[Green0]

I have a Hurco machine here- and I can skew the axis for a work offset so we don't have to indicate fixtures, saving time. Does the Fanuc OI-MD on the DNM5700 support this? I wasn't able to find any information on axis skus in the provided documentation.

It seems like it should be a function. I'm pretty sure Fanuc 31I's actually use a skew to drive Y axis offsets with X and Y motion in one of the machines on our floor, so it seems like Fanuc is certainly capable of driving a linear move using a compound axis motion.

[Green0]

I talked to someone at corporate. The impression I got was that it is not software supported- definitely not in the GUI software. There is also no work offset based skew support, so you can't have multiple work shifts on different skews as far as I know. There is some sort of macro function where you can manually program the skew- and it will handle one skew, but it seems that is probably actually harder to work with than touching two points, doing trigonometry, and using the G68 function like G68 X0. Y0. A0.1 <angle in degrees positive for counter clockwise from 3 oclock and negative for clockwise from 3 oclock.

Support in Fanuc for an angle value in each workshift and a two bore and line by two points skew function in the Renishaw GUI software would be massive improvement as this would support cad cam perfect code creating perfect work on imperfect workholding being re-used the second or third time for the same job.

[spackermen]

hi,

I am not totally familiar with the machine and exact controller. But if you have a probe you most likely have the macro function. And on pretty well any other machine I have been around if you have probing you also have coordinate rotation and scaling. You can look into G68/69 codes and that should get you in the ballpark.

The renishaw cycles for outside corner/inside corner will write angle and angle error into a variable and you can pull that into the g68 call to update your wcs. The problem is it’s not live axis skew using it in the program like this. So if you call g68 R1.22 and then jog the machine it will not show it has rotated. But in a program it will rotate the wcs.

Donno if this is what your after, I know you can input an angle into a fanuc wire edm and it will rotate all the globals so even when jogging it will remain in the skewed coordinate system but that’s the only time I have ever seen anything like what I think your after.

G68 will likely work for your application, however It is a solution that requires you to call and cancel it in program every time you want to use it.

[Green0]

I didn't find a solution to put angle skews into work offsets. I did use the G68 function to program a skew using two points with the renishaw, and a calculator on the internet for angle distance. It doesn't support efficient production manufacturing with multiple offsets, but it works ok for tool work without a lot of tools on one part.

[DouglasR]

OK. So, after a little digging in the Renishaw Inspec manual I found a few gems. One is the 9816 and 9815 Corner macro. This would be using the output something like:
M165 P9816 X2. Y2. B5.; Where as X and Y are nominal locations of a corner.
The "B" word is the angle tolerance.
The measurement values of this feature are stored in variables #135 thru #149. Variable #139 is angle of X surface measured from X+, #142 is value of Y surface measured from X+.
These values can then be used in your G68 rotation function to get the correct "skew" needed.
If you need the manual, I can send, in PDF.