[inthebay]

Hey guys,

I'm running a job at the moment and have just set up ~24 tools in our EC400. Now the tools that require diameter probing do so nicely, and output the measured diameter into the tool diameter column of the offsets page. However, this alters the diameter in the control, and doesn't change the wear column.

Currently, I'm using Mastercam X8 and having it use wear compensation (rather than control) because it has less of a chance for catastrophic failure (a few thou here or there rather than half a tool). Is is possible to either:

A: Change how the probing system outputs its diameter settings, along the lines of "Actual Diameter"-"Diameter" and input that into the wear column? or:

B: Should I just be using control compensation and stop worrying about it.

Thanks!

EDIT1:

After much googling, I found this Thread

Which provides the following:

I can do it here, I guess. It's not like a secret Fanuc parameter or something.
In the case of which I speak, the edit is in program O09852. I would suggest uploading it somewhere for safe keeping, just in case it gets hosed up.
Anyway, change setting 23 to OFF, so you can edit 9000 series programs.
Open O09852.
Find the line N31.
The next line should read: #[ 2400 + #7 ]= #8 / #156
Change it to: #[ 2400 + #7 ]= #8 / #156 - #19 (add the -#19 to the end)

When finished, select some other program than a 9000 series.
Reset setting 23 to ON.

Try it, but check what it enters into your offset page before you run that tool.
Setting 40 on our VF3 is set to "DIAMETER". If the tool is supposed to be .500 and is .490, our offset page will show -.010.
Again, verify what's entered into your offset table vs. what setting 40 is set to before running.

I'm going to give that a shot, I guess.

EDIT2: So I gave that a shot, and it outputs the amount of wear correctly, however does so into the tool diameter column, not the wear column.

Any ideas?

[haastec]

Hey guys,

I'm running a job at the moment and have just set up ~24 tools in our EC400. Now the tools that require diameter probing do so nicely, and output the measured diameter into the tool diameter column of the offsets page. However, this alters the diameter in the control, and doesn't change the wear column.

Currently, I'm using Mastercam X8 and having it use wear compensation (rather than control) because it has less of a chance for catastrophic failure (a few thou here or there rather than half a tool). Is is possible to either:

A: Change how the probing system outputs its diameter settings, along the lines of "Actual Diameter"-"Diameter" and input that into the wear column? or:

B: Should I just be using control compensation and stop worrying about it.

Thanks!

EDIT1:

After much googling, I found this Thread

Which provides the following:

I can do it here, I guess. It's not like a secret Fanuc parameter or something.
In the case of which I speak, the edit is in program O09852. I would suggest uploading it somewhere for safe keeping, just in case it gets hosed up.
Anyway, change setting 23 to OFF, so you can edit 9000 series programs.
Open O09852.
Find the line N31.
The next line should read: #[ 2400 + #7 ]= #8 / #156
Change it to: #[ 2400 + #7 ]= #8 / #156 - #19 (add the -#19 to the end)

When finished, select some other program than a 9000 series.
Reset setting 23 to ON.

Try it, but check what it enters into your offset page before you run that tool.
Setting 40 on our VF3 is set to "DIAMETER". If the tool is supposed to be .500 and is .490, our offset page will show -.010.
Again, verify what's entered into your offset table vs. what setting 40 is set to before running.

I'm going to give that a shot, I guess.

EDIT2: So I gave that a shot, and it outputs the amount of wear correctly, however does so into the tool diameter column, not the wear column.

Any ideas?

It will work with the value in either column, but I would prefer that it be in the wear column as well.

Although I do not have the answer to your question, but if nobody else comes along with a solution, get in touch with Renishaw USA. I have used them many times for technical support with questions similar to what you are asking and they have been nothing but helpful.

Good luck!

[Ydna]

I'm not in front of a CNC right now, but perhaps try this and see what happens:
#[ 2600 + #7 ]= #8 / #156 - #19

The reasoning for that is as follows. Haas uses variables #2401-2600 for the diameter geometry column, and variables #2601-2800 for the diameter wear column. The fix you're looking for might just involve editing that "starting" value in the o9852 subroutine to accommodate the correct column.

I'd try it out myself but would need to wait until we're in the middle of a changeover...

EDIT! I'm looking at the o9852 subroutine right now. I see the very next line is meant to zero out the diameter wear column (#[2600+#7]=0). You'll have to get rid of that or switch it to initialize the dia geometry register instead, by setting the value to 2400 instead of 2600.
Maybe try this group of lines instead....
N31
#[ 2400 + #7 ]= 0 (CDC diameter)
#[ 2600 + #7 ]= #8 / #156 - #19 (CDC wear "difference")

[Matt@RFR]

I don't use the tool setter to set diameters anymore and I've never done this, but I have a note that indicates the use of input Ii.iii on a G65 P9852 or P9853 line will use nominal dia to output wear size instead of measured dia. So it would be like G65 P9853 B3 T1 D1 S.5 I.5 I guess. Might need to drop the S.5. That would be for 1/2" tool in T1.

[Ydna]

hmmm, I can't get the I-input to work myself. Have you tried it on yours? (might be a different revision of the renishaw programs)
On my machine, it seems to compound the inputs for I and D together, and ends up being twice as far from the presetter head that it should be. When I try it with a 3/4" diameter endmill, the machine positions the tool as if it were a 1.5" diameter cutter. I can't get it to play nice.

I did test out the modified 2400-to-2600 code though, it seems to work.
EDIT - I had originally typed a bunch of crap about changing the branching routines to accompany the changes (o9023 and o9995) but I tried out my suggestion and it screwed everything up. so nevermind