Insert mill for roughing on a less rigid setup.

[BRIAN.T]

I've got a part I'm running on a 5 axis hsk63a 40hp machine. It's about 6x6" cube of 1018. It ends up looking like a "T" when it's finish. It's clamped in a lang vise on the bottom of said "T", the specifics aren't super important other than to say it's not a super rigid setup, but for various tolerance call outs, it's exactly how it should be held. the bulk of the part and stock is up, over and outside the vise.

Now as it currently stands most of the roughing happens with the table at 90 degrees.

I'm using a 1/2 6 flute end mill
650sfm
1.1 axial
.09 radial
.004 chip.
11.8 cubes.
12 parts, before tool change.

This seems to be the sweet spot. I'm up from 10 percent at .007 chip. Far fewer entries, better tool life.

With that being said, I'm not usually one to try to save a couple bucks, but in this instance I feel like I've got some decent room for improvement. I'm wondering what kind of insert cutter might be available for a less stable setup. I don't have much experience with high feed mills, but I do suspect the considerable down force produced by a high feed cutter might be too great (remember part is at 90 degree) with a high feed capable of cutting a comparable MMR.

Thanks.

 

[mhajicek]

I'd go with solid carbide endmills and dynamic paths. They work well for me in grade 5 Ti in similarly nonrigid setups; I can get 5 cut hours out of one. Cutting forces on indexables are generally higher, causing more deflection, but maybe a screw on high feed tip if you want to try something different?

 

[BRIAN.T]

I'd go with solid carbide endmills and dynamic paths.

I believe in my heart you are right, that's where I'm at now for a reason... I feel like there is a cool alternative I'm not aware of. Maybe Im just looking for a reason to play with new tools.

 

[Orange Vise]

Your decision doesn't need to be binary.

Combine the two. Hog out 75% of the material with a 2.5" or 3" diameter indexable and then have at it with solid carbide.

 

[Milland]

If I had an inherently flexible machine (due to the many stacked axis and long distance from mechanical joints to cutting forces), I'd be very happy with smooth, continuous low-load cutting.

I would avoid "impacting" types of cuts from inserts. Ditto avoiding large radius cutters.

Can you rough on another, "regular" three axis mill? That might be the best option.

 

[BRIAN.T]

Your decision doesn't need to be binary.

Combine the two. Hog out 75% of the material with a 2.5" or 3" diameter indexable and then have at it with solid carbide.

Damnit, deleted my own reply by mistake. I've tried a 2" 90 degree shouldering type mill. It's a great tool for a rigid setup, but in this instance it just chattered like hell. I'd need something that it's so aggressive.

 

[Lastu]

So is there a reason the roughing can't be done at table 0? Can't really visualize the part.

Some high-feed mills cut smoother than other, but typically inserts are always rougher than endmills.

Lähetetty minun SM-G973F laitteesta Tapatalkilla

 

[BRIAN.T]

So is there a reason the roughing can't be done at table 0? Can't really visualize the part.

Some high-feed mills cut smoother than other, but typically inserts are always rougher than endmills.

Lähetetty minun SM-G973F laitteesta Tapatalkilla

Yes sir! I'll try to get a drawing posted later today, but for now you'll just have to trust me. Think of it as two pockets on either side of a cube. In your experience which tools cut smoother than others? Thanks

 

[BRIAN.T]

If I had an inherently flexible machine (due to the many stacked axis and long distance from mechanical joints to cutting forces), I'd be very happy with smooth, continuous low-load cutting.

I would avoid "impacting" types of cuts from inserts. Ditto avoiding large radius cutters.

Can you rough on another, "regular" three axis mill? That might be the best option.

I may go to roughing on a separate mill, there isn't a good reason not to, other than this machine is significantly more powerful than my 3 axis selection, and I like doing as much as possible in on op, just less to setup. But that's minor details.

 

[plastikdreams]

Just thinking a little, having not seen the drawing....is this a high volume part? Could wire edm be used to remove the bulk leaving you with a nice surface to complete the finishing on.

 

[BRIAN.T]

Just thinking a little, having not seen the drawing....is this a high volume part? Could wire edm be used to remove the bulk leaving you with a nice surface to complete the finishing on.

Certainly could be. We could even band saw it off. It's reasonably high volume. But I really hate paying other people to do work I can do. But also, where is the fun in that? I love roughing steel.

 

[mhajicek]

Yeah, I'm sticking with screw on solid carbide high feed tips as your most viable alternative option. It'll be sharper than an insert, so tool force will be lesser. Plus high feeds are pretty chatter tolerant, and you can get the shank whatever length is optimal.

 

[BRIAN.T]

Yeah, I'm sticking with screw on solid carbide high feed tips as your most viable alternative option. It'll be sharper than an insert, so tool force will be lesser. Plus high feeds are pretty chatter tolerant, and you can get the shank whatever length is optimal.

Interesting, I'd be curious to that that. Who's do you like? I have a few iscar multi master tools, and I've been happy with them. But I'm open to anything.

 

[Matt_Maguire]

I've got a part I'm running on a 5 axis hsk63a 40hp machine. It's about 6x6" cube of 1018. It ends up looking like a "T" when it's finish. It's clamped in a lang vise on the bottom of said "T", the specifics aren't super important other than to say it's not a super rigid setup, but for various tolerance call outs, it's exactly how it should be held. the bulk of the part and stock is up, over and outside the vise.

With that being said, I'm not usually one to try to save a couple bucks, but in this instance I feel like I've got some decent room for improvement.
Thanks.

The cutter may not help as much as a good setup, your forces at the outer edges lever back to the center & then "couple" down to the top of the vice jaws... That's a bunch.

Just thinking (vert. spindle), if the tool is 4” or more over the top of the vice jaws you’ve got a beautiful demonstration of why “steel” makes great springs, LOL.

I’d trade the 10 seconds for vice clamping with a 15-20 minute one time setup using a 6” angle plate with a side fence + 3 toolmakers clamps + 2 “Little Giant” style screw jacks (go under the outside of “T” shape). If things are right the jack screws never need adjusted after the first part (they are just a fixed extension of the table surface). Fiddling with the 3 clamps make for 30-60 seconds to loose the misery of the part wobbling under the tool. Your actual tools to machine way surface will be less than with a vice also, believe it or not it helps some.

Good luck,
Matt

 

[Peter from Holland]

Have the shapes oxycut out of 6" 1018 plate perhaps


Peter

 

[BRIAN.T]

The cutter may not help as much as a good setup, your forces at the outer edges lever back to the center & then "couple" down to the top of the vice jaws... That's a bunch.

Just thinking (vert. spindle), if the tool is 4” or more over the top of the vice jaws you’ve got a beautiful demonstration of why “steel” makes great springs, LOL.

I’d trade the 10 seconds for vice clamping with a 15-20 minute one time setup using a 6” angle plate with a side fence + 3 toolmakers clamps + 2 “Little Giant” style screw jacks (go under the outside of “T” shape). If things are right the jack screws never need adjusted after the first part (they are just a fixed extension of the table surface). Fiddling with the 3 clamps make for 30-60 seconds to loose the misery of the part wobbling under the tool. Your actual tools to machine way surface will be less than with a vice also, believe it or not it helps some.

Good luck,
Matt

While I like where you head is at, I've got to machine all sides of this part. Certainly I could rough a lot of this part on another machine, but as soon as I move to 5 axis I need all the sides free. Thanks

 

[Orange Vise]

Damnit, deleted my own reply by mistake. I've tried a 2" 90 degree shouldering type mill. It's a great tool for a rigid setup, but in this instance it just chattered like hell. I'd need something that it's so aggressive.

Ok so the workpiece itself is fine (a 6" cube is inherently very rigid). The problem is the workholding.

Have considered an entirely different method of workholding?

For example, ditch the vise. Prep your stock to take the pull studs in the 96mm pattern and directly clamp to the riser.

 

[mhajicek]

Interesting, I'd be curious to that that. Who's do you like? I have a few iscar multi master tools, and I've been happy with them. But I'm open to anything.

I haven't used high feed cutters for about six years or so; I haven't had the right application. Back then I was doing die and mold, so the indexables for big areas, and Niagara 3mm solids for small areas. I did just get some of Helical's new solid HFMs in 3/8", but I haven't used them yet.

With the HFM, maybe you could rough out a pocket, leaving the walls on the ends for rigidity so you can cut more aggressively, then come back and cut away the walls later.

 

[Matt_Maguire]

Damnit, deleted my own reply by mistake. I've tried a 2" 90 degree shouldering type mill. It's a great tool for a rigid setup, but in this instance it just chattered like hell. I'd need something that it's so aggressive.

See your problem now (from post #6), except for how bad 1018 can move while cutting most of it away… Your left with the machining recipe & tools.

I’d prolly near finish the top & then work under the top balancing the roughing cuts side to side moving down to the vice. You used to be able to get endmills with reduced helix or straight sided that significantly reduced the complex pulling that happens to the cutter (and somewhat to the part). Most inserted shoulder mills are already like that?

The 1018 (6” brick) will move (bow) fairly machining along the grain (rolling direction) and move very little across the grain.

Good luck,
Matt

 

[TeachMePlease]

Interesting, I'd be curious to that that. Who's do you like? I have a few iscar multi master tools, and I've been happy with them. But I'm open to anything.

Just FYI, per my GWS guy, GW Schulz now makes custom tips that fit Iscar multimaster bodies. So you could talk to them about some tools with optimized geometry for what you're doing.