PUZZLE FOR THE FANUC GURU'S

CADCAM396 · May 25, 2022, 07:05 AM

I have a very strange situation on a head head router with fanuc 30i control.
after a tool change the machine is not positioning correctly to location, it is suspect it is using relative position. G55 G90 X22.255 is clearly commanded but the machine is not respecting it. instead it is positioning X19.8948.

what might I be doing wrong here?

N5600 G0 Y15.9087
N5610 M81
N5620 M5
N5630 G49
N5640 G0 G28 G91 Z0.(PARTIAL Z RETRACT FOR UNWIND)
N5650 G90B0C0(UNWIND)
N5660 G91G30Z0(FULL Z RETRACT)
N5690 M01
N5700 G0 G17 G40 G49 G80 G90 G94 G98
(.563 BORE END MILL |TOOL - 25|DIA. OFF. - 25|LEN. - 25|TOOL DIA. - .563)
N5710 T25 M6
N5720 G0 G55 G90 X22.255 Y9.7341 C-90. B18.905 S7332 M3(MOVES TO X19.8948 WTF)
N5730 M34
N5740 M32
N5750 G43.4 H25 Z11.8854 M80
N5760 Y10.2277 Z10.444(BORES HOLE WRONG LOCATION goes to x19.8948 and bores hole)
N5770 G1 Y10.3612 Z10.0542 F36.66
N5780 G4 P500
N5790 G0 Y10.2277 Z10.444
N5800 X23.755(NEXT LOCATION THIS POSITIONS CORRECT)

gcode · May 25, 2022, 08:07 AM

N5720 G0 G55 G90 X22.255 Y9.7341 C-90. B18.905 S7332 M3(MOVES TO X19.8948 WTF)
N5730 M34
N5740 M32
N5750 G43.4 H25 X22.255 Y9.7341 <------- you've got to get X and Y position AFTER the G43.4
Z11.8854 M80
N5760 X22.255[/color] Y10.2277 Z10.444(BORES HOLE WRONG LOCATION goes to x19.8948 and bores hole)
N5770 G1 Y10.3612 Z10.0542 F36.66
N5780 G4 P500
N5790 G0 Y10.2277 Z10.444

gcode · May 25, 2022, 08:19 AM

This is proven gcode from our JOBS 5X gantry mill
Note how all three axis are defined on the G43.4 line so that the control can comp the tool length offset
to the tool tip

N5 (MACHINE RIGHT WALL POCKET #1 LEAVING .03 STOCK)
(GET 5 AXIS HEAD)
G321 A4
(NEXT TOOL = T34 )
M98 P7003
(HELICAL - 47256 - END MILL FOR ALUMINUM - VARIABLE PITCH - 3 FLUTE X 40° HELIX X 0.5000 DIA X 0.6250 LOC X 3.3750 REAC)
N6 G54 G17 G90
N7 M62 M64
N8 G00 C-114.869
N9 A21.519
N10 G01 G94 X21.7932 Y-3.0096 S5000 M03 F500.
N11 G43.4 H34 X21.7932 Y-3.0096 Z40.3081
N12 M08
N13 X24.2041 Y-3.3426 F200.
N14 X24.2873 Y-3.3812 Z40.0755
N15 X24.5369 Y-3.4969 Z39.3778 F120.

CADCAM396 · May 25, 2022, 09:49 AM

Thanks for the reply but it does not explain why the machine is positioning to X19.8948 on this line
G0 G55 G90 X22.255 Y9.7341 C-90. B18.905 S7332 M3

TCP is in a canceled state prior to this line.

mayday · May 25, 2022, 10:05 AM

Quote from: CADCAM396 on May 25, 2022, 09:49 AMTCP is in a canceled state prior to this line.

that is probably why
activate G43.4 before you move

mayday · May 25, 2022, 10:08 AM

N5750 G43.4 H25 Z11.8854 M80
you only have a Z move, try adding XY also

Flycut · May 25, 2022, 12:58 PM

Out of curiousity...
Does the previous tool have a large diameter offset?

CNCAppsJames · May 25, 2022, 05:44 PM

Quote from: CADCAM396 on May 25, 2022, 09:49 AMThanks for the reply but it does not explain why the machine is positioning to X19.8948 on this line
G0 G55 G90 X22.255 Y9.7341 C-90. B18.905 S7332 M3.

I believe this is because that's where the pivot point is prior to G43.4 activation. Head/Head machines need that X, Y, and Z on the G43.4 line to get you pre-positioned properly.

Quote from: Flycut on May 25, 2022, 12:58 PMOut of curiousity...
Does the previous tool have a large diameter offset?

Ok... I'm totally intrigued with this one. What have you seen to ask that question?

CADCAM396 · May 26, 2022, 06:06 AM

0 diameter offset on all tools.
still seems odd to me that with g40,g49 commanded and then g55 g90 X22.255 it positions to X19.8948. fyi the C-90. B18.905 is tilted in a direction that would and does comp in y when tcp is on. all rots in this program are B so x tcp comp never comes into play.
I did ad x,y,z in the g43.4 line. we are still testing

gcode · May 26, 2022, 06:50 AM

The X19.8948 is the position of the c/l of the spindle face because your tool length offset = 0
when G0 X22.255 is commanded

draw a 18.905° triangle with your tool length offset as the long leg
I'll bet the short leg's length is 22.255-16.8948 = 2.3602

Flycut · May 26, 2022, 07:23 AM

I have witnesed something to this effect some 20 years ago.
The previous tool was a facemill.
The operator had a 1.0 dia offset to compensate for a smaller facemill.
The next operation acted similar to what you are discribing.
A center drill would spot out of position then the drill would be forced to drill at an angle creating a wonky hole.
Took me a long time to realize that removing diameter wear offset from a previous tool would affect the drilling postion of the next tool.

Flycut · May 26, 2022, 07:25 AM

Machine was Feeler with Fanuc control.

Flycut · May 26, 2022, 07:29 AM

Quote from: CNCAppsJames on May 25, 2022, 05:44 PMI believe this is because that's where the pivot point is prior to G43.4 activation. Head/Head machines need that X, Y, and Z on the G43.4 line to get you pre-positioned properly.
Ok... I'm totally intrigued with this one. What have you seen to ask that question?

I don't know if you can go back far enough in the EMastercam archives but I beleive you and I have had this conversation before.

CADCAM396 · May 26, 2022, 07:43 AM

sorry I am not splaining this very well. its head head machine with b and c but technically it is rotating in an A axis.

meaning any tcp happens in the Y direction.

CNCAppsJames · May 26, 2022, 12:51 PM

Quote from: CADCAM396 on May 26, 2022, 07:43 AMsorry I am not splaining this very well. its head head machine with b and c but technically it is rotating in an A axis.

meaning any tcp happens in the Y direction.

TCP will happen in all 6 degrees of freeedom. A and B, A and C, or B and C depending on the configuration will compound the primary and secondary to get to the 3rd.