Z axis over travel with probe routines on Mazak Reinishaw Probe

[cjelley]

I am hitting the soft limit in Z when trying a probing inspection routine. Any ideas what's wrong here?

O5556 (PROBE UPDATED MACHINE CONFIG)
(MACHINE)
( VENDOR: MAZAK)
( DESCRIPTION: MAZAK VCN-570C)
(T30 D=0.2362 CR=0.1181 - ZMIN=-0.9862 - PROBE)
G90 G94 G17 G49
G20
G53 G0 Z0.

(PROBE WCS3)
G90
T30 M6
(RENISHAW OMP60 6MM X 100MM)
G54
G0 X0. Y0. ==========> (THIS LINE IS WHERE THE MACHINE TRYS TO MOVE + IN Z PAST MACHINE POSITION Z0)
G43 Z3. H30
G65 P9832
G65 P9810 Z1. F100.
G65 P9812 Y7.5 Z-0.9862 Q0.4 R0.5 W1. S1.
G65 P9810 Z1.
G0 Z3.
G65 P9833
M5
G53 Z0.
G53 X0. Y0.
M152
M30

With this line of code in MDI:



G0G90G54

G43 Z3.0 H30



The probe goes right to Z3.0 with no problems.



Distance from Z3.0 to the Z soft limit is 7.0918



Just an idea:

Probe length is 8.41757

Could the problem be in G65 P9832

Due to the probe length?

 

[CNC Hacker]

Usually this is from a mismatch of settings program 9724 and the machine tool offset parameters. The probe can look at the Tool Data page or the Tool Offset page. Check the setting of #120 in 9724. If all your lengths are on tool data, set #120 = 1. This would be with parameters F93 bit 3 = 1 and F94 bit 7 = 1.

If you're using the tool offset page (F93.3 = 0 and F94.7 = 0), set #120 to 2 for Type A offsets (one entry for every number) or 4 for type B (separate length and radius fields for every number).

The settings are shown in chapter 11 of the Inspection Plus manual. If you do change #120 you will need to recalibrate the probe and put the tool length in the appropriate field.

 

[MacroGcode]

P9832 is used to turn the probe on.
It could be a readahead issue.

 

[cjelley]

Are these parameters for a Mazak Smooth G?

 

[cjelley]

I just checked the machine...

Program 9724 #120=1
Tool Lengths are on Tool Data

Funny that you mention this, I've used the probing cycles in the past and had no issues. The Mazak applications guy was here yesterday and switched the machine to use the tool data page for comp wear Z (H) and comp wear (D). I'm not sure if this caused the problem but it sounds like you are onto something. I will check F93 Bit 3 and F94 Bit 7 now.

Do my parameters seem correct?

 

[CNC Hacker]

Yes the parameters are for SmoothG.

Yeah if you were using the tool offste page before for wear comps that could explain it, are there any values on the tool offset page for #30?

 

[cjelley]

F93 00001000
f94 01010100

 

[cjelley]

No values on Tool offset page for #30

 

[cjelley]

Yes the parameters are for Smooth G.

Yeah if you were using the tool offset page before for wear comps that could explain it, are there any values on the tool offset page for #30?

To be clear, I was using only the Tool Data page for offsets, the Mazak Applications Guy set the machines up to use Tool Offset in addition to Tool Data. For example if I have T02 -.001 Comp (D) on Tool Data and T02 -.001 Comp (D) when running the program the machine combines the two offsets so the tool will run with -.002 Comp.

 

[CNC Hacker]

Ah ok, that was my suspicion. In that case, I think you need to set #120 = 3 for "ISO tool data".

 

[MacroGcode]

F93 00001000
f94 01010100

#116 will show the active tool length.
It would appear your #120 setting is wrong. What is the parameter O4 set to?

 

[SpeedsandFeeds]

It could be a simple mistake.

You should have your code in this order
;
G00G90G54
G43 H30 Z3.0;
G00X0.Y0.;
G65P9832;
;

 

[cjelley]

Problem solved for now. I believe I need to modify Renishaw program 9750 or 9754 #102 value.

F93.3 = 1.
F94.7 = 1. (WAS 0)

This is what is causing a conflict between the using the tool offset page for comp along with renishaw macros.

CNCHACKER, You were right! Thank you.