What's new
What's new

Probe setup using different height offset

Fellhoelter

Plastic
Joined
Nov 22, 2011
Location
Hazlehurst, Mississippi
So, naturally a 10 tool changer isn't enough.

How do I setup the Renishaw probe on a TM-1P to use a different height offset than the tool number that is in the spindle?

I'd like to set tool #50 to be the probe... (or any random # other than T10)

The tech set it up as tool 10, but my very first program needs 10 tools...

I am sure there is a setting somewhere to to read T10 H50, but I can't find it.

Basically, I'd like to be able to use all 10 tools, and insert and use the probe when I need it, but not as part of a program.
 
Last edited:
OK, so further experimentation has shown that setting one of the work offsets uses the H value of the tool in the spindle.

I would like to set it to use a specific H value... Not the one in the spindle.
 
If you run WIPS under VCQ, choose "Probe calibration" and then "Spindle Probe Z Calibration of TS27R". Key in the desired tool number and follow the instruction. This will set up the probe as a new tool. I don't think you can do it with different H values since it is stored in a macro variable.
 
Leave the probe as T10 H10...make your tool T10 H20(or whatever H value you see fit). Make sure you turn off the H and T agree setting.
 
If you run WIPS under VCQ, choose "Probe calibration" and then "Spindle Probe Z Calibration of TS27R". Key in the desired tool number and follow the instruction. This will set up the probe as a new tool. I don't think you can do it with different H values since it is stored in a macro variable.
All this seems to do is output the Z offset to the specified tool, it doesn't make it call that tool later, when actually probing.
I have learned a little since I posted, since I have been fixated on this issue.
Turns out, at least in my version of WIPS (V2.8) that the macros have a call out for variable #3026, which is the current tool in the spindle.
So, they always use the H value from the tool in the spindle.
I edited this out on my PC, making them all call H30 instead of #3026, reloaded, and at least so far, it is working.
I have not tested all of the probing cycles though, so time will tell if it's a real fix or not.
At least now, when I am setting up my work offsets, it is functional.

Leave the probe as T10 H10...make your tool T10 H20(or whatever H value you see fit). Make sure you turn off the H and T agree setting.
That is one of several workarounds, but I hate working around stuff...
 
OK,if it works for one probe cycle it will work for all. WIPS is built on top of Renishaws macros and always calls the same "sub macro" to do the same things.
I once made some custom probe routines in WIPS and spent a lot of time following the calls since i did not have the documentation.
 
If you say so I guess it is that way. It was a year ago or so I worked with it and it was 2.7.

But still think it sounds strange. As long as no measurements are done in the Z direction the H value should not matter. If you can probe correctly in Z, everything should work.
You might have changed to much. Did you just "search and replace" or made an effort to understand the function at the different locations?
 
Oh, I made a very concerted effort to understand what I was doing, and not just blindly replace things.
There is one call out I replaced though, that concerns me.

It's not just a height callout, but a formula of some sort.

#[ 2000 + #3026 ]= #[ 2000 + #3026 ] + #192

Changed to

#[ 2000 + #2030 ]= #[ 2000 + #2030 ] + #192
 
#[ 2000 + #2030 ]= #[ 2000 + #2030 ] + #192


2000 + (10) would give you variable #2010, which is the height offset for tool 10.

#192 is a general purpose variable. You can do a search for this further up in the program to see what is being input here.

This exchange would not work.

Instead:
#2030 = #2030 + #192
 








 
Back
Top