[shags72]

Ok I have an Okuma ma600 H and an HB. I know on some controls if you make a Z move with G41 on then the machine can do funny sometimes disastrous things. What I need to know is if the OSP200 can deal with it. Thanks everyone.

[Superman]

As far as I'm aware

Cutter comp is only applied/active to the axes defined in the machining plane G17(XY), G18(XZ), G19(YZ)
- the 3rd axis has no comp applied, as it would assume to be the "depth" component ( ie Z for G17, Y for G18, X for G19 )

No compensation is applied to any rotary axis

I think there is a 3D compensation option ( I think G43 ) for use, only with a ball-nose, but then CAM comes into use, & tool-length offsets set to the ball centre
- but don't quote me on this

[shags72]

So if youj rapid in Z from a comped x,y position what will it do? I have seen that it may move in an inconsistent way on the Z move. And not the same way EVERY time. I just won't make a rapid Z lone move while milling. I was taught to always cancel on a retract x,y move and then move the z/

[Algirdas]

read the manual, it's explained very clearly. It is simple.
I have seen crazy movement right after compensation off (G40) on non-japanese machines only. Okuma does canceling of compensation exactly according description

[broby]

We have a MA600HB and an older MC600HB and have NEVER seen any movement of the likes that you describe.
As Superman points out G41 only applies to the active plane G17/18/19.
I would suggest that there OBVIOUSLY some other reason for the problem you have described.
I have programmed thousands of times a compensated program along with changes in Z axis and have never seen anything untoward happen with the Z axis movement.
Regards
Brian.

[shags72]

No real experience with this machine so just a bit leery with moves I never use. This is a program someone else wrote and just thought it weird to rapid to center of the slot at clearance Z level, engage CC to one side of slot off the part, then drop to Z depth and engage the cut. But if it works, I am ok with it.
I saw on a fanuc a threadmill op that didn't shut off CC to the center of the hole and Z out to go to next hole, run 4 holes fine and then on the 5th hole when it came out it took the cutter out as it comped to one side as it brought the cutter out. Same code on every hole. Strange things indeed. Was told that the control doesn't know where to go as there is no right or left side of the line on a Z move. Ah we'll.

[Superman]

So if youj rapid in Z from a comped x,y position what will it do? I have seen that it may move in an inconsistent way on the Z move. And not the same way EVERY time. I just won't make a rapid Z lone move while milling. I was taught to always cancel on a retract x,y move and then move the z/

I don't think it is wise to do any rapid positioning movements with comp active.
- rapids can create a "dog leg" path on any move with more than 1 axis.
Best practice is to
- rapid to XY position
- rapid to Z
- feed to depth
- comp to start point ( comp must be taken up on a line )
- do contour
- lead off the contour
- cancel comp while doing line to safe point
- rapid retract


But a rapid Z move, with G17 active, & G41/G42 comp active ...will not make any other axis move, but go directly to the stated Z position

run 4 holes fine and then on the 5th hole when it came out it took the cutter out as it comped to one side as it brought the cutter out. Same code on every hole

I would guess that G40 was use on a line by itself. Comp was not removed so on the retract, the tool also moved in X & Y ( It is strange, I'd say parameters would need looking at )