Renishaw probe

[machine_man]

I have a part that is first turned on a lathe and has holes drilled around the face of the part at weird angles and a flat milled on the edge of the part. It is a muilti axis lathe/milling machine. Anyway the part is then taken from that machine and put into a 3 axis TR3 Haas where is has surfacing done to both sides. The machine is equiped with a renishaw probe, but we use a dile to ensure the flat is in the machine perfectly straight with the "Y" axis.

My question is:

Can I eye ball putting the part in straight and probe the part so there is some sort of a degree offest?

The program is in G-code and since it is surfacing two concave circles in diferent directions the program is very long, so it would have to be a code that applies to everything, not a code on each line.

Hope this makes sence

Thanks

[christinandavid]

You can use the probe to find the angle of rotation then use G68 to rotate your program by the result.

DP

[txcncman]

You can use the probe to find the angle of rotation then use G68 to rotate your program by the result.

DP

+1

Actually you will probe 2 points along one side, a known distance apart, and the calculate the angle. I do not recall that any of the probing macros automatically calculate angle for you.

If possible, I would recommend placing a flat edge against the fixed vise jaw, making sure my vise was indicated in square. Then do all of the programming and machining based off that.

[machine_man]

This is how I am doing it right now. I just thought maybe it was possible to do it the other way. I know some machines with advanced conversational can do it, but I don't know how to do it in just plain "G-code"

[txcncman]

The probing is not done with "just plain G-code". It is done with macro programming, a much more advanced way to program, in my opinion. The rotation of a coordinate system is done with G-code and is outlined in the Haas manual. Read up on it and then come back here with any specific questions you might have.

[Matt@RFR]

I do not recall that any of the probing macros automatically calculate angle for you.

Any probe routine that touches two different points will store an angle in #189. BUT, I think you're right that there isn't just a one-liner that will work for this. Here's what I would try, assuming the flat is facing away from the operator (Y+) and is 2" long and G54 is the center / top of a 6" OD turned part:

M6 T25
G43 H25
G65 P9832
G103 P1.
G0 G54 X.875 Y3.1 Z.5
G65 P9810 Z-.25 F150.
G65 P9811 Y2.8284
G65 P9834
G65 P9810 X-.875 F150.
G65 P9811 Y2.8284
G65 P9834 A0.
(THE ANGLE OF THE FLAT SHOULD NOW BE STORED IN #189)
G68 X0. Y0. R#189
G65 P9833
G103
M6 T1
(MACHINE PART)

[mick.w]

have you tried using p9814, we use this for working out angle to rotate table on horizontal borers, not sure however if it can be used for rotating coordinate system using g68

regards

mick w

[Optics_Mfg]

Take two points of the flat part as far away as possible from one another and calculate the slope of that line which should give you the angle. Do it with optics with a Renishaw OMP-400 with a 10mm stylus. You will have to look in the Renishaw manual to get the correct macro and just put it in the front end of your program and like said below use G68 #N. N being some variable you store in your locals and have that macro spit it out and use that to rotate your corrdinate system us G68 X0. Y0. R#N.