Rotary Machining with Vertical Rotary - How

[Rotary Ninja]

We have a lathe part we have to cut a profile on with our rotary. The part is too big to just clamp to the table and machine. So the rotary will allow us to rotate the part to machine the surfaces. We were thinking that we could just position and machine the surface in quadrants. But I want to use the rotary to just surface the part all the way around. So I would like the tool to stay at -Y- 0, and machine with -X- -Z- and technically -C-. I have never had to do this before. Do I have to create a new machine definition to make this work? Ours has the rotary sitting horizontal along -X- axis (-A- axis rotary).

 

I am attaching a model I created to represent the part. The area that needs to be machined is the 1.500" rad and the ID angled wall.

 

Thanks.

Rotarty Vertical.mcx-8

[Matthew Hajicek - Singularity]

That could be tricky.  Maybe a lathe C-Axis path with the axis labels changed?

[Rotary Ninja]

Our reseller is sending me a 3+1 Machine def and post that he says will work for me.

[Rotary Ninja]

The only problem I am having is I now can't control the start point for the toolpath. I am using flowline. It wants to place the tool on the right side of the part and I need it to be on the left at Y0. I have tried a Transform rotate without much luck.

[Machineguy]

Use the flowline parameters in the tool path window. Its at the bottom after you pick the geometry.

[Rotary Ninja]

All that does is flips the direction of the arrows. The tool is still cutting on the X positive side. I even tried rotating the part 180.

[Rotary Ninja]

I just moved my X 0 location in my machine definition and that appears to have worked. It still backplots on the right side (X positive). But all the coordinates are X negative.

[Colin Gilchrist]

The big issue you'll run into with this is the way that the Generic Fanuc 4X Mill Post is setup to process rotary motion. This post is explicitly setup to operate a VMC machine, with a Rotary that is either A on X, or B on Y. Sure, you can change the address labels, and the direction of rotary motion, but the post wasn't designed to process calculations for a Vertical Tool, with a C-Axis rotary.

 

You could probably go through the process of converting a Router post to Mill, (Generic Fanuc 4X Router), but where is the fun in that?

 

I modified the Generic Fanuc 4X Mill Post to support this output, using the "Polar' output method. ("3 Axis" in the rotary selection dialog). I had to modify the Feed calculations, since the values are designed to be calculated with the Z axis position. (I switched it to xabs, instead of zabs, for the 'circum' calculation).

 

For the output to work, I had to comment out 'linarc$' inside 'pxyzcout2', so that it wouldn't linearize the arcs, and then I copied 'pcirout', and make a 2nd 'pcirout' that would get called when "Polar" was active. Then I just suppressed the 'G2/G3' values, which gives you the ZX steps to reposition the tool, and then the "arc" output is just done as a C-Axis move (with Degrees per Minute feed output). So you'll see the post spit out a normal IPM feedrate for the step motion, but a DPM feedrate for the rotary.

 

In order to get this to work, you might try messing with the "break arcs" settings in the CD. I didn't try messing with them yet, and I was getting arcs that were broken at the quadrants. So I would get XZ to position the tool, then C90., C180., C270., C360. as output after the position move. I think with "don't break arcs" set, and "Allow 360 degree arc output" turned on, it might be possible to get it to spit out a single rotary move that rotates 360.

 

EDIT: Ok, I tried to attach my example Z2G file, but it appears I have "exceeded my allotted disk space" for uploads. That sucks. PM me your email address and I'll send you a Z2G example file with the toolpath and the modified post.

 

By the way, when I tried Flowline on your Solid Faces (radius and angled wall), it wouldn't keep the start point for each face lined up. So it would start at X+ on the radius, but then have a rapid move across the center of the part when it reached the "Gap" between the faces. I ended up creating two surfaces, and then rotating the top surface 180 degrees only to get the flowline start positions the same for both surfaces. It was also critical to give the toolpath enough Arc Filter tolerance to be able to spit out clean arcs for the cut motion.

[Matthew Hajicek - Singularity]

Showoff. 

[Colin Gilchrist]

To be fair, it did take me about 30 minutes to find the solution, including debugging the post output, and making the modifications...

 

And... this is a total hack to suit a particular purpose. Converting a Router post to run in Mill probably wouldn't be a good solution either, since the Router post is generally designed to function with the rotary "C" axis mounted to the head of the machine.

 

Hey Kevin, was that what you needed?

[Rotary Ninja]

I got pulled off and stuck on 6 other jobs LOL. I will post the results as soon as I get back to it.

 

Thanks!

[Rotary Ninja]

Colin asked me to post his zip2go file so you guys could see what he did. This works much better than what I came up with.

ROTARY-C_COLIN.Z2G

[Rotary Ninja]

With Colin's Machine/Control Definition and post it wants to put -X- on the positive side of the part. We need it on the left. I tried flipping the axis zero position like I did on our Haas definitions but it is not making a difference. Any ideas? 

[Colin Gilchrist]

Try rotating the surfaces 180 degrees. That should do it...

[Newbeeee™]

To be fair, it did take me about 30 minutes to find the solution, including debugging the post output, and making the modifications...

 

Double showoff!

A whole half hour...