Haas T and D agreement

[Flycut]

Does anyone know how to assign a macro to the diameter offset on a Haas the way it works on the height offset or some trick to accomplish the same thing?

[gcode]

The Haas controls I ran in the 90's had a Setting that would throw an alarm if D and H did not match

It's my understanding that the control settings in modern Haas machines are locked down and require
a deal USB hasp to change them

[Flycut]

I can change H and T agreement without a hasp but I don't even see a setting for D and H
Or D and T for that matter

[JParis]

https://www.haascnc.com/service/codes-settings.type=setting.machine=mill.value=S15.html">https://www.haascnc.com/service/codes-s ... e=S15.html">https://www.haascnc.com/service/codes-settings.type=setting.machine=mill.value=S15.html

[kccadcam]

Also, you can use Variable #3026

[media]">[/media]

[Flycut]

I like using the #3026 method but that doesn't prevent somebody from missing a D offset with the wrong value when changing tool numbers.

[CNCAppsJames]

One could always add a MACRO variable to the tool change cycle and use MACRO variables as H and D instead of hard numbers then you never run the risk of running the wrong H/D offset.

Just a thought.

[Flycut]

But if D is found anywhere within the program will it not simply override anything applied in the tool change macro?

[CNCAppsJames]

But if D is found anywhere within the program will it not simply override anything applied in the tool change macro?

My apologies, I don't think I explained this well enough.

In the Tool change MACRO, after the M06 happens, the control "knows" what tool number is in the spindle. That number is stored in a system variable. So, after the M06, one could set the value of a Common Variable to be the same as the System Variable.

Let's pretend we're calling T74. "74" would be in the control's system variable after the M06, so after the M06 happens we can set variable say #517 to be equal to the system variable's contents. Then in your part program instead of calling G43 H74 and G41/G42 D74, we would now call G43 H#517 and G41/G42 D#517.

Now you never run the risk of the wrong tool offset being used.

JM2CFWIW

[Flycut]

Might have helped If I explained what I was doing as well.
I am in the middle of implementing a "Master" tool list on every machine.
80% of our jobs can be done with a bout a dozen common tools.
As we run old proven programs, we are reassigning those tools to match the Master list.
We need to change the T, H and D to the new list as we go along.
The post here is set up to spit out a D with every G41 or G42 line.
I'm telling everyone that only one D is needed and should be kept on the G43 line along with H.
Sometimes, because there are so many or they are in a subroutine, some get missed.
I would have liked to have a safety net the way T and H work together.

[CNCAppsJames]

By using the variable method, you would only need to change the T and not have to worry about H's and D's.

For the majority of the machines I support we use that as opposed to actual numbers for H and D. It serves two purposes, 1 - tool life management and 2 - ensures the correct offset is activated with the tool.