High speed 3D machining with a Fusion640 control.

I'm wondering if any of you have experience with high speed 3D toolpaths (EIA) on a Mazak Fusion 640 control?

Is it worth upgrading to the MAZACC3D package for small line segment machining?

The feature being machined is not too complicated. It's basically a tapered, angled cone with a 3.5 inch O.D., and a 2.5 inch I.D., about 2 inches deep. The accuracy is not critical, as long as the finish is consistent and gouge free.

I already do quite a bit of high speed 2D machining, using G61.1, but that seems to get pretty ugly in a 3D path with line segments of .0002-.0005.

Is there another way to increase the 3D cutting performance of a Fusion640 control? The machine is a PFH5800 with 15,000RPM.

If you're machining a cone, you don't need the Mazacc3D, you can do it with simple 2D circles. In that way, you can use G61.1. Or is the part a little more than a cone?

why can't you turn the part with custom fixture. I think it's faster like that.

Unfortunately, it's a little more than a cone, and it's compound, so even in 2D arcs, it will still be tiny line segments, and G61.1 doesn't seem to like those at all.

The inside of the cone could be machined 5 axis simultaneous, but I don't have that capability, and the part still needs a high speed 3D toolpath for the .1875 corner rounding operation around the compound curves.

This feature can't be turned on a lathe.

You can tweak G61.1 to run better in the short line segments. I wouldn't bother though, it will affect the overall performance in 2D and super high speeds.

I'd look into installing the high speed 3D option. Its really not that much.... to me anyway.

Another option is to slow down the feedrates and run. I think you'll have to shut off G61.1 though since your segments are so small and run in G64.

Buy BobCadd Pakage V20. We us it for 3D milling all the time and works Great.

Orbea is obviously not with this conversation......

Talking about machine dynamics here... not programming.....

What kind of tolerance are you seeking? We have 3-4-5 axis Mazaks here and we run 3-d contours all the time, with no problem good finish (16 or better sometimes) no gouging, and tolerances of
+\-.001to2 and thats flying. If we slow down, I can hold +\-.0003to4 We drip feed off of the card all the time. Very large programs with .0005 long line segments sometimes. I think a lot of the time its not the control with the problem its the code that was generated. We have ug nx4.and its tool paths are dead nuts.

everfabchad makes a good point on programming. I may owe Orbea an apology...

How much 3D programming have you done in the past? The code could very well be the culprit as well. Many systems have adjustments you can make on the accuracy of the surface or solid you're cutting on. If its too "loose", you could end up with some gouging, rough tool marks, faceting, etc. G61.1 may only amplify this effect. For the most part, if the transitions are smooth and the toolpath accuracy follows the surface (even with a .0002 step), the machine should still do a pretty good job.

The Mazacc 3D software allows for some leniency to the code. The option looks to smooth out the moves instead of forcing vectors. I believe it also has Nurb Spline with it as well which really speeds up the program and cutting ability. But you'll need a CAD system that supports spline programming and outputs.

Anyway,there are a few possibilities of the culprit. Machine parameters, machine metrology, programming codes, and CAD system accuracy at the time of toolpathing.

You guys both bring up a few other areas I'm concerned with:

-There is basically no size tolerance. It just needs to look good.

-I need to be able to feed quick and smooth. Minimum of 200ipm.

-For the CAM output: what size line segment should I force? I'd think a smaller line segment, like .0001-.0002 would allow the machine to travel from point-to-point in a more "flowing" motion, but I don't know if it can process fast enough to feed 200-300ipm with .0001 line segments. At the same time, I think .001 segments may cause a more jerky, start/stop type motion.

-This is going to turn into a relatively high volume part, so spending the time and money to get the process sorted out early will be worth it for me.

-Any ideas on which Mastercam toolpath strategy I should use? I'd like to have one continuous toolpath for finishing, that would start at the bottom and helix all the way to the top and then "blossom" out over the sides for the corner rounding operation.