Wierd tool offset issue <resolved, set tool # when setting Z 0>

[GDawson]

Good Morning, Thanks for the replies, I'll try to answer as best I can..
we are using g43 and h1 (for this program anyhow)

We do have a rack type tool changer, the program is from the centroid website modified by me..

We don't maintain a tool library per se, but we do manually touch off each tool we are planning on using per program and enter the offsets in the tool offset library

all axis's have home switches and home to them

for tool setting we use either a mechanical switch or manually touch off on top of the work, Z zero is at the top of the travel (home) and all offsets are negative

I'll grab the report zip here in a second

As said it seems to snap around if you visit the tool offset page..
Thank you,
Greg

Heres the header of the G code ( I didnt post the whole thing cause its spaghetti and it gets in trouble right off when it decides to get in trouble)

%
O1123
(T1 D=1. CR=0.5 - ZMIN=-0.7832 - ball end mill)
G90 G94 G17
G20
G28 G91 Z0.
G90
(Parallel1)
T1 M6
S10000 M3
G17 G90 G94
G0 X4.3167 Y-1.4901
G43 Z0.6 H1
G1 Z0.099 F40.
G18 G3 X4.2168 Z-0.001 I-0.1 K0.
G1 X1.4455 Z-0.0035
X0.0396 Z-0.0052
G3 X0.0176 Z-0.0001 I-0.0001 K0.05
G2 X-0.0044 Z0.005 I-0.022 K-0.0449
G1 X-0.0045
X-0.0067 Y-1.49
X-0.0089 Y-1.4898 Z0.0049
X-0.011 Y-1.4894
X-0.0131 Y-1.4889 Z0.0047
X-0.0152 Y-1.4882 Z0.0046
X-0.0172 Y-1.4874 Z0.0044
X-0.0192 Y-1.4864 Z0.0042
X-0.0211 Y-1.4853 Z0.004
X-0.0229 Y-1.4841 Z0.0037
X-0.0246 Y-1.4828 Z0.0035
X-0.0262 Y-1.4813 Z0.0032
X-0.0276 Y-1.4797 Z0.0028

[GDawson]

And here is the compressed report file from today

[GDawson]

As to the which method of offset from your discussion paper Keith, we have a reliable z home we use as 0, and use method one, no reference tool

[cnckeith]

; ICN_PATH = C:\intercon\g43.icn
; --- Header ---
N0001 ; CNC code generated by Intercon v5.09 BETA, Rev 4
; Description:
; Programmer:
; Date: 27-Feb-2024
M25 G49 ; Goto Z home, cancel tool length offset
G17 G40 ; Setup for XY plane, no cutter comp
G21 ; millimeter measurements
G80 ; Cancel canned cycles
G90 ; absolute positioning
G98 ; canned cycle initial point return
; --- Tool #1 ---
;Tool Diameter = 20.0000 Spindle Speed = 1200
;Center Drill
G49 H0 M25
G0 X-5.0 Y0.0
N0002 T1 M6
S1200 M3
G4 P3.00 ; pause for dwell
G43 D1
; --- Rapid Traverse ---
N0003 M25 H1
X10.0 Y0.0
; --- Line ---
N0004 G1 X10.0 Y0.0 Z-1.0 F10.0
; --- Line ---
N0005 X0.0 Y0.0 Z-1.0
; --- End of Program ---
N0006 G49 H0 M25
G40 ; Cutter Comp Off
M5 ; Spindle Off
M9 ; Coolant Off
G80 ; Cancel canned cycles
M30 ; End of program

[GDawson]

Hi Keith,
We have tried canx the offsets with g40 / g49 and it seems to have no impact.. here is another program posted from mastercam that sometimes works sometimes not..

%
O00119
(FINGERBRD6)
(DATE=24-02-24 TIME=10:51)
(UNDERSIDE AND SIDES LONG)
G20
G0G17G40G49G80G90
(1" BALL ROUTERBIT)
T1M6
G0G90G54X.8866Y-2.3196Z0.S10000M3
G43H1Z2.
Z-.2241
G1Z-.4741F30.
X.8955Z-.4794

[cnckeith]

ok, we need to know your work flow. lay it out step by step

1.) .....
2.) ....

etc..

[GDawson]

1: power up centroid and start CNC12
2: hit reset, home machine
3: load program
4: find WCS xy (set G54 0)
5: If tools are new touch off on top of stock and record values in library (EX -4.474)
6: set z wcs to machine 0
7: if z dro read out shows other than 0 zero out dro
start program
8: this is where it throws a z overtravel alarm, but not always.. Often re running the program will cause the alarm even if it has worked previously

when we get the overtravel alarm you can usually get it to go with a combination of visiting the tool library (don't change anything) re-zeroing z to home position and Z WCS, and holding your mouth just like so on one foot.

We have noticed It does a very good job remembering the XY WCS zero, but the Z WCS is not reliable it does not seem to reliably recognize / apply the recorded offsets when you call a g43.

Thanks,
Greg

[grossmsj]

Next time you do this, notice the state of the Tool/Tool Height Offset. It is in the middle of the screen, second line from the top. It will appear as either T1 H1 or T1 H-.
My guess is that you are setting the wcs Z0 when that line reads T1 H-.

You need to have that line read T1 H1 when you zero. That requires a manual G43 H1 in the MDI.

[cnckeith]

1: power up centroid and start CNC12
2: hit reset, home machine
3: load program
4: find WCS xy (set G54 0)
5: If tools are new touch off on top of stock and record values in library (EX -4.474) < tools should not be reference to the top of the stock>
6: set z wcs to machine 0
7: if z dro read out shows other than 0 zero out dro
start program
8: this is where it throws a z overtravel alarm, but not always.. Often re running the program will cause the alarm even if it has worked previously

when we get the overtravel alarm you can usually get it to go with a combination of visiting the tool library (don't change anything) re-zeroing z to home position and Z WCS, and holding your mouth just like so on one foot.

We have noticed It does a very good job remembering the XY WCS zero, but the Z WCS is not reliable it does not seem to reliably recognize / apply the recorded offsets when you call a g43.

Thanks,
Greg

[cnckeith]

if you decide to maintain a tool library with height offsets
setting tools lengths and setting part z zero positions are two completely different operations. don't mix them and don't confuse them.
setting height offsets using the top of the stock is fraught with dangers.

i go over all this in my 20 year old CNC videos for both the machine home as reference method and the reference tool method.