[cncClintain]

Whats more efficient for roughing decent size stainless parts on a mill? Trochoidal with solid carbide or traditional tool paths with 2" inserted cutters? Im mainly talking about cycle time but also need to consider tool life and cost.

[barbter]

Dynamic. Spiral in with a 4x flute centre cutting carbide, and let her go with a 10% stepover.

[jamesu229]

Depends on too many factors for an instant answer. Part profile, pockets, thickness, cubic inches to be removed, machine capabilities, tool manufacturer and type of stainless steel would be the main things to decide this.

[cncClintain]

Depends on too many factors for an instant answer. Part profile, pockets, thickness, cubic inches to be removed, machine capabilities, tool manufacturer and type of stainless steel would be the main things to decide this.

Lets just say an area 10" x 10" x 2" in 316, not necessarily a pocket. And lets just say SGS solid carbide with a good coating around 3/4" vs. 2" sandvik inserted cutters with 5 inserts.

[jamesu229]

trochoidal paths most likely would be best. 316 ss is part of the 18-8 series of stainless, slightly more abrasive than 304. The part in the video was 304 and roughly the same area as yours. Proghrammed using truemill.

[nomedia="http://www.youtube.com/watch?v=XtKMefi4Ck4"]YouTube - ‪TRUEMILLING 304 SS‬‏[/nomedia]

[cncClintain]

trochoidal paths most likely would be best. 316 ss is part of the 18-8 series of stainless, slightly more abrasive than 304. The part in the video was 304 and roughly the same area as yours. Proghrammed using truemill.

YouTube - ‪TRUEMILLING 304 SS‬‏

Thanks. I always liked the dynamic toolpath in mastercam but never used it in 316 and the shop i just started at is in love with their inserted cutters but theyve also been doing everything in mazatrol

[jamesu229]

have they looked at any videos like this one or researched high speed machining. If not, It may not take much to get them hooked. Get them to watch my other videos, I have one posted that is running 17-4 ss at 1650 sfm and up to 720 actual ipm, dry

[cncClintain]

have they looked at any videos like this one or researched high speed machining. If not, It may not take much to get them hooked. Get them to watch my other videos, I have one posted that is running 17-4 ss at 1650 sfm and up to 720 actual ipm, dry

Thats a hefty feed rate. How do you figure your feeds and speeds for the small step over? I have found several formulas for the Radial Chip Thinning Factor but your feed rate still seems to be pretty high in comparison to recommended feed rates even with the Radial Chipping Thinning Factor taken into consideration. Is it the cutter you are using? Also, as your step over decreases I know your SFM can be increased. How do you figure this as well? Thanks for all of the info. We cut a lot of 316 and 304 and I think this should be the approach we take from now on.

[jamesu229]

Thats a hefty feed rate. How do you figure your feeds and speeds for the small step over? I have found several formulas for the Radial Chip Thinning Factor but your feed rate still seems to be pretty high in comparison to recommended feed rates even with the Radial Chipping Thinning Factor taken into consideration. Is it the cutter you are using? Also, as your step over decreases I know your SFM can be increased. How do you figure this as well? Thanks for all of the info. We cut a lot of 316 and 304 and I think this should be the approach we take from now on.

The endmills in the videos are my regrinds. The feed rates are from trial and error. In steel alloys under 30Rc I use a sliding scale .025 radial = .015 ipt translating to .250 radial = .005ipt for a 1/2" endmill at full depth. more times than not, sfm is determined by the machines lack of horsepower, accuracy and/or feed rate capabilities. I usually max out the machine in one way or another. Its great to program for a regular employer during the day and run a high performance endmill sharpening service at night, makes long term testing easy. With 300 series stainless, lower sfm and high feed rates are the best combination. Wish it was all 17-4, aka butter.

[cncClintain]

The endmills in the videos are my regrinds. The feed rates are from trial and error. In steel alloys under 30Rc I use a sliding scale .025 radial = .015 ipt translating to .250 radial = .005ipt for a 1/2" endmill at full depth. more times than not, sfm is determined by the machines lack of horsepower, accuracy and/or feed rate capabilities. I usually max out the machine in one way or another. Its great to program for a regular employer during the day and run a high performance endmill sharpening service at night, makes long term testing easy. With 300 series stainless, lower sfm and high feed rates are the best combination. Wish it was all 17-4, aka butter.

Thanks a lot. This is my first time with the stainless and Ive been watching them feed these inserted cutters straight into the side of the parts to rough them and its just beating the hell out of the cutters and I was wanting to show them this method but I just wasn't certain on feeds and speeds and Im new so I didn't want to go in and just start blowing up cutters.

[barbter]

and I'd run 1/2" rather than 3/4 tools. It gets the revs up and the tools are cheaper!

[Ydna]

I agree with the above, for ferrous materials anyway.
If working with aluminum you probably max out the removal rate by taking a full-depth, widest stepover cut as possible. it can be slow, but the amount being removed per pass is tremendous with a quality endmill. But with steels it's hard to do that unless you have a freakishly heavy spindle, and/or want to sacrifice the tool for only a few parts. So I agree that a dynamic toolpath is the way to go....I like using the 6 flutes for roughing myself (not with a crazy feed per tooth tho since I don't do a lot of production work in steels)

But if you were trying to rough out a surfaced feature you may want a different toolpath (high feed), unless you have X5 which as a dynamic surfacing ability.

[cadcam]

I have used the Dynamic paths in mastercam to do high speed removal they work well for sure.
There are some charts for chip thinning on the Mastercam forum that can help with different tool and materials.
You do not have to have surfcam for what James is doing or even truemill that could be added to MC.