Angle Plane

I have a mold half that OP2 seems to be difficult to indicate. Can I use the offset of the two through-holes to tell the control to shift the angle of the G17 plane, and pick one of the holes as the WCS? That would seem way more accurate to me than indicating a surface I have no access to.

I'm using a Mitsubishi Meldas 64s control with a Haimer probe and spindle-mounted DTI. First, is this possible, and second, what is the parameter for this?

Alright, I figured out that it requires G68 and cancels with G69. Does that mean I need this value in the program or does G68 just call a value I have inputted in parameters?

When doing mold work we would ALWAYS reference the center of the plate by sweeping the sides of the plate with an indicator, ALWAYS! My answer to your question would be to adjust the plate so it was parallel with your axis vs rotating the coordinates.

Also, my experience with those clamps was they don't work very well, as in not well enough to use. I found it very hard to get them to stay in place on the table well enough to clamp the part. If you have been using them for awhile and like them disregard my thoughts about them. If this is your first rodeo then watch out as they may shift and lose clamping pressure.

DavidScott said:

When doing mold work we would ALWAYS reference the center of the plate by sweeping the sides of the plate with an indicator, ALWAYS! My answer to your question would be to adjust the plate so it was parallel with your axis vs rotating the coordinates.

Also, my experience with those clamps was they don't work very well, as in not well enough to use. I found it very hard to get them to stay in place on the table well enough to clamp the part. If you have been using them for awhile and like them disregard my thoughts about them. If this is your first rodeo then watch out as they may shift and lose clamping pressure.

Click to expand...

I hear you. Normally I would sweep a side square or put it in a vise, but the plate is too big for vises and I just got these clamps to try this out. They seem to move when I tighten them, I can confirm. That's why I figured I would figure out the angle once it was tight and then adjust fire with G68 (which I have never used before).

First OP, for sure I would start with top center. Second OP, there is no top center!

EDIT: Just thinking, if it isn't straight, I CAN'T indicate top center, BTW. It has to be a bore reference!

Veteran Bicycle said:

I hear you. Normally I would sweep a side square or put it in a vise, but the plate is too big for vises and I just got these clamps to try this out. They seem to move when I tighten them, I can confirm. That's why I figured I would figure out the angle once it was tight and then adjust fire with G68 (which I have never used before).

First OP, for sure I would start with top center. Second OP, there is no top center!

View attachment 263056

Click to expand...

If you haven't used these clamps yet I would say send them back!!!! Just my opinion of those things. Trying to adjust the coordinate system for out of square parts while trying to hold tenths, I am assuming, sounds like too many things can go wrong to me. Unless you are facing the top how about strap clamps with the plate on some 1-2-3 blocks? If strap clamps are too high try toe clamps. I still see top and center of that plate as my reference. I would also rough that plate out before finishing if I was making it from scratch, that looks like a prime candidate for movement. But it is nice that it will be bolted to a solid plate and clamped under high pressure when in use so some movement won't matter in use, just a PITA when doing any subsequent machining.

Edit: Cleaning up after a brain fart.

Veteran Bicycle said:

Alright, I figured out that it requires G68 and cancels with G69. Does that mean I need this value in the program or does G68 just call a value I have inputted in parameters?

Click to expand...

For starters, G68 is an option that not all machine builders or buyers spec. Have you tried it to see if the control generates an alarm? You can just use MDI and key in G68 X0 Y0 R90. input and press cycle start. If the option is not available you will get some kind of alarm saying invalid command or similar.

Your G68 line will need an X and Y position about which to do the rotation and an R value which would be the angle to rotate. Most of the time i have seen X0 Y0 used for the center of rotation. Your R will have to be calculated using the positions of the reference holes.

Vancbiker said:

For starters, G68 is an option that not all machine builders or buyers spec. Have you tried it to see if the control generates an alarm? You can just use MDI and key in G68 X0 Y0 R90. input and press cycle start. If the option is not available you will get some kind of alarm saying invalid command or similar.

Your G68 line will need an X and Y position about which to do the rotation and an R value which would be the angle to rotate. Most of the time i have seen X0 Y0 used for the center of rotation. Your R will have to be calculated using the positions of the reference holes.

Click to expand...

No error.

Which is preferable?

1) G68 X0Y0 R0.01 - before the first tool
2) G68 X542.262 Y-137.593 R0.01 - (the G59 position) before the first tool
3) G68 X0Y0 R0.01 - after G59 on every tool
4) something else

I'm trying to wrap my head around what happens to the WCS when the XY plane is rotated. Does the machine still respect absolute positions like my G59 hole location?

Vancbiker said:

For starters, G68 is an option that not all machine builders or buyers spec. Have you tried it to see if the control generates an alarm? You can just use MDI and key in G68 X0 Y0 R90. input and press cycle start. If the option is not available you will get some kind of alarm saying invalid command or similar.

Your G68 line will need an X and Y position about which to do the rotation and an R value which would be the angle to rotate. Most of the time i have seen X0 Y0 used for the center of rotation. Your R will have to be calculated using the positions of the reference holes.

Click to expand...

I added G68 X0 Y0 R45 to a short program prior to the first tool call to see what would happen and I got the error "P37 Prog No Zero". The Mitsubishi manual doesn't really explain what that means, but I'm going to try tomorrow with a G68 after the WCS call and see where it goes. It's a shot in the dark.

The alternative isn't terrible, but it's not ideal. I can create a WCS in CAM that references the real-world offset, and just program it like that. It'll work but it's a lot of back and forth from the office to the machine.

Veteran Bicycle said:

I added G68 X0 Y0 R45 to a short program prior to the first tool call to see what would happen and I got the error "P37 Prog No Zero". The Mitsubishi manual doesn't really explain what that means, but I'm going to try tomorrow with a G68 after the WCS call and see where it goes. It's a shot in the dark.

The alternative isn't terrible, but it's not ideal. I can create a WCS in CAM that references the real-world offset, and just program it like that. It'll work but it's a lot of back and forth from the office to the machine.

Click to expand...

This is embarrassing...

I typed XO YO instead of X0 Y0. Duh.

Okay, so I loaded this program, which is chamfering of a real part - just safely above the part, just to check out the G68 command.

O205108 (45 TEST)
(T37 D=6.35 CR=0. TAPER=45DEG - ZMIN=79.75 - CHAMFER MILL)
N10 G90 G94 G17
N15 G21
N20 G28 G91 Z0.
N25 G90
(2D CONTOUR6)
N30 M09
N35 T37 M06
N40 S3000 M03
N45 G59
N47 G68 X00 Y00 R-45.000
N60 G00 X-24.635 Y26.905
N65 G43 Z99.75 H37
N70 G00 Z84.75
N75 G01 Z81.75 F360.
N80 Z80.385
N85 G19 G02 Y26.27 Z79.75 J-0.635
N90 G01 Y25.635
N95 G17 G03 X-24. Y25. I0.635
N100 G01 X284.774
N105 X285.774 Y24.
N110 X285.775 Y-204.
N115 X284.774 Y-205.
N120 X-24. Y-205.001
N125 X-25. Y-204.
N130 Y24.
N135 X-24. Y25.
N140 G03 Y25.898 I-0.449 J0.449
N145 G01 X-24.45 Y26.347
N150 X-24.52 Y26.418 Z79.758
N155 X-24.588 Y26.486 Z79.781
N160 X-24.653 Y26.551 Z79.819
N165 X-24.713 Y26.611 Z79.871
N170 X-24.767 Y26.665 Z79.936
N175 X-24.813 Y26.711 Z80.012
N180 X-24.85 Y26.747 Z80.097
N185 X-24.877 Y26.774 Z80.189
N190 X-24.893 Y26.791 Z80.286
N195 X-24.899 Y26.796 Z80.385
N200 G00 Z99.75
N210 M09
N212 G69
N215 G53 Z0.
N220 G53 X500. Y0.
N225 M30
%

It errored out P11 plane chg (CR), because a G17, G18 or G19 cannot be called when G68 is active. Does that mean I should put the rotation above the tool calls and use the G59 absolute position as the center of rotation, OR SOME OTHER THING?

Calling planes may be a phenomenon of HSM 2D Contour toolpaths when chamfering, so I'll try something else that doesn't call any planes.

SUCCESS

HSM calls planes when leading in and out, so I'll have to modify this behavior. G17-G19 cannot be called when G68 is active.

Veteran Bicycle said:

SUCCESS

HSM calls planes when leading in and out, so I'll have to modify this behavior. G17-G19 cannot be called when G68 is active.

Click to expand...

Yeah, don't bother with those vertical arc lead in-out moves. Pointless most of the time.