Macro parameter settings for auto tool offset measurement
Close
Login to Your Account
Likes Likes:  0
Results 1 to 6 of 6
  1. #1
    Join Date
    Nov 2018
    Country
    ALAND ISLANDS
    Posts
    289
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    81

    Default Macro parameter settings for auto tool offset measurement

    Evenin' folks,

    OK, tool probe installed, level, wired, getting feedback from PLC DGN, life is good.

    I'm trying to set the silly thing up in the parameters. The manual says G900 is the distance from the table to the probe, G901 and G902 being the X-Y positions, G903 changes whether the offset is from the spindle or the bottom of the machine (mine is a high column, 300mm), G904 being breakage detection tolerance, G905 being overrun distance,and G906 being the total gage line to table surface (being 300mm in this instance).

    When I have it set with G900 in inches, I get a SETTING DATA ERROR #900, which means the height of my switch is too small. My first thought is that it must be in millimeters not inches, so I convert it (but left X and Y in inches). The program now progresses to a point where my tool moves in X and Y to center over the probe, but then gets a DATA ERROR B without budging in Z, which means my B value is too short. The tool was 3.5 inches long, so I simply put B3.5 in the probe command. This is where things don't quite add up; my X and Y parameters were in inches, and that worked perfectly. If I have to convert all of my tool length estimates to metric for every probing, it's going to get old real quick. Changing G903 and G906 didn't seem to make any difference either.

    Does anyone understand where the operator error lies here? I know I'm doing something wrong, I just don't know what. My tool probe is set very high in the machine, but it has to be since it's a high column machine and some tools won't reach if I go any lower.

    Added: It's a Fanuc Robodrill D21iDL with 16i control, TS27R tool probe, and a generic Fanuc tool length measurement macro. Pretty sure it's identical to the one in the manual.

  2. #2
    Join Date
    Nov 2018
    Country
    ALAND ISLANDS
    Posts
    289
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    81

    Default

    To break it down a bit further, the exact issue is the line where it rapid's down over the switch:

    G00Z-[#906-#900-#2-25.0](*)

    This comes up with a Z- overtravel alarm, which doesn't add up. #906=780.0, #900=314.2183, #2=250. Thus; 780-314.218-250-25=190.782mm, or 7.5 inches. This is definitely not an over-travel issue. At this point, Z is at 0. The only reason I can see it being over travel is if it's reading inches and not millimeters.

    To be on the safe side, I switched the machine to read in metric; same overtravel error. I switched it back into inches, then changed G903 and G906 incrementally down; 680, 580, and 480 (the other possible models of robodrill in case I got it wrong). Same error.

    My next step; I'm rewriting the entire O9010 macro into SAE instead of metric. We'll see how that plays out.

    I tested G31 skip: X0004 bit 7 is 1 until you press the switch, then it's 0. So I ran this:

    G91
    G31 X-4.0 F1.0

    This only works if I depress the switch continuously. If I don't, it moves .0001 in X then stops. I don't think this is my issue, but it would indicate that once I get past my problems with the rapid movement, I'll need to change a parameter to skip when the switch is off rather than on... does that sound right?

  3. #3
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    42

    Default

    I think 6200.1 reads whether the skip signal as active when high/low.

    Can you post the 9010 macro?

  4. #4
    Join Date
    Nov 2018
    Country
    ALAND ISLANDS
    Posts
    289
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    81

    Default

    Quote Originally Posted by footpetaljones View Post
    I think 6200.1 reads whether the skip signal as active when high/low.

    Can you post the 9010 macro?
    Sure:

    %
    O9010(AUTOMATIC TOOL OFFSET)
    (S.T X500.0 Y400.0 Z330.0+150+HC)
    (TOOL OFFSET MACRO PROGRAM V4.0)
    (G910 S* H** B*** D*** M0 )
    (CHANGE PARAMETER NO.6050 DATA 910)

    (START)
    #30=#4001
    #31=#4003
    IF[#900GE100.0]GOTO10
    #3000=110(SETTING DATA ERROR #900)
    N10
    IF[#901NE#0]GOTO20
    #3000=110(SETTING DATA ERROR #901)
    N20
    IF[#902NE#0]GOTO30
    #3000=110(SETTING DATA ERROR #902)
    N30
    IF[#903NE#0]GOTO40
    #3000=110(SETTING DATA ERROR #903)
    N40
    IF[#11NE#0]GOTO50
    #3000=110(DATA ERROR "H" NOT EXIST)
    N50

    IF[#905EQ0]GOTO60
    IF[#905EQ#0]GOTO60
    #24=#905
    GOTO70
    N60
    #24=5.0
    N70

    IF[#906EQ480.0]GOTO80
    IF[#906EQ580.0]GOTO80
    IF[#906EQ680.0]GOTO80
    IF[#906EQ780.0]GOTO80
    #3000=110(SETTING DATA ERROR #906)
    N80

    G91G28G00Z0
    #22=#5043
    #20=#5021
    #21=#5022
    G00X[#901-#20]Y[#902-#21]M19
    IF[#19EQ1]GOTO1000
    IF[#19EQ2]GOTO2000
    #3000=110(DATA ERROR "S")

    N1000
    (AUTOMATIC TOOL MEASURING)
    IF[#2EQ#0]GOTO100
    IF[#2GT30]GOTO110
    #3000=110(DATA ERROR "B")
    N100
    #2=250.0
    N110
    IF[#7EQ#0]GOTO120
    G00X#7
    N120

    G00G21Z-[#906-#900-#2-25.0](*)
    IF[#13EQ#0]GOTO130
    S50M03
    G04X0.1
    M05
    M00
    N130
    G31Z-[25.0+#24]F100(*)
    #25=#5063
    #26=#903-[ABS[#22-#25]+#900]
    IF[[ABS[#906-#900-#2+#24-ABS[#22-#25]]]GT0.001]GOTO160
    #3000=110(DATA ERROR B TOOL SHORT)
    N160
    Z5.0
    G90G10L11P#11R#26
    G91G28Z0
    IF[#7EQ#0]GOTO3000
    G00X-#7
    GOTO3000

    N2000
    (AUTOMATIC TOOL BROKEN)
    #29=#[10000+#11]
    #3=#29+#900-#903
    G00Z-[ABS[#3]-5.0](*)
    G31Z-[5.0+#24]F200(*)
    #25=#5063
    Z5.0
    IF[#904EQ0]GOTO200
    IF[#904EQ#0]GOTO200
    #15=#904
    GOTO210
    N200
    #15=0.5
    N210
    IF[ABS[ABS[#3]-ABS[#25-#22]]LT#15]GOTO220
    G91G28Z0
    #3000=120(TOOL BROKEN)
    N220
    G91G28Z0

    N3000
    G#30G#31M05
    M99
    %

    Turns out the techs know what they're doing. I was thinking I didn't need an HSI interface since I was happy enough getting a signal, but it's the hardware solution to a normally open signal instead of normally closed. While I was told it was a good idea, the Renishaw guy made it sound optional. What he did say I needed was $500 of software that would create macros for me... so 6 some, then buy another 1/2 dozen... Anyways. That solves the skip signal issue.

    I'm still messing with this rapid movement, and I'm debating whether to just take the whole line out of the code. It looks like it was just to save time. The probe is mounted really high, so I don't really need to rapid down at all.

    My math was wrong though; it's a high column mill, but only 580mm, not 780. Thus G903 and G906 are 580.000:

    580-314-250-25= -9.063

    Which is double negative. What bugs me is it comes up with a Z- error. You'd think it was trying to go down...

    The more I look at this code, the more I feel like rewriting it. I'm no macro expert, but I don't see any reason for this to be in metric. On top of that, I see nothing to take the diameter of the tool. There's actually spelling errors in the code straight from the manual. The one above was on the machine when I got it.

    EDIT: I didn't read into the macro enough and assumed #2=250. My calibration tool is actually 77.5, which is greater than 30, thus: 580-314-77.5-25= 163.5

    That makes more sense, but it still doesn't explain why I'm getting z-axis overtravel. Now that I have my math right, I might try adding a G21 to that line and see what happens.

    I still feel like I might take out the rapid movement completely.

  5. #5
    Join Date
    Nov 2018
    Country
    ALAND ISLANDS
    Posts
    289
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    81

    Default

    Tell me if I'm wrong in this assumption:

    G910 S1 H01 B3

    S*=#0 , H**=#1 , and B****=#2

  6. #6
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,959
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1628

    Default

    Quote Originally Posted by thunderskunk View Post
    Tell me if I'm wrong in this assumption:

    G910 S1 H01 B3

    S*=#0 , H**=#1 , and B****=#2
    Yes, you're wrong.

    S=#19, H=#11 and B=#2

    Regards,

    Bill


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •