Reply with QuoteI see numerous G49s in your code. These cancel tool length compensation. Is this intentional?
Tool Compensation... Need HELP!
I just started using a probe and are running into some problems with tool table tool length compensation (per tool table) and hope someone more experienced with Gcode can give me a hand.
Sometimes... after running a Gcode with Tool change, on next Gcode file, the tool length compensation will be off. I.e. I ran a Gcode called TTBODYTOP1.TAP and when complete, Open and ran a second Gcode called TTBODYTOP2.TAP. On the 2nd file, when it reaches G90 on line 12, I can see on the screen that the Z compensates by -3.125 which is the tool length of T5 but it has not reach that line of code yet. So when it hits the Tool change line, it compensates for another -3.125 making the Z0 off by -3.125. I can't figure out what I'm doing wrong. I hope someone can take a look at my Gcode and tell me if something is wrong in here.
A few more details....
1. I don't always Reference the Table... is it absolutely necessary for the Tool compensation to work correctly? This is part of the reason I bracketed the G28 Z0 so it will skip this command.
2. Between the first and 2nd file, I had to move the part for the next orientation so had to re-zero X and Z using the probe. When the 2nd Gcode starts, I have tried leaving it on T99 and let the Gcode change the tool to T5 as well as manually change the tool to T5 first but both gave me the same result where the compensation goes off around G90 on line 12 of the 2nd file.
Any pointers will be greatly appreciated!! Thanks in advance.
FILE 1
***************************
%
O5000 (TTBODYTOP1.TAP)
( MCV-OP ) (01-JUL-2009)
(SUBROUTINES: O2 .. O0)
( = ORIENTATION 1 = )
( Flat: front )
( Top: left )
( Origin: left bottom )
G90 G17
G80 G49 G40
G54
G91 (g28 z0)
G90
M01
N4 M6 T3
(TOOL -3- MILL DIA 0.375 R0. MM )
G90 G00 G40 G54
G43 H3 D33 G0 Z2. S3200 M3
M8
(-----------------------------------)
(3/8" EM POCKET LP COUNTER2 - POCKET)
(-----------------------------------)
X0.688 Y1.195 Z0.4
Z0.079
G1 Z-0.188 F12
G3 X0.688 Y1.195 I0. J0.023 F14
G0 Z0.4
Z-0.109
G1 Z-0.375 F12
G3 X0.688 Y1.195 I0. J0.023 F14
G0 Z0.4
Z-0.296
G1 Z-0.391 F12
G3 X0.688 Y1.195 I0. J0.023 F14
G0 Z4
G91 (g28 z0)
G90
M01
N5 M6 T10
( TOOL -10- DRILL DIA 0.188 MM )
G90 G00 G40 G54
G43 H10 D40 G0 X0.688 Y1.218 Z2. S2400 M3
M8
(---------------------------)
(3/16" DRILL LP HOLE - DRILL)
(---------------------------)
X0.688 Y1.218 Z0.4
G98 G83 Z-1.951 R-0.313 Q0.063 F16
G80
G91 (g28 z0)
G0 Z4
G90
M5
M30
%
**************************
Partial of File 2
**************************
%
O5000 (TTBODYTOP2.TAP)
( MCV-OP ) (01-JUL-2009)
(SUBROUTINES: O2 .. O0)
( = ORIENTATION 2 = )
( Flat: back )
( Top: up )
( Origin: center center )
G90 G17
G80 G49 G40
G54
G91 (g28 z0)
G90
M01
N6 M6 T5
(TOOL -5- MILL DIA 0.02 R0. MM )
G90 G00 G40 G54
G43 H14 D44 G0 X0.765 Y0.322 Z2. S3200 M3
M8
(----------------------------)
(1/4" VMILL ENG-ATD - PROFILE)
(----------------------------)
X0.765 Y0.322 Z0.4
Z0.079
G1 Z-0.01 F12
X0.6 Y0.4 F16
Y0.397
X0.674 Y0.362
G2 X0.68 Y0.353 R0.01
G1 Y0.24
G2 X0.674 Y0.231 R0.01
G1 X0.6 Y0.196
Y0.194
X0.82 Y0.295
X0.765 Y0.322
G0 Z0.4
X0.618 Y0.12
Z0.079
*****************************
Similar Threads:
Last edited by apeman88; 07-14-2011 at 03:11 AM.
I see numerous G49s in your code. These cancel tool length compensation. Is this intentional?
you MUST reference the table, especially to use the M988 command, which I do not see in your code. I also found out this past week I have to take specific steps.
1. Load Gcode
2. Reference machine
3. Regenerate TOOL PATHS for the Gcode
Failing to do that 3rd step was causing X0Y0Z0 to all be wrong on my machine. Not sure why, but I now have more end mills as a result. And I do that anytime I reload or change any Gcode.
I only count 1 G49 per file... this should be okay.... no? I'm don't know Gcode very well... I'm depending on a friend's SolidCAM (using Fanuc post) to generate these G codes and that's what it gave me. The Gcode above has been manually modified (cut and pasted) a few times but it seems to work good unless I'm cutting one file after another and the start of the 2nd or 4rd file will screw up the tool length compensation.Originally Posted by flyinchips
Ken
if it is the 3rd or 4th file that is messing up then you should post it as well. I did see a G91 with the G28 Z0 commented out (). if you are not returning to G90 that could cause a problem.
I agree make sure all your "Z" parameters are correct and then work on your program. All "T" codes should have the same reference point your "G" codes are basically functions. That is "T" codes reference from the same point they maybe have individual lengths, if so check all references points, in the parameters menu.
Last edited by admit_84; 07-15-2011 at 08:23 PM. Reason: Technicalities
I think I'm figured it out. Been emailing Matt at Tormach back and forth on this for the past 2 days but have not confirmed my latest findings yet. The problem, I think, is G49 (cancel tool compensation). If I probe the work piece with T99 (T99=6.5830") and if it is referenced to machine Z at say machine Z=-8", work Z0=machine Z=-8". when G49 is issued, it cancels all compensation including the T99=6.5830" which makes the work Z0=machine Z-1.417. Then say T5 tool change is issued (T5 being 3.0155")... since all compensation has been canceled, the new work Z0 is actually machine Z-1.417" + T5 tool length of 3.0155" which is work Z0 = machine -4.4325. But the work Z0 should actually be machine Z-8". So there is a 3.5675 difference.
Confusing... yes... took me hours to figure out the math next to the Tormach.
There are 3 solutions I see. One is to not use G49 in the Gcode at all.... or 2 is to write in the Gcode a T99 to reference work piece after the G49 command. 3rd is to set T99=0 in the tool table so it will not cancel out the 6.5830"(T99 tool length).
I think I'm going to opt to delete the G49. No need to cancel the compensation if I am going to probe for the work Zero for the compensation before running the Gcode.
BTW... this problem exist on every Gcode with the G49 command unless the tool table is completely zeroed out.
Ken
apeman88 there is no problem with your G-codes.you see in the machine that the tool length compenseation is still from the first tool because the controller still hasn't read the H(the place where the tool length is in the tool table) so it cannot know what the length is of the tool.
One likely problem is shown below - the tool change T5 and the tool length offset H - should be the same number (address)
N6 M6 T5
(TOOL -5- MILL DIA 0.02 R0. MM )
G90 G00 G40 G54
G43 H14 D44 G0 X0.765 Y0.322 Z2. S3200 M3
M8
(----------------------------)
(1/4" VMILL ENG-ATD - PROFILE)
(----------------------------)
X0.765 Y0.322 Z0.4
Z0.079
Jeff
