[gpettit]

I have a 2012 VF-2 with the WIPS option. I have my probe in pocket 20 and in the tool offset table there is a length offset.

When I probe a part, does it use this length offset when setting the work offsets or is everything the probe needs stored in global variables? Is the length offset for the probe only used when positioning the probe during a part program?

When starting with a new setup, I would like to be able to hit origin and zero out all of my tool offsets to start with a clean table; however doing so would delete the probe tool offset. It would be nice if there was a setting that prevented the tool offset that was set as a probe from being zeroed.

Thanks,

Greg

[Matt@RFR]

Yeah, H20 is pretty important for you. If you really want to, you could enter your probe height offset value into a macro variable, then use that variable when calling G43. Like this:

G43 H#505

But, the Haas control is so easy to just overwrite values into all the offset registers, I'm not sure why you would want to zero everything first.

[txcncman]

I see your concern and understand what you wish to do by zeroing all of the offsets. I have found through much practical experience there is no reason to zero everything out. I reuse tools from part to part as habit. And would rather quickly change a tool number and offset and cutter comp number in a program than reset a tool. At least in my mind, changing the T, H, and D is faster than setting up a new tool to be probed.

[christinandavid]

I suppose you could write a macro program to clear a range of tool offsets or work offsets. Don't know how to assign a g code to the macro on haas I confess.

DP

[Matt@RFR]

I suppose you could write a macro program to clear a range of tool offsets or work offsets. Don't know how to assign a g code to the macro on haas I confess.

Sure, but I'd still like to know why?

[txcncman]

Would be easier to add a line to the probe macro that overwrites the offset to a correct value so that if current offset is 0.0000 it will be changed to correct value.

[gpettit]

Thanks, lots of good options.

I do find it easy to overwrite the tool table. Sometimes I just like to start with a clean setup and don't want to see other tools in my table. I think this helps to make sure a value is not left from a previous setup. Haas does have the offset filter setting 201, "Show only work and tool offsets in use"; however, you still see them during setup.

I made a suggestions to Haas to add a setting that would prevent a tool in the tool offset table that is set as a probe to not be cleared when you hit origin.

I would also like to say, I really love the probe option and I don't think I will ever get another mill without it!

Thanks again,

Greg

[angelw]

Thanks, lots of good options.

I do find it easy to overwrite the tool table. Sometimes I just like to start with a clean setup and don't want to see other tools in my table. I think this helps to make sure a value is not left from a previous setup. Haas does have the offset filter setting 201, "Show only work and tool offsets in use"; however, you still see them during setup.

I made a suggestions to Haas to add a setting that would prevent a tool in the tool offset table that is set as a probe to not be cleared when you hit origin.

I would also like to say, I really love the probe option and I don't think I will ever get another mill without it!

Thanks again,

Greg

Hi Greg,
You can easily achieve your aim by doing as DP suggested and use a User Macro program to clear all Offset except the one for the Probe.

The HAAS User Macro system allows Custom G and M codes to be created to call the Macro Program instead of using G65. This is achieved by registering the number of the G or M code you wish to create in a parameter that corresponds to a particular program number. This parameter/program number association is as follows:

M Code Parameters --- Associated Program Num
81 --------------------------------- 9000
82 --------------------------------- 9001
83 --------------------------------- 9002
84 --------------------------------- 9003
85 --------------------------------- 9004
86 --------------------------------- 9005
87 --------------------------------- 9006
88 --------------------------------- 9007
89 --------------------------------- 9008
90 --------------------------------- 9009

G Code Parameters --- Associated Program Num
91 --------------------------------- 9010
92 --------------------------------- 9011
93 --------------------------------- 9012
94 --------------------------------- 9013
95 --------------------------------- 9014
96 --------------------------------- 9015
97 --------------------------------- 9016
98 --------------------------------- 9017
99 --------------------------------- 9018
100 --------------------------------- 9019

To set a G or M code to call a Macro Program, the number of the G or M code is registered in an unused parameter in accordance with the above table, and the Macro Program is created using the Program Number associated with the parameter used to register the code. For example, to call a Macro Program with G100, the number 100 will be register in a parameter from 91 to 100. If the number is register in parameter 91, then program number O9010 will be used for the Macro Program. The Macro Program to clear all but the Tool Offset for the probe could be something like the following.

%
O9010
#1=1 (INITIALIZE #1)
WHILE [#1 LE 24] DO 1 (24 IS THE HARD CODEING OF TOOL MAG CAPACITY)
IF [#1 EQ 20]GOTO10 (BYPASS RESETTING OFFSET 20)
#[2000 + #1]=0 (RESTE LENGTH GEOMETRY OFFSET TO 0)
#[2200 + #1]=0 (RESTE LENGTH WEAR OFFSET TO 0)
N10
#1=#1+1
END 1
M99
%

The above Macro Program can then be called by commanding G100 via MDI.

In the above Macro Program, the Maximum Tool Capacity of the machine and the Tool Offset Number to avoid resetting are hard coded. These values could also be passed as arguments in the G100 call block. This would make the Macro a bit more flexible and allow a range of offsets to be Reset.

Following is the Macro Program call block and the modified Macro Program.

G100 K1 M24
Where:
K = The start tool offset num to reset.
M = The end tool offset num to reset.
%
O9010
(ERROR TRAP FOR ARGUMENTS PASSED)
IF[[#6 EQ #0]OR[#6 LT 1] OR [#6 GT 24]]THEN #6=1
IF[[#13 EQ #0]OR[#13 LT 1]OR[#13 GT 24]]THEN #13=24
IF[#13 LT #6]GOTO20
WHILE [#6 LE #13] DO1 (#13 IS THE LAST TOOL OFFSET NUM TO PROCESS)
IF [#6 EQ 20]GOTO10 (BYPASS RESETTING OFFSET 20)
#[2000 + #6]=0 (RESTE LENGTH GEOMETRY OFFSET TO 0)
#[2200 + #6]=0 (RESTE LENGTH WEAR OFFSET TO 0)
N10
#6=#6+1
END 1
GOTO30
N20
#3006=1(OFFSET RANGE ERROR)
N30
M99
%

In the above Macro Program, if any argument is omitted from the Macro Call command block, default values will be used.

I've only just written this Macro Program and haven't tested it on a machine. It looks OK and should work without error. If you use it, proceed with care.

Regards,

Bill

[gpettit]

Bill thanks for taking the time for such a detailed post! I will write the macro and let you know how it goes. Thanks again and hope everyone has a great weekend.

Greg