sined rotary table

[JER0619]

Hello all,

As per the title I have a ring on a rotary table signed at 40 degrees about the y-axis on a 4-axis mill.  I want to locate the tool at X- and Y0 and rotate the table to mill the tab features on the ID of the part.  I have struggled for a couple of days trying to get anything that I can work with.  Currently I am trying a 4-axis swarf toolpath but am unsuccessful in getting the part to rotate.  Upon scrubbing forums I believe that I need to make edits to the post file to "turn on" and define the rotary table because the post uses minimal info from the machine definition.  Can anyone confirm this and better yet tell me what  need to be changed in the machine definition and post for the particular setup?

Thanks in advance,

Jer

 

 

[Guest]

Actually need a 5 axis post to output properly

 

[JER0619]

I am using the generic 5 axis post but using the 4 axis option in the toolpath. 

[nickbe10]

Using the 4th axis option , I believe, locks one axis and stops it giving rotational output and assumes 0 degrees rotation on the locked axis. You have rotational output, it is just fixed in one axis. Unless you can generate the fixed 40 degrees on the locked axis, you will need 5 axis toolpath. Not familiar with the new Moduleworks options, I saw a screen shot on here not long ago and it seemed to have a lot of options so maybe there is something in Moduleworks, but I don't think this would work with legacy multiaxis with one axis locked.

[crazy^millman]

43 minutes ago, JER0619 said:

I am using the generic 5 axis post but using the 4 axis option in the toolpath. 

Have you configured it for your process? I would make the hole my Zero make a plane for that operation and then make toolpaths for one tooth. Then just output the indexes needed and call it a day. Unless you are extremely good with Mastercam posts not something easily done with getting a 3rd Party Post or being very good at editing Mastercam posts.

[nickbe10]

19 minutes ago, C^Millman said:

Have you configured it for your process? I would make the hole my Zero make a plane for that operation and then make toolpaths for one tooth. Then just output the indexes needed and call it a day.

Correct me if I'm wrong here Ron, buy I think because he has created an unaccounted for (as far as Mastercam is concerned) compound angle  he will have to compensate for this on his rotation angles (indexes)....?

[Ewood42]

If the wall on those tabs are parallel to Z axis, and this is a one-off type job...Wouldn't it be easier to just program that one contour, post, then hand edit to make it a sub program call? (Wash-rinse-repeat) Just be sure it retracts enough before rotating.

[crazy^millman]

30 minutes ago, nickbe10 said:

Correct me if I'm wrong here Ron, buy I think because he has created an unaccounted for (as far as Mastercam is concerned) compound angle  he will have to compensate for this on his rotation angles (indexes)....?

No if Mastercam is not setup to understand the layout correctly then it may look good in the backplot, but not produce the desired code on the machine. Really comes down to where you establish zero from and what does the post have to do to give the correct output. I use to make rings like this 20 years ago using a Bridgeport. I had jaws to hold the ring with the ID radius cut in them of the ring. I then kicked the head over and milling what I needed at each angle. Each index was marked and was close enough for the purpose it served. I would simply this doing what I needed and then just do like Ewood said and call the indexes and have a good day.

[nickbe10]

17 minutes ago, C^Millman said:

I had jaws to hold the ring with the ID radius cut in them of the ring. I then kicked the head over and milling what I needed at each angle.

So your angular rotations were as per the drawing in the top view of the part. But he will not be rotating in this view.

 

19 minutes ago, C^Millman said:

Really comes down to where you establish zero from and what does the post have to do to give the correct output.

So this is what is important here. But how do you know you are getting the correct angular output. Of course it also depends on the tolerances and the diameter of the ring. Might be worth crunching the numbers through a compound angle calculator though just to make sure you are staying within tolerance. If say the print shows 30 degree rotation of the tabs in the top view the first few rotations might be OK and then you might go out as the variation stacks up.

[JER0619]

First off thanks for all of the input guys. This is the kind of stuff I need to help me think out of the frame of mind I'm stuck in  

The issue here is that the entire ID and tabs surfaces are parallel to the z-axis at the appropriate a-axis position. The topside of the tab is wider than the bottom side of it.  If I break the features up by milling the tabs and then milling the ID I need to have the a-axis move. I actually never considered this process because of this but it's worth looking into the error in milling the tabs using Y-axis movement , index and repeat. The diameter in between is the easy part to program offline. I can easily find the a-axis position where I need to plunge into the diameter, rotate and retract.  

I will look into the error if I were to use the y-axis to form the tabs but what I really need to know to make it right is how to make the a-axis move in sync with my x-axis. I started to paw though machine definitions (with very little experience) and there you can tilt a rotary but any changes I make to the tilt angle does not produce different code. It seems to me that it should be as simple as saying the a-axis is at a 40 deg angle. Go ahead and rotate about it. 

I hope I'm not overlooking something simple here. 

 

[crazy^millman]

1 minute ago, JER0619 said:

First off thanks for all of the input guys. This is the kind of stuff I need to help me think out of the frame of mind I'm stuck in  

The issue here is that the entire ID and tabs surfaces are parallel to the z-axis at the appropriate a-axis position. The topside of the tab is wider than the bottom side of it.  If I break the features up by milling the tabs and then milling the ID I need to have the a-axis move. I actually never considered this process because of this but it's worth looking into the error in milling the tabs using Y-axis movement , index and repeat. The diameter in between is the easy part to program offline. I can easily find the a-axis position where I need to plunge into the diameter, rotate and retract.  

I will look into the error if I were to use the y-axis to form the tabs but what I really need to know to make it right is how to make the a-axis move in sync with my x-axis. I started to paw though machine definitions (with very little experience) and there you can tilt a rotary but any changes I make to the tilt angle does not produce different code. It seems to me that it should be as simple as saying the a-axis is at a 40 deg angle. Go ahead and rotate about it. 

I hope I'm not overlooking something simple here. 

 

The Machine definition for generic 5 Axis posts are not connected to the post. Where you need to go to a 3rd party group that does and you life will be much easier. I have done 5 Axis for some years and every situation presents it's own things to consider and sort out. You are thinking correctly just need to get the post to take the kinematic process into account. The generic will do this, but like I said you need to be really good with them to make sure you are taking everything into account. Best of luck and keep us posted. 

[huskermcdoogle]

I would cheat it and be done with it for now if this is a one time thing.  Draw out a straight line profile as you want your cut to be, as if it is not tipped (at right radius) and use axis sub with a standard 4 axis post.

[JER0619]

UPDATE -- Finally figured it out.  The toolpath required a custom post and machine definition.  The post takes into consideration the 40 deg sine plate.  The toolpath was generated from the top view using a projected curve path.  

After endless attempts I never found a way to get the right numbers using flat geometry with axis sub or 5-axis paths alone. 

I appreciate the input from everyone. Now I'm moving onto programming an integrex for the first time.  Tough year for my brain lately.

Thanks so much

[crazy^millman]

Excellent work and glad you got it all sorted it.