LIVE TOOLING LATHE CONTROL DEFINITION

[skymont]

HELP,

I'M HAVING TROUBLE MILING 3D SHAPES IN MY LATHE. I'M WONDERING WHAT I CAN CHANGE IN MY LINEAR SETTINGS IN THE MILL. IF IT WILL FIX MY PROBLEM OR IT COULD BE A POST PROBLEM. I'VE ATTACHED A SCREEN SHOT OF WHAT CONTROL TOPICS I'M TALIKING ABOUT.

THANKS

[Guest]

You might want to let us know what kind of problem.....the answer may or may not live there...but without knowing what's happening, it's tough to guess

[skymont]

I'm using 2018 and using a surface rough. My Back Plot and Verify shows what I want it to. When I run in the lathe (OKUMA LB4000) it does moves that the Back Plot and Verify doesn't. The lathe mills off some of the part that it is not suppose to touch. I have attached 3 pics to maybe explain more. The last picture is what the lathe did.

Thanks

[crazy^millman]

Yes your clocking is off. Has the post been tested before now and run other parts with no issue?

I look at it more and then I am not sure. Do you have a file you can share? Have you called your dealer to see what their take on it is?

[skymont]

No the post has not been tested on milling. Seems to do simple face contour and face drill but this is now a 1st doing 3D milling. I have tried 2 different roughing tool paths and both do the same(surface rough,area rough). I have told the dealer and give them every file i know program, code and even these pictures. I have not go anything from them. I think there needs to be a Z axis re-track to clearance move before the lathe does a re-clock. Maybe? 

What file do you need and i can try to send it?

Thanks

[crazy^millman]

a .z2g is the best an include the post and we can see a much as anyone can see. I am thinking it will come down to just dialing in the post. Once that is done you should be good to go.

[huskermcdoogle]

Looks to me like the machine isn't air cutting in the right direction when the tool stays down.  If this is optirough, set to retract to safe height always and see if it clears up the issue. 

If so, basically it is a post issue where you will need to break up angular motion to force direction.

[Colin Gilchrist]

It looks like instead of your "retracts" rotating the "long way around", the machine is taking the "shortest path" on the rotary, and milling off the back side of the part. I'd change up the tool path, to either "retract" along the Z axis, before the re-position move to start the next cut, or increase the "lead in/out" so that the tool won't cut off the "back side" of the part...

[skymont]

i have done a old surface rough pocket tool path and i have also done a surface high speed (area rough) tool path used full retract 50mm above my Z zero. both tool paths showed same results. i believe it is a post problem . today i'm about to try 3 tool offsets (ex. T020202) to see if it may change. my post right now just puts out 2 offsets. i've read before some people using 3 but idk. i will also change my C rotary and see where it gets me. i will do all of this one setting at a time.

thanks,

[crazy^millman]

Pay close attention to the moves as you are going through the program. When you see a C Axis move pay attention its going like you would expect it to and not the opposite direction. I was not thinking about that until Husker and Colin mentioned it and then it reminded me I have seen the same thing on Okuma. There is a shortest distance command code for them and if the M15 M16 or M13 M14 depending on the control for CW and CCW direction are not coming out correct you will see the issues you are seeing.

[skymont]

Okay i used the 3 tool offset on the program and it still cut my back side of part. Yes it is throwing out M15 and M16 in to code, but i think it like might need more to keep from cutting back side or it needs to retract in z to allow re-clock. I have not tried to use a big lead in-out yet i will try this next. 

Colin do you know where i can find this retract along z axis? 

[nickbe10]

Machine parameter? Breaking (or not) rotary motion?

[huskermcdoogle]

5 hours ago, skymont said:

Colin do you know where i can find this retract along z axis? 

Which toolpath are you using?  Can you post a file?

[skymont]

Surface High Speed (Area Roughing).  I can post a file if I can.

Thanks

[crazy^millman]

Here is a link to his file:

His Link:

[Alex Dales]

What is the Rotary axis type on the machine?

The Machine def has the C set to Signed Direction and is using M15 and M16 to indicate the direction.

What happens if you MDI 5 degrees? 355 degrees? Does the M15 and M16 influence the direction it rotates to find that position?

 

If the M15 and M16 are working correctly in the machine, then Colin was right, your machine is going the long way around.

X92.603 C311.383 M15 F633.28
X88.828 C311.858 F687.47
....
X97.368 C356.708 F4510.42
X97.265 C357.988 F4502.71
X97.107 C.133 M16 F4519.87 <<<<<The c-axis direction is changing instead of crossing zero with a M15 and is taking the long way around.
X96.964 C2.283 M15
X96.838 C4.436 F4528.18
X96.727 C6.592 F4534.86
X96.632 C8.751 F4539.83
 

[crazy^millman]

10 minutes ago, Alex Dales said:

What is the Rotary axis type on the machine?

The Machine def has the C set to Signed Direction and is using M15 and M16 to indicate the direction.

What happens if you MDI 5 degrees? 355 degrees? Does the M15 and M16 influence the direction it rotates to find that position?

 

If the M15 and M16 are working correctly in the machine, then Colin was right, your machine is going the long way around.

X92.603 C311.383 M15 F633.28
X88.828 C311.858 F687.47
....
X97.368 C356.708 F4510.42
X97.265 C357.988 F4502.71
X97.107 C.133 M16 F4519.87 <<<<<The c-axis direction is changing instead of crossing zero with a M15 and taking the long was around.
X96.964 C2.283 M15
X96.838 C4.436 F4528.18
X96.727 C6.592 F4534.86
X96.632 C8.751 F4539.83
 

Yes we have seen this many times and comes from the NCI out of Mastercam sending bad information. Hard to have a post builder fix bad stuff they are getting from the NCI.

[Alex Dales]

1 minute ago, C^Millman said:

Yes we have seen this many times and comes from the NCI out of Mastercam sending bad information. Hard to have a post builder fix bad stuff they are getting from the NCI.

Looks like the post logic isn't tracking when it crosses zero correctly. Even though it is outputting C.133 the post should be adding a revolution and tracking an absolute angle of 360.133. this will keep the direction the same and the incremental move at 2 degrees instead of 358.

I just ran this operation through one of our posts and you can see the direction does not change when crossing zero.

(This post is set up to use the Sign on the Angle instead of a modal M code to indicate the direction, so instead of M16 we have negative C values, and Positive C values for M15)

X96.462 C-310.936 F55.6
X92.603 C311.383 F627.4
X88.828 C311.858 F681.3
...
X97.368 C356.708
X97.265 C357.988
X97.107 C.133
X96.964 C2.283
X96.838 C4.436
X96.727 C6.592
X96.632 C8.751

 

We didn't provide this post, so I can't change the encrypted logic for you. Contact your post provider and they should be able to get this sorted out for you.

[huskermcdoogle]

 

8 hours ago, skymont said:

Colin do you know where i can find this retract along z axis? 

 

Look for full vertical retract in the top right dropdown in linking parameters section of the path parameters, then in cut parameters change the value for keep tool down within to a small number, this combo should force retracts.

[Rocketmachinist]

Does this machine have a milling mode like the Haas? I have found that giving the control the power to use X's and Y's works so much better than using X's and C's. Plus the code is way smaller.

[Alex Dales]

14 hours ago, huskermcdoogle said:

 

 

Look for full vertical retract in the top right dropdown in linking parameters section of the path parameters, then in cut parameters change the value for keep tool down within to a small number, this combo should force retracts.

A full Z retract will not fix this. the error is occurring when the machine crosses over the zero degree position while cutting. Using interpolation like below should get the part running.

 

14 hours ago, Rocketmachinist said:

Does this machine have a milling mode like the Haas? I have found that giving the control the power to use X's and Y's works so much better than using X's and C's. Plus the code is way smaller.

Misc Int #9 is set for face interpolation this will convert it to X and Y. thsi will avoid the issue and get this part running.

[Guest]

This looks to be a Postability post....

I wonder why the OP didn't just go back to Dave on this one?

[crazy^millman]

1 hour ago, JParis said:

This looks to be a Postability post....

I wonder why the OP didn't just go back to Dave on this one?

It is a Postability Post and I have talked to him and he has not had good results with his reseller. I will forward to Postability and see if they can assist him through 5th Axis.

[gcode]

I'm thinking this needs an M460 (C axis shortest distance) callout

We had a lot of trouble with tool paths like this on our Okuma VTM

M460 at appropriate places solved a lot of those issues

[skymont]

It is a post problem. I was just making sure I wasn't doing anything wrong in the control definition or my programming before went any further and if anyone had any ideas about fixing this.

Thanks everyone for the help, maybe by end of week this will be fixed.