New compound rotary programming question

[wdg5555]

My shop is buying a new okuma mill with a compound rotary on it. I've programmed a mill/turn machine with a positional B axis (the tool turret rotated). My question when programming for this compound rotary is do I have to use a different work offset at the machine for each B angle.

 

In other words. I set a x,y,z zero at the machine when the part is at 0 degrees. Then i want to rotate the part on its side to 90 degrees. Is my only option to create a new x and z zero at the machine or is there some way in mastercam to account for this? I'm guessing you would have to know the distance from the pivot point to your z zero?

 

I don't have the multi axis or the 5 axis addon at this time. Not sure if i need them.

 

Thanks for the help.

[HateWhatOwnsYou]

our 5axis has "kinematics" and as far as i know all 5axis machines have some form of the same system. basically it maps the center point of rotation for all axii so they move on center and the machine compensates accordingly to where your work offset is.

 

 

in mastercam you just create a new plane so the part is oriented the way you want it(make sure x,y and z arrows are facing the right way) and select that WCS in your toolpath for "tool plane and construction plane", you will leave WCS as TOP.

setup the part us as you have it in your "TOP"  plane and the machine will rotate it to the TP and CP orientation.

you DO NOT need 5 axis addon to do positioning work like this.

[gcode]

We do a lot of work like this.

All 3+2 work.

You don't need a multiaxis license to do it, but you will need a 5X post

If I'm doing standard angles like B0 and B90, I'll usually use a separate work offset  for B0 and B90

and let the operator handle it

For odd angles you'll either have to account for the pivot distance

or if you're lucky, the machine's control has a tilted workplane option

[wdg5555]

our 5axis has "kinematics" and as far as i know all 5axis machines have some form of the same system. basically it maps the center point of rotation for all axii so they move on center and the machine compensates accordingly to where your work offset is.

 

 

in mastercam you just create a new plane so the part is oriented the way you want it(make sure x,y and z arrows are facing the right way) and select that WCS in your toolpath for "tool plane and construction plane", you will leave WCS as TOP.

setup the part us as you have it in your "TOP"  plane and the machine will rotate it to the TP and CP orientation.

you DO NOT need 5 axis addon to do positioning work like this.

Thanks for the info. I'm not sure if this will have kinematics though since its a 3 axis machine with a compound rotary on it.

[gcode]

Thanks for the info. I'm not sure if this will have kinematics though since its a 3 axis machine with a compound rotary on it.

A 5 axis post will handle this.

The mpgen post that ships with Mastercam can handle this easily, though if it's

you first experience with 5X, it would be good to pay a professional to do the post.

[jlw™]

Does the control support G68.2? If so your life can be real easy as far as 3+2. If not, I suggest using G54.4.

[wdg5555]

A 5 axis post will handle this.

The mpgen post that ships with Mastercam can handle this easily, though if it's

you first experience with 5X, it would be good to pay a professional to do the post.

I did a search for "mpgen" in my shared mastercam folder and didn't find anything. Is that short for something?

 

And doing this through a post seems like a bit of a pain, but maybe its the only way? Doing it this way I think I would have to set the machine x,y, and z zero at the center of the axis of rotation for the two axis on the rotary. Then I would have to put my 3d solid in mastercam at the distance above those axes where it physically rests on the machine. Then all of the positional moves would be correct. Am I missing something or is this the only way to avoid having multiple work offsets at the machine?

[gcode]

I just noticed this is an Okuma

the 5X posts that ship with Mastercam are fanuc posts.

I would advice you seek professional help withthis

what in the model and control of your machine??

 

You can experiment with this one

"C:\Users\Public\Documents\shared Mcam2017\CNC_MACHINES\MILL 5 - AXIS TABLE - TABLE HORIZONTAL.MCAM-MMD"

but the code will not be correct for your machine.

 

Our Okuma 5X HMC uses a macro (CALL 1088) for 3+2 work

[Greg Williams]

Okuma's use CALL OO88 for TWP (G68.2) and G169 for TCP (G43.4) in table coordinates, you will need a custom post or you can use the generic 5 axis post if you have time and knowlegde of post editing

[wdg5555]

Okuma's use CALL OO88 for TWP (G68.2) and G169 for TCP (G43.4) in table coordinates, you will need a custom post or you can use the generic 5 axis post if you have time and knowlegde of post editing

Thanks for the info. Its usually cheaper for me to edit the post than to buy one so I'll give it a try. Never done any editing to a 5 axis post so not sure how it will go. I think I understand okuma's wcs shift and rotation commands to be able to do it. Wish me luck!

[jlw™]

For the cost of a bought post you're stepping over dollars to pick up pennies.

[wdg5555]

For the cost of a bought post you're stepping over dollars to pick up pennies.

Maybe that is true for this case. Not sure how much of a challenge it will be. But the last time I got a quote for a post it was $3k (If i remember correctly). And it took me 10 hours to get the post where I wanted it (was for a twin turret lathe). And at a $75 shop rate thats $2200 saved. Also my limited experience with sending posts out to get fixed have not gone well and I've never seen a brand new post without things that need to be fixed. Which is why I learned to edit posts. Plus if I do it myself I can set it up however I want and can fix any issues on the spot. And I'm guessing if I buy a post its going to be encrypted and that sucks. Granted, the last post I was working with I could bypass most of the stuff that was encrypted but it was still a bummer.

[Guest]

I do almost all of my own posts....add some pretty neat functionality sometimes too...

 

There are just somethings that I leave to the professionals

[Brad Lisle]

for the Genos M560-V with a 4 or 5 axis rotary CALL OO88 (TWP) and G169 (TCP) are not standard. Unless you purchased those options you will need to know the physical location for center of rotation and move models accordingly. The main question I would ask, are you doing positional 3+2 only or will you be using full 5 axis contouring? A majority of companies that purchase a trunnion table to sit on a 3 axis VMC typically only ever use 3+2 positional moves with maybe the occasional full 5 axis contour. It makes it difficult for them to justify the expense for additional options and usually are not informed enough to make the decision on how important these options are to fully utilize the potential of what they purchased. It's like buying a Sandvik Hydro-grip holder just to put a HSS jobber drill in it. Depending on what your shops actual needs out of the rotary unit will help determine what options, if any you will need to get by. I know there are a few macros out there that can do the same as the CALL OO88 (TWP) if you look hard enough or ask nicely.

[Mjölnir]

 

 And at a $75 shop rate thats $2200 saved. 

 

double your shop rate to calculate your savings. the time you were working on the post was time you were not doing something productive. and certainly there's debugging to do also, which chews into productivity, therefore any savings as well. 

[wdg5555]

for the Genos M560-V with a 4 or 5 axis rotary CALL OO88 (TWP) and G169 (TCP) are not standard. Unless you purchased those options you will need to know the physical location for center of rotation and move models accordingly. The main question I would ask, are you doing positional 3+2 only or will you be using full 5 axis contouring? A majority of companies that purchase a trunnion table to sit on a 3 axis VMC typically only ever use 3+2 positional moves with maybe the occasional full 5 axis contour. It makes it difficult for them to justify the expense for additional options and usually are not informed enough to make the decision on how important these options are to fully utilize the potential of what they purchased. It's like buying a Sandvik Hydro-grip holder just to put a HSS jobber drill in it. Depending on what your shops actual needs out of the rotary unit will help determine what options, if any you will need to get by. I know there are a few macros out there that can do the same as the CALL OO88 (TWP) if you look hard enough or ask nicely.

Mainly will be doing positional work. The salesman from hartwig did tell us that we would be able to do full 5 axis cuts if we wanted to. Don't have the machine here yet so I can't answer the question about macros so I might be asking about them when the machine comes.

 

 

double your shop rate to calculate your savings. the time you were working on the post was time you were not doing something productive. and certainly there's debugging to do also, which chews into productivity, therefore any savings as well. 

 

I like post editing

And before I got to my current shop people were doing a lot of hand edits just like the last shop before I edited the posts. Machinists for whatever reason don't take the time to send out posts in my limited experience.

[Brad Lisle]

Mainly will be doing positional work. The salesman from hartwig did tell us that we would be able to do full 5 axis cuts if we wanted to. Don't have the machine here yet so I can't answer the question about macros so I might be asking about them when the machine comes.

You can do full 5 axis without the additional options. BUT, there is always a catch right, in order for Mastercam to output proper rotary feedrates. Whether it be in degrees per minute (standard for Okuma) or inverse feed (optional) it needs to know where the part is in relation to the machine rotation pivot points. You will need to program your part, setup your part to find the actual offset value, then possibly and more than likely move the model or geometry for your part, regen and post. With the other options, TCP for full 5-axis all you need to do is post the code, setup and run. The control will dynamically track the location and continuously compensate for the rotation pivot points. If you only do a few parts a year with full 5 axis it might be best to not jump for TCP. Fixture tracking however is very effective for 3+1 or 3+2 positional. Typically programmers use multiple work offsets and possibly different points of origin for different planes. This leaves the setup guy to have to find and set multiple work offsets. Sometimes they face difficulties finding an edge to set from. Using CALL OO88 (similar to TWP) you only need to set the original work offset then use the CALL OO88 cycle to move and/or rotate the planes from the original offset to a new offset. As I mentioned earlier I believe if you do some searching on this forum someone posted a macro capable of doing the same as the paid option. If you cannot find it let me know. I strongly suggest using it. You can also kindly ask the Applications Engineer, as we tend to have other custom macros we might share.

[wdg5555]

You can do full 5 axis without the additional options. BUT, there is always a catch right, in order for Mastercam to output proper rotary feedrates. Whether it be in degrees per minute (standard for Okuma) or inverse feed (optional) it needs to know where the part is in relation to the machine rotation pivot points. You will need to program your part, setup your part to find the actual offset value, then possibly and more than likely move the model or geometry for your part, regen and post. With the other options, TCP for full 5-axis all you need to do is post the code, setup and run. The control will dynamically track the location and continuously compensate for the rotation pivot points. If you only do a few parts a year with full 5 axis it might be best to not jump for TCP. Fixture tracking however is very effective for 3+1 or 3+2 positional. Typically programmers use multiple work offsets and possibly different points of origin for different planes. This leaves the setup guy to have to find and set multiple work offsets. Sometimes they face difficulties finding an edge to set from. Using CALL OO88 (similar to TWP) you only need to set the original work offset then use the CALL OO88 cycle to move and/or rotate the planes from the original offset to a new offset. As I mentioned earlier I believe if you do some searching on this forum someone posted a macro capable of doing the same as the paid option. If you cannot find it let me know. I strongly suggest using it. You can also kindly ask the Applications Engineer, as we tend to have other custom macros we might share.

Good info thank you! I stumbled upon a article on Okuma's website that lists all(?) of the options somebody might want to have on a 5 axis machine from Okuma.

 

http://www.okuma.com/essential-multi-axis-control-options

[gcode]

Good info thank you! I stumbled upon a article on Okuma's website that lists all(?) of the options somebody might want to have on a 5 axis machine from Okuma.

 

http://www.okuma.com/essential-multi-axis-control-options

I know Ron.. he came by and helped iron out some issues we had with our Okuma VTM1200

He definitely knows his stuff

[Guest]

Programming using TWP/TCP is nice because then you can have the part anywhere in space you want (say top of the stock, left upper edge), pick up your origin and go. No need to mess with having the part relative to COR. Frankly, I prefer to NOT have my origin anywhere near C-Axis because of singularity issues.

 

JM2CFWIW YMMV

[Brad Lisle]

Here is the one I was speaking about that I found on here

 

http://www.emastercam.com/board/topic/65330-okuma-horizontal-offset-rotation-macro/?hl=okuma#entry1062179

 

I noticed this is for a horizontal though. I will have to keep digging for a 5-axis one if there is one available on here.

[Mick]

Programming using TWP/TCP is nice because then you can have the part anywhere in space you want (say top of the stock, left upper edge), pick up your origin and go. No need to mess with having the part relative to COR. Frankly, I prefer to NOT have my origin anywhere near C-Axis because of singularity issues.

 

JM2CFWIW YMMV

 

And a hot tip. If you programme the part assuming it is located approximately in the centre of the table, but it ends up being actually set up off centre, be sure to run your simulation software (if you have the luxury of that) with the part positioned as per the actual setup on the machine. Travel limits, and collision potential, changes depending on workpiece placement.

 

I know Ron.. he came by and helped iron out some issues we had with our Okuma VTM1200

He definitely knows his stuff

 

Ron trained me on the Okuma MU500V-II at the Thinc facility in Charlotte. That was some of the best training I have ever had. In that one trip, I configured the post, and the Vericut machine model, and learnt how to operate the machine. They're a great team there, that's for sure. Ron sure knows his stuff, and he is a great guy.

[wdg5555]

And a hot tip. If you programme the part assuming it is located approximately in the centre of the table, but it ends up being actually set up off centre, be sure to run your simulation software (if you have the luxury of that) with the part positioned as per the actual setup on the machine. Travel limits, and collision potential, changes depending on workpiece placement.

 

Programming using TWP/TCP is nice because then you can have the part anywhere in space you want

 

I was thinking about this and I a bit confused. 1st, I'm not sure how you would program it in mastercam. Lets say the X,Y, and Z zero is set to the corner of the part. Is that where your WCS is in Mastercam? Seems like your rotations would be off by alot that way.

 

Then once at the machine do you have to turn TCP on and off or is it always on.

 

I'm just not seeing exactly how TCP would work.

[Brad Lisle]

you would need to turn it on in the program

[Guest]

Lets say the X,Y, and Z zero is set to the corner of the part. Is that where your WCS is in Mastercam?

Yes. You would keep the same origin point (so long as you're planning on using the same work offset.

 

 

Then once at the machine do you have to turn TCP on and off or is it always on.

 

I'm just not seeing exactly how TCP would work.

TCP is G43.4 and would be activated in place of G43. It gets turned on and cancelled the same way (G49)