Turncut Problems On Okuma MA-500HB

[CHeimbach]

Hello everyone, I am somewhat new to Mastercam (2019) and i am having issue trying to turn cut.  When i do my chain, it tells me "the contour does not lie in the construction plane".

Not sure what is going on because i have tried changing my cplane, and still doesn't seem to want to work. What am i doing wrong?

[crazy^millman]

What type of path are you trying to use? What is the machine and control definition for the machine you are programming this for? Do you have a Sample file you can share? Have you reached out to your Mastercam dealer?  

[CHeimbach]

The machine is an Okuma MA-500HB 3 Axis CNC Horizontal Machining Center.   Mill/Turn. 

Does this help at all? I guess i should clarify, i am totally new to Mill programming on Mastercam. 

[crazy^millman]

Okay your lathe plane for that feature has to be where you are going to be turning it. This is something that experienced programmers struggle with that I teach on how to go about the process. The Lathe plane needs to be establish on the front face of the feature and Zero should be the center of that bore you are going to be turning. Then you setup your Workoffset to that feature and done. You try to use a base WCS and go about it and you going to have a nightmare understanding the code and sorting it out.  normally teach to setup your plane for the turning then make your Lathe Group. Make sure the Stock Plane is the same plane. Once you define that and understand how to sort out that relationship you should be good to go. You can use the create WCS by geometry and pick the face. That will not become a new WCS. Then make a relative plane to that in front and that should be the plane you need to do the turning.

Then you define your turning planes with correct turning tool and the post should do the rest of the work for you. I setup a Aerospace Company up wit ha process to define their tools based off the type of tool. 101-110 Was OD and OD FACE Turning Tools, 111-120 ID and ID Face Turning Tools, 121-130 Was OD Back Turing and Facing and 131-140 was ID Back Turing and facing. That allowed them to go about setting up a standard process for some tools to help with the Verification implementation I also had some help with. I strongly suggest some training with your dealer or get a contract programmer in your area to work with you to help.

[CHeimbach]

That look complicated lol. I will do that and see how it works. Thank you for your help. 

[JoshC]

your stock plane is set to front in the stock setup page. Typically when you see the "the contour does not lie in the construction plane" it means the plane that you are using in stock setup is not perpendicular to the plane the geometry you are selecting is on. If you cant post a part file and want some guesses i would guess you should try Top plane since that is 90 degrees off of the Front plane you currently have set in stock setup. Also make sure to go to edit tool and make sure the turret is set to the correct turret, upper or lower turret in tool setup is important based on where the geometry is located.

[Tim Johnson]

12 hours ago, CHeimbach said:

The machine is an Okuma MA-500HB 3 Axis CNC Horizontal Machining Center.   Mill/Turn. 

Does this help at all? I guess i should clarify, i am totally new to Mill programming on Mastercam.

  Unless Okuma has radically changed a machine that they don't manufacture (other than the electronics) this machine is not a mill/turn machine and you need  to use the milling side of Mastercam.

[Chris In-House Solutions]

Quote

Unless Okuma has radically changed a machine that they don't manufacture (other than the electronics) this machine is not a mill/turn machine and you need  to use the milling side of Mastercam.

I believe the video below shows the Turn-Cut feature Okuma has.  Its similar to a d'andrea head.  

@CHeimbach maybe reach out to the company that provided the post and ask them for a sample part file so you can see how it should be programmed.  Everyone above has pointed you in the right direction in terms of setting up your planes properly.  

 

[Tim Johnson]

43 minutes ago, Chris In-House Solutions said:

I believe the video below shows the Turn-Cut feature Okuma has.  Its similar to a d'andrea head.  

@CHeimbach maybe reach out to the company that provided the post and ask them for a sample part file so you can see how it should be programmed.  Everyone above has pointed you in the right direction in terms of setting up your planes properly.  

 

Nice. I could use that. So you would program the turn-cut with MC mill-turn?

[Chris In-House Solutions]

@Tim Johnson We've setup a couple of these posts in the past and its been a while so I may not be correct but I believe the posts were setup with 2 machine defs a mill one and a lathe one.  You would do most of your programming within Mill and then then when you need to use this option you would load a lathe machine def in and program your toolpath within Lathe.

I also believe this is an option and you may have to order at the time of purchasing the machine.  But you might be able to get it added on after the fact.  You would have to check with Okuma.  

Mazak has something similar called Mazak Orbiturn but I'm not sure how that cycle works and am pretty sure again this is an option on the Machine.  

[crazy^millman]

Chris you are correct that is what I have done for one of your customers and I found it best like I suggested to make the Zero a new Workoffset in the machine where you want to do the turning and then match that plane in Mastercam using the lathe definition and call it a day. 

GROB was doing this for a 10" bore on a 5 Axis machine you couldn't watch it run it made anyone who tried sea sick. They were holding a .002 profile tolerance, but being 5 years later I wonder how well it is holding up after all this time.