Fanuc 16i G43 Z+ Overtravel

I've seen others here with this issue and did a ton of research looking for other threads that could help solve this problem with G43 triggering a Z+ overtravel alarm after a tool change. In other Fanuc controls you can change P5006.6 to 1 to stop Z axis motion and resolve this. I have a Robodrill 21iD with a 16i-MB that has this issue and cannot figure out how to resolve it. Looking through the manual for P5006 only shows a bit for automatic offset for inch and metric conversion at Bit(0). I tried setting 5006.6 to 1 but no luck. I checked the current parameters of tool compensation and only see 5001.1 (TLB) as active. I am setting tool offsets referencing the spindle face on a 123 block so that the offsets are positive and are the gage length of the tool. Any help or ideas would be much appreciated.

A sample of code for a job I am running will produce a Z+ overtravel right when the next tool offset is set.

%
O2121
(T4 D=0.375 CR=0. - ZMIN=0.125 - FLAT END MILL)
(T5 D=3. CR=0. - ZMIN=0.7156 - FACE MILL)
G90 G94 G17 G49 G40 G80
G20
G53 G00 Z0.

(FACE1)
M06 T5
S2063 M03
G54
M08
G5.1 Q1
G00 X6.2602 Y6.95
G43 Z1.35 H05
G00 Z1.0156
G19 G02 Y6.65 Z0.7156 J-0.3 F40.
G01 Y5.
Y0.
G17 G02 X3.8568 I-1.2017
G01 Y5.
G03 X1.4535 I-1.2017
G01 Y0.
G19 G02 Y-0.3 Z1.0156 K0.3
G00 Z1.35
G17
M05
G53 G00 Z0.
G49
G5.1 Q0

(2D ADAPTIVE1)
M09
M01
M06 T4
S9002 M03
G54
M08
G5.1 Q1
G00 X7.5845 Y-0.0294
G43 Z1.35 H04
G00 Z0.95
Z0.5162
G01 Z0.4787 F108.
Z0.4
G03 X7.3804 Y0. I-0.2376 J-0.9274
G01 X7.3789
X7.3664 Y-0.0194
X7.3519 Y-0.0374
X7.3357 Y-0.0539

...try replacing G43 with G44 and see what happens
https://cnc-programming-tips.blogspo...pensation.html


Note: After changing any Params you must restart the machine to activate.

Setting to G44 triggers a Z- overtravel right away. I set 5006.6 and power cycled with no luck. What is confusing me is there is no issue on the first G43 H** in the program.

So when M6 is called for a tool change G91 is set and does not get set back to G90 before the next G43 offset is called which causes the overtravel situation. I'm sure this could be resolved by changing something in the tool change coding which is the right way. Instead I modified the post processor to call a G90 after the work offset callout on every tool change.