Trochoidal Milling Parameters

[jbel]

I am looking for help with trochoidal milling parameters. I have looked around on the net and have not found any good results.

 

We are cutting H-13 Rc 45 using 1/4" Turbo-Carb ball mills. The machine is an OKK VP600 with 20000 RPM.

 

When roughing pockets I usually use a Surface Rough Pocket routine with .050" stepover and .050 step down, 12000 RPM and 120 IPM.

 

Just a standard parallel spiral from the inside out has given good results. I would like to try the high speed milling routine with trochoidal milling only in the corners but the cycle times for the cuts are about 50% longer than just a plain parallel spiral.

 

I am using the same stepover and stepdown. I know I need to change these values but I was hoping for a little guidance instead of trial and error.

 

Any help would be greatly appreciated.

[PE @ IHS]

your stepdown needs to be doubled or tripled. The whole idea is to take a much deeper Z cut, but reduce axial load by "nibbling" at the material radially. Also, use trochoidal cuts in full material only.

 

I have taken an .800" deep cut in 4140 steel using a .25v dia endmill using trochoidal cutting.

[T_MALENA]

Jbel, do you have a .mc9 file you can post? Like Peter says the idea is to take deep z-depth cuts & small axial cuts. I've done this with good results. Sometimes its faster sometimes not. It really shines when needing deep cuts as opposed shallow cuts( thin walls, tool wear etc.)

[steve f]

jbel,

 

what's worked well for me in the past, depending on the pocket geometery, is to use a morph spiral toolpath: thread mill toolpath with very shallow pitch somewhere at pocket center to enter the material, create a small false island at entry point location and morph spiral the pocket chain and island using small stepover. Like Peter mentioned a deep axial and small radial cut works better than expected, and the feed can really be bumped up because the actual chip thickness is far smaller than taking a 50% radial cut...it sounds like you have the perfect machine to do it too.

 

steve

[BernieT]

Is there a way to cut a 'slot' using 'trochoidal milling'? Not a pocket, but a slot going clear thru a block. I haven't been able to find a way to make it do just one pass and not return as in an open pocket.

 

Thanks.

[jbel]

NDA's prevent me from posting files to the FTP, but here's what seemed to work the best.

 

Axial and radial step over set to the ball mill radius and trochoidal cutting at full material only. For a 1/4" ball mill, loop radius and spacing both at 0.05".

 

BerTau,

For a slot why not just use the pocket toolpath??

I set the depth as deeper than the workpiece and it worked well for me.

 

T_Malena,

Where in Solon are you?? I work right on Cochran Rd.

[Tom Szelag]

Peter do you have a sample MC9 of the settings youre running that you could upload? This whole thing is new to me and I'd love to see the run times for that as opposed to conventional milling.

[T_MALENA]

Jbel,

 

I work right off Cochran Rd.

 

Carter st. Christopher Tool

 

I'd guess you work right around the corner. Small world huh?!