in the correct location after calculating the center of the hole/shaft.
    this also allows for full manual probes where you can start a macro but then stop before each x, y, and z probe, JOG to pickup the position and save to the fixture offset table.
    here is corrected code. i added P1 to line 375 and PZ1 to line 390 to call the Z coordinate.
    works great!!!

    N340 (STOP PROG FOR JOG TO Z POSITION)
    N345 #PRINT "JOG TO Z POSITION AND START"
    N350 M0

    N355 (Z PROBE TOUCH MOVEMENT)
    N356 G1 G91
    N360 Z-3.0 F15. G31
    N365 Z.50 F15. G31.1
    N370 Z.01 F15. G1
    N375 Z-3.0 F.1 G31 P1
    N380 (M0)
    N385 (#V5=AZ this line can be deleted)
    N390 #V6=(PZ1+10.4593)
    N395 #R3=V6
    N396 G1 G91 Z.5 F30.

    N405 (SAVE X Y Z TOUCH POSITIONS TO FIXTURE OFFSET TABLE)
    N410 G90 G10 L2 P+R9 X+R1 Y+R2 Z+R3

Similar Threads

  1. Another newb question about setting up a z touch probe on a Chinese 6040 clone
    By t2krookie in forum General Off Topic Discussions
    Replies: 3
    Last Post: 07-17-2015, 06:54 PM
  2. Help!!! Touch probe grounding through spindle???
    By Momentz in forum DIY CNC Router Table Machines
    Replies: 1
    Last Post: 11-28-2014, 10:21 PM
  3. Replies: 14
    Last Post: 02-11-2014, 02:56 AM
  4. Replies: 12
    Last Post: 06-05-2013, 06:05 PM
  5. Renishaw touch trigger probe question
    By Shotout in forum Okuma
    Replies: 3
    Last Post: 02-11-2011, 06:34 PM

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
  •