Writing values to a Heidenhain tooltable

[Chipmakr]

Does anyone know if it is possible to write values to an active Heidenhain tooltable?

 

I want to write a "zero" into the radius column if the tool is using cutter comp. This would be about the same as loading with G10 on a Fanuc style control.

[Steve Hattori]

Which model is the control? We have the 530, and I don't know how you can get mastercam to post out a value to the tool tool table- we generally edit it in Cimco 5 after reading it from the machine with TNCRemo. Most times, we just set tool

lengths using the laser's 583 cycle, which does only lenght, and no radius. I try NOT to edit tool tables offline- if you change a dimensional value and don't re-set the tool in the machine, obviously this can cause a problem....

We mostly only use posted mcam programs with wear comp, and don't have a radius value in the tooltable unless the cutter needs a small adjustment.

[silky_johnson]

I'm not sure about the Mastercam side of things but if your post can output "FN17:syswrite" and then the proper index and number (see the manual) this should work.

 

Steve, cycle 583 will work for bsll mills but is less accurate for endmills and bull nose cutters due to the fact that it does not use the "R:offs" value in the tool table.

[Chipmakr]

HSM400:

Do you have a example of the FN17 syntax writing a value back to the system? I do not see any reference to it except within the probing manual and it does not show an example of passing along a value.

 

Steve:

We are working on the TNC 530 control. I can get our post to output whatever commands are needed

but from what I can see in the Heidenhain manuals it does not seem possible to write to the active tool table. We have been in the habit of lasering tools with cycle 584 L&R. We really like being able to evaluate the tool runout using this cycle even though we do not use the R value at all. If we have to change the R value manually we are just asking for trouble down the road. If I could automate it this would let us evaluate runout and eliminate problems with the R value down the road.

 

I will just put a statement in the post that states if cutter comp is used in a operation change the R value to zero.

[Chipmakr]

Well I just went out to the machine and tried the text.

 

FN 17: SYSWRITE ID50 NR2 IDX102 = 0

 

and it worked. The R value for tool #102 was set to zero automatically.

 

Thanks for the help.

[Steve Hattori]

HSM, you are right about the 583 not using R-offs- Thanks for that clarification. The 584 set to 0 will just do length, but still uses the r-offs, so thats what we'll do...

And the FN17 was a good tip- thanks!