4th axis toolpath question

[jeff]

I have a part that looks like a simple round part with 2 male keys at 180 degrees from each other sticking out. 

It's in my rotary, and I have holding stock. What toolpath would you guys use to mill this form?

Using a 1/4" ballnose.

 

I cut the sides of the male keys with a 1/2" endmill using a normal 2D contour, now I need to cut the diameter

4" stock 

keys are about 3/4" wide

diameter at bottom of keys is 3-1/2 -ish

[Chipmakr]

Can you put up a screen shot or file? You could just use a 3 axis path and do 180° the flip & repeat. If I did multi axis maybe a morph between two curves locked down to 4axis motion.

[jeff]

Here is a rough model of the surfaces. 

[JMahon]

I would contour finish the tabs, then use surface finish parallel on each side. Your mismatch will be at the tabs and won't be so noticeable.

So contour tabs at 0 and 180. And surface the od at 90 and 270.

[jeff]

Thanks, 

I'm new at contouring on a 4th axis. All I've done so far is your basic hole patterns and whatnot.

[JMahon]

Or morph between two curves for added coolness...

[djstedman]

I would say this really depends on your tolerance.. if the part needs to be a tight tolerance diameter you need to worry about  having a 'bump' at the top as you hit 0 surface footage as the tip of the ball drags over the top surface, using an indicator and rotating the part after contouring you will probably see about .002 'bump' where it doesn't cut well at the center of the ball.

 

If diameter tolerance is important then a full fourth axis path which keeps the tool cutting off centerline is going to work out much better.

 

And if the shape truly is that simple you could just write an sub with rotation included to make a cut across the part and back then incremental rotation, then call it however times you need..

[jeff]

The tolerance isn't critical, this is more of a learning experience for me.

I used multi/rotary with a .02 stepover. 

After 7,000 attempts I finally figured out what my problem was, the default value for keeping the tool down within 300% of the tool dia. 

Changed that to .01" and it worked fine. 

I was mainly looking for other path options that you gurus would use.

[djstedman]

Well I had to do something similar that was fussy.. I used a multisurf  5 Axis (constrained to only 4) , Cut pattern set to surface and chose surfaces, then tool axis control as pattern surface and give it some side tilt (or lead lag depending on direction of cut)

 

The side tilt / lead lag keeps the tool cutting on the side of the ball rather than ever using the tip. by changing flow parameters you can make this path cut full fourth while rotating or cut across the surface and index.. either way I have found this to be an extremely handy toolpath.

 

If you do try and use it keep in mind it doesn't (or at least didn't in my case) respect linking parameters between toolpaths very well at all.. hopefully multiaxis linking helps this..?? In my case I just used force tool change between toolpaths to make it go home before starting the next path.