Large Diameter Broken Tool Probe Check

[McLaren]

 Still having issues finding anything with search so sorry if this has already been answered. I'm trying to figure out how to check a >.500" diameter tool for breakage but can't locate any literature on what the cycle options are. Right now our post spits out;

G65 P9023 A24. T28 H.005

Which I understand will check tool 28 and alarm out if it's off by more than .005". However searching my renishaw pdf's I am not finding any 9023 codes, and searching the haas manuals is no luck either. Anyone have any thoughts? Machine is an UMC750 with renishaw probing option. Thanks in advance!

[Tim Johnson]

If you're using the NC4 then the edge checking macro is O9862. The broken tool detection (plunge checking) is macro O9863.

[civiceg]

Haas uses its own macros to populate Renishaw's. You are using Renishaw's macros in the end. I don't believe you can start off with using the Haas macro to step off center to probe a large tool for tool breakage, as it remains on center. I mean you can but if its an end-mill you will have to increase your tolerance, due to the angle on the bottom of the endmill. If its a shellmill, than probing on center is a no go, due to the large difference between insert and center bolt.

If you really have to you can type the long hand Renishaw tool breakage call (from the Haas Renishaw macro manual), which will move over the radius of the tool and spin. 

As the Haas GUI does not support what you are after, but Renishaw does. 

[civiceg]

Haas GUI-->Haas Macro to populate Renishaw--> Renishaw macro drives probe

[McLaren]

Problem solved!

G65 P9853 T25. H0.010 B1. S1.6

T - Tool number

H - Tolerance

B - Length Only

S - Tool Diameter

 

Using manual entry like so to check a facemill between z depths:

 

M89
M05
G255
G53Z0.
G53X-30.Y0.
G49
G65 P9853 T25.H.010B1.S1.6
G00 G17 G90 G54
M88
S310 M03
B0. C0.
G254
B0. C0.
X-4.547 Y1.1969
G43 H25 Z3.