What's new
What's new

Climb vs conventional milling in HSM toolpaths to maximize production

SRT Mike

Stainless
Joined
Feb 20, 2007
Location
Boston MA
I have a dilemma. I have hundreds of parts that need to be done ideally within a couple of weeks, but my cycle time is hanging around 30 min/part. The machine is a horizontal w/20k spindle. It has plenty of balls and very fast rapids, but it's a big machine and doesn't accelerate quickly. 20 min of the cycle is spent roughing (14,000rpm, 275IPM). I am looking at options to cut cycle time so I can get these parts done on time.

One option is changing my toolpath to cut also on the backstroke of the HSM roughing toolpaths, i.e. conventional milling. I tried a test part and it didn't sound too great until I bumped the RPM up to 20k (500ipm on the test cut in climb milling, 350 in conventional on the back cut).

I am using a Garr end mill with "alumastar" coating, 14k/275ipm was the recommendation from HSM advisor.

I have seen Helical Solutions recommends 16k RPM and up to 1,000IPM on their 3FL endmills. That seems almost too good to be true, but maybe? Another option is Destiny Diamondback, they are around similar numbers with their tools.

If I can cut both directions at higher RPM, I can cut 10+ minutes out of my cycle time, or increase daily part count by 50%.

Sooo... are these endmills really so different that I can run them at twice the feed? Or is it marketing BS? Should I be looking at other options besides these? ALso thinking about a corn cob rougher if I can get the speed, and come back with a finishing mill to clean up.

I have high pressure TSC and using TSC shrink holders for this application.
 
I have a dilemma. I have hundreds of parts that need to be done ideally within a couple of weeks, but my cycle time is hanging around 30 min/part. The machine is a horizontal w/20k spindle. It has plenty of balls and very fast rapids, but it's a big machine and doesn't accelerate quickly. 20 min of the cycle is spent roughing (14,000rpm, 275IPM). I am looking at options to cut cycle time so I can get these parts done on time.\

Conventional cutting on the HSM return paths is totally possible, but not ideal. Lopping off 1/3rd the cycle is a pretty massive savings though.

Can you tell us a little more about the part? Is this an open outside profile? Pocketing? Deep Z sorta deal? Your options are highly dependent on the nature of the material being removed.

You have a lot of power; I might look at putting a Sandvik 790 in that bad boy and going to town.
 
What about those Fraisa roughers Greg? The feeds and speeds on those were pretty healthy as I recall? Mike, I have removed about 100 cubic inches/minute in 6061 with the Hanita TC6A0R series corncob rougher with a 10 hp BT30 machine. 1/2" cutter, 1.25" axial, .300" radial, 275 IPM, 10k rpm. With your machine you can probably use a 5/8 or 3/4 and higher removal rate. I do like the idea of cutting material on the back move to increase removal rate, even if it is conventional. I try to do spiral type paths when possible for maximum engagement.
 
Conventional cutting on the HSM return paths is totally possible, but not ideal. Lopping off 1/3rd the cycle is a pretty massive savings though.

Can you tell us a little more about the part? Is this an open outside profile? Pocketing? Deep Z sorta deal? Your options are highly dependent on the nature of the material being removed.

You have a lot of power; I might look at putting a Sandvik 790 in that bad boy and going to town.

It's cast tooling plate. Helical's website has about 20 different flavors of cast AL plate with radically different feed possibilities, but the feeds are >600ipm on all of them, up to 2000ipm (which seems batshit insane).

I am going .825 deep on a 1" plate, basically hitting all surfaces. I have a large L-shaped open pocket about 3" wide on each leg of the L. Then I have another open pocket that is basically a square inside a square, and I am machining the area between them. It is an open pocket extending out the side of the part, and about 2" wide on the square path. Total part is about 23" x 10" x 1".

On the insert endmills, I thought about it but I am not sure I'd have time to get such a beast in time. I really need to get something locally in-stock. With my current 3FL 1/2" EM, I can hit 80% spindle load at 500ipm, which should be fine if I can just use a tool that will run reliably in that 500-750ipm range.
 
What about those Fraisa roughers Greg? The feeds and speeds on those were pretty healthy as I recall? Mike, I have removed about 100 cubic inches/minute in 6061 with the Hanita TC6A0R series corncob rougher with a 10 hp BT30 machine. 1/2" cutter, 1.25" axial, .300" radial, 275 IPM, 10k rpm. With your machine you can probably use a 5/8 or 3/4 and higher removal rate. I do like the idea of cutting material on the back move to increase removal rate, even if it is conventional. I try to do spiral type paths when possible for maximum engagement.

100cu-in/min is right about the magic number I am trying to hit. Ideally would like to achieve it with an endmill I can get locally from one of the resellers. I can get Helical, Destiny easily. I will check if the distributors carry that Hanita one. I've heard good about Destiny. And we have tried the high-balance EM's from Helical and gotten ungodly feeds (like 1000+IPM, at full DOC, but this is on a precision machine with 36k spindle).
 
What about those Fraisa roughers Greg? The feeds and speeds on those were pretty healthy as I recall? Mike, I have removed about 100 cubic inches/minute in 6061 with the Hanita TC6A0R series corncob rougher with a 10 hp BT30 machine. 1/2" cutter, 1.25" axial, .300" radial, 275 IPM, 10k rpm. With your machine you can probably use a 5/8 or 3/4 and higher removal rate. I do like the idea of cutting material on the back move to increase removal rate, even if it is conventional. I try to do spiral type paths when possible for maximum engagement.

I've got that order in on them to do testing with, but in my experience, serrated roughers don't like conventional milling at all. The Diamondbacks and TAS roughers I've done it with sound like hell unless you back way off on the parameters. At that point, you aren't gaining much while losing some process reliability and definitely dulling aluminum tools faster.

If SRT is really cutting roughing by 50% using conventional cuts on return loops, that usually indicates that it is a wide open part where you may have access with something like a 1.25 Sandvik 790 or Mitsubishi ASX. It is worth throwing it in CAM and giving it a simulation. He isn't power or RPM or rigidity or workholding limited, and this is one of those situations where old-school ploughing paths with a big, high performance indexed tool may totally cream HSM paths.

So many variables here, it is an interesting puzzle to figure out!
 
If you can get the Hanita in a 3/4 with TICN coating, you should be able to run that at 11k rpm, .850" axial,. 375" stepover, 330 IPM which is 105 cu"/min. Very efficient cutters, powdered metal, nice small chips, good price. Maybe try a back cut with reduced stepover like .100"?

This a possibility? :
TC6A0R-19007
 
If you can get the Hanita in a 3/4 with TICN coating, you should be able to run that at 11k rpm, .850" axial,. 375" stepover, 330 IPM which is 105 cu"/min. Very efficient cutters, powdered metal, nice small chips, good price. Maybe try a back cut with reduced stepover like .100"?

This a possibility? :
TC6A0R-19007

I could use that, although we try to stick mostly to 1/2" EM's in the shop, occasionally 5/8... mostly due to cost, although in this particular part, I have 6mm radii in the corners, so a 3/4 or 7/8 would he leaving a fair bit of material in the corners. But they have those in 1/2 and 5/8 also. But curious how they compare to Helical or Destiny - have you tried either of those?
 
I could use that, although we try to stick mostly to 1/2" EM's in the shop, occasionally 5/8... mostly due to cost, although in this particular part, I have 6mm radii in the corners, so a 3/4 or 7/8 would he leaving a fair bit of material in the corners. But they have those in 1/2 and 5/8 also. But curious how they compare to Helical or Destiny - have you tried either of those?

My frame of reference is optimizing for 30 taper. The Helical rougher looks great and I have recommended those to users. I like the lower helix for roughers. The Helical is 35 and the Destiny is 45 degrees I believe. If you are running this on a 40 taper or HSK 63 the 45 degree will be fine too I would think. What step over are you taking? If you can take bigger cuts radially you can cut down on the passes. I like how the Hanita has the Weldon flat for holding in a sidelock. Being that aggressive with a 1/2" you want to be sure it can't pull out of the holder. This video is a standard BT30 Brother with a 1/2" Cleveland PM rougher that used to be very good (they changed it). 1.25" x .300" x 200 IPM. I've done 275 IPM with the Hanita which is very similar to how the Cleveland design was.

YouTube

That was done quite a while ago when Dynamic milling was in beta testing, back feeds are at the same speed as cuts.

Your axial DOC is lower so you should be able to increase stepover and feed some I would think.
 
Last edited:
This video is a standard BT30 Brother with a 1/2" Cleveland PM rougher that used to be very good (they changed it). 1.25" x .300" x 200 IPM. I've done 275 IPM with the Hanita which is very similar to how the Cleveland design was.

YouTube

Those parameters (1.25 DOC, 0.30 WOC @ 200IPM) wouldn't break 100 cubes a minute, but the 275ipm would. Problem is, the old calculator says this is a 26hp cut, at over 9ft_lb of torque. I would be crazy to do that on my 16k Speedio, and I would be utterly irresponsible to do that on a client's BT30 machine.

Now, a beefy horizontal? I would probably crank it to 400 or even 500ipm with those same engagements, assuming we are happy with a ~30HP cut. This would all be with a .5 end mill, but if I wanted a little more process reliability, you could bump it to a .625 or .75 just to increase the tool rigidity a bit, get some room in the gullets, and help with chip evacuation.

There are all kinds of things you can play with on a part like this. If non-engagement moves are really soaking up so much of the cycle, you could start using sketches to break up the adaptive path so the algorithm optimizes a little bit. On low-depth applications, I'll even crank up the stepover to basically be at full slotting. Or bring in a big face mill and eat at everything it can access before stepping into the primary solid carbide tools.

One trick is that the algorithms all take geometry and offset it out into open areas, which can lead to a lot of excessive linking moves. Drop in a containment sketch with a circle or two that covers most of the stock to be removed; HSM paths are wicked efficient when spiraling outwards, and you can eliminate a lot of linking. A couple more sketch containments to bite around the excess as efficiently as possible, and you can dramatically increase the cutter engagement time.
 
Sorry if I missed it, but using adaptive HS paths, can you have the "return" moves go at rapid speeds? (sorry if that is a 'duhhh' moment)...

Also, and mentioned, maybe just purely 'hogging' with a bigger cutter may gain you some time vs HS paths..? Maybe plunge roughing, although the depth you have seems shallow for that type of path...
 
Sorry if I missed it, but using adaptive HS paths, can you have the "return" moves go at rapid speeds? (sorry if that is a 'duhhh' moment)...

Also, and mentioned, maybe just purely 'hogging' with a bigger cutter may gain you some time vs HS paths..? Maybe plunge roughing, although the depth you have seems shallow for that type of path...

You typically don't want to do rapids on your stay-down linking moves (the ones where the tool loops around, not the full linking with a Z lift). The problem is that most controls pause between G00 and G01/2/3 moves; they exact-stop check as the contour control pipeline refills. You also can get some funky motion depending on how CAM outputs the moves. The best practice is to set non-engagement feed rates to maximum machine feed and treat the whole thing as a cut.

Some controls (or Fanuc ladder configs by MTBs) are perfectly happy switching all day from G00 to cut feeds with no pauses, or treating a bunch of tight G00 moves as sort of a rapid G02/3. In that case? Go for it... but do test your CAM output with the machine.

This is the sort of stuff that Brother's deeply misunderstood High Accuracy comes into play. I can turn it off and rip in simple parts or complex stuff where I am leaving a lot of stock, so linking moves happen at crazy speeds. In a couple of production jobs, I've even manually edited code to turn High Accuracy on (or tighter) for only the handful of corners where gouging takes place, everything else is wide open. You have nowhere near this level of control with any Fanuc or Haas controller.
 
Sooo... are these endmills really so different that I can run them at twice the feed? Or is it marketing BS?

The alumastar is everything it says it is as far as speeds and feeds. I dont get any difference with niagras alum endmills(forget the name 50% cost more than alumastar) but the sharp corner last twice as long than the alumistar.
I havent cut conventional with any of them as far as roughing so I haven't heard the screeching, I also only go max 12k and if I recall I made a few rough cuts on big hog outs at 180IPM using a 1/2" standard length 1.25"? alumastar. big chips coming off.

the alumstars last a long time but the corners tend to chip rather fast, the Niagras running same feeds and speeds run longer and no chipping but again 50% more cost
 
Sorry if I missed it, but using adaptive HS paths, can you have the "return" moves go at rapid speeds? (sorry if that is a 'duhhh' moment)...

Also, and mentioned, maybe just purely 'hogging' with a bigger cutter may gain you some time vs HS paths..? Maybe plunge roughing, although the depth you have seems shallow for that type of path...

Set the no engagement feed to the max feed rate of your machine if you haven't done so already. I can set it faster than my machines feed and the controller just defaults to max feed rate, don't know if this could set an alarm on some controllers. Sorry if you already knew this but IMO sometimes its worth stating the basics.

Screenshot (65)_LI.jpg
 
Those parameters (1.25 DOC, 0.30 WOC @ 200IPM) wouldn't break 100 cubes a minute, but the 275ipm would. Problem is, the old calculator says this is a 26hp cut, at over 9ft_lb of torque. I would be crazy to do that on my 16k Speedio, and I would be utterly irresponsible to do that on a client's BT30 machine.

I was using this example to highlight the efficiency of the cutter. If a 10 hp 30 taper can take out 100 cu"/min with it then it should be able to do more with a higher horsepower/heavier duty machine I would think.
 
What about those Fraisa roughers Greg? The feeds and speeds on those were pretty healthy as I recall? Mike, I have removed about 100 cubic inches/minute in 6061 with the Hanita TC6A0R series corncob rougher with a 10 hp BT30 machine. 1/2" cutter, 1.25" axial, .300" radial, 275 IPM, 10k rpm. With your machine you can probably use a 5/8 or 3/4 and higher removal rate. I do like the idea of cutting material on the back move to increase removal rate, even if it is conventional. I try to do spiral type paths when possible for maximum engagement.

fraisa endmills are THE SHIT!

100 cubes in a bt30 machine? wow... thats impressive!
 
Just to add another good tool suggestion and because they aren't as well known for their end mills. This Emuge 20MM rougher is a beast, my personal favorite aluminum rougher I've ever used.

2888RZ.020 | Emuge Corporation

Parameters I got from Emuge that were spot on with a Mazak Variaxis with an 18K HSK63-A spindle:

3000 SFM -> 14800 RPM
0.008 IPR -> 355 IPM
40% Stepover -> 0.315"
1XD Stepdown -> 0.800" (Relieved neck so lower DOC)

With the thru spindle coolant running, the chip breakers, and the high RPM it looks like a chip explosion going off. I used Voiumill style HSM paths and it happily chew thru material all day. By my calculation that should be about 90 in^3/min MRR. I didn't really experiment with pushing the feed beyond that because it was fast enough for my application, but you can probably get more out of it. Should be a good fit for a horizontal machine application.
 
Set the no engagement feed to the max feed rate of your machine if you haven't done so already. I can set it faster than my machines feed and the controller just defaults to max feed rate, don't know if this could set an alarm on some controllers. Sorry if you already knew this but IMO sometimes its worth stating the basics.

View attachment 271478

Ya I don't go max because our machines will never reach it*. But I thought it might be worth a shot on using rapids for OP to cut cycle time.

Didn't see machine type, but if you have smoothing (filtering-accuracy or whatnot) settings you can adjust be sure to make use of those too.

* for clarity, our parts are small, we don't have enough acceleration to even get close to max feed in an inch or two.
 








 
Back
Top