HSM thoughts/help

OK folks, I went back in the archives, and I've got some help there, but I probably just still don't understand enough to make it useful...

Have to hog out areas of the parts I'm working on. Material is 303 Stainless. Machine is a Haas VF2ss. I've got Kennametal cord profile 1/2" diameter 5/8" CEL Roughers. Their book gives me 300-380 SFM, and .0025 chip. They also give me 40% for the stepover, and 1/2" depth of cut. So I was running that, and just destroying the cutters in short order, but that run had to go out, so I just threw cutters at it, and finished...

Next project isn't such a rush, so digging in to some HSM info gave me a recommendation of double the low side of the SFM, and 2.5 times the chip load with a 4% stepover. So far that sounds a lot better in the machine, service life is yet to be determined since I just got the parts running... Looking forward to the next side of these parts is where the real material removal is, I'm just wondering if those numbers look good to those with more experience...

The next question is, should I even be bothering with roughers, or just go to a regular cutter? Does anyone even run roughers with HSM paths? I have found exactly zero posts here or elsewhere talking about that...

If you're brand new to HSM, Harvey tool put together a nice document that explains all the principles with some graphics and guidelines. Worth a look through.

Download the Free HEM Guidebook

I typically like to run 5-15% stepover at full DOC if I'm doing HSM style. A lot of end mills out there can handle higher stepover nowadays, but you need to look at your holders, the machine, part geometry, workholding, etc. before getting too crazy. You very quickly get to where a cheap ER collet is not able to keep up.

As far as roughers, I'm a big fan of chip splitters on cutters, not so much the old "corncob" style roughers. Modern chip splitters take care of the massive chip buildup problems you can have making all those long needles, and can still leave a decent finish behind sometimes.

What are you programming with?

CNC Hacker said:

If you're brand new to HSM, Harvey tool put together a nice document that explains all the principles with some graphics and guidelines. Worth a look through.

Download the Free HEM Guidebook

I typically like to run 5-15% stepover at full DOC if I'm doing HSM style. A lot of end mills out there can handle higher stepover nowadays, but you need to look at your holders, the machine, part geometry, workholding, etc. before getting too crazy. You very quickly get to where a cheap ER collet is not able to keep up.

As far as roughers, I'm a big fan of chip splitters on cutters, not so much the old "corncob" style roughers. Modern chip splitters take care of the massive chip buildup problems you can have making all those long needles, and can still leave a decent finish behind sometimes.

What are you programming with?

Click to expand...

I don't know stainless very well, but 4% sounds pretty low. I would try upping that first. Also, .0025" ipt will probably (again, not sure with stainless) be too low for HSM paths with chip thinning.

Programming via HSMWorks.

The Haas is low mileage... The company bought it, used it for a few months, then it sat idle for a number of years until I got here. So it's a few years old, but everything is still solid, and tight. Tool holders in this case are Techniks, side lock. I could go to Techniks ER 25 if I had to. I run some no name China holders on non demanding tools, but I don't mess around with them if it is going to need to be right, or loaded up...

My background in CNC is from Routing, and wood/plastic. I've been doing pretty well with the aluminum work, and stainless has been ok because it has been low volume in house parts only until recently. My real job here is more on the design/R&D side, most of our parts get jobbed out to a shop that does immaculate work...

Stick with the sidelock, stick with 600SFM, go up to .006IPT (still on the light side), and I would be more like 6-7% stepover. 4% is very light. Keep increasing the stepover until you don't like tool life or the machine complains. Then go back to a good stepover and start increasing the feedrate. Adjust for tool life, season to taste.

Make sure your machine is actually feeding somewhere around what you programmed. If, for example, you program 400IPM but it's only actually cutting at 200IPM, you're going to rub the tool to death and have no idea why.

Next, start learning about G187 and how you can adjust it to get the feedrate up to programmed speed.

I am sitting here reprogramming somes parts for HSM while the 1t 2 ops are running. happen to see this thread. o figured I would put my 2 cents into it.

I can tell you what not to use, thats the 3 and 4 flute indexable holders by sandvik or anyone for that matter, your hass vf2ss wont handle it and will beat the snot out of the machine. not to mention insert wear is very high. solid carbide in 3 and 5 flute works much nicer except again it wears them out fast.
I ended up tossing the job on the old fadal and had no problems except with the indexable inserts they werent beating the machine up but they wore fast. tried 4-5 different grades and every sfm imaginable.
were running another 50+ of these parts and this time using all solid carbide, corn cob style for roughing and 5 fluters for finishing had real good luck with the HTC hot mills and there other mills.

The blanks are 7x9x1.125 weigh about 35-40lbs each? when there done they may weigh 2 oz's tops .030 and .050 wall thickness.
I'm going to try a few with HSM to see if that induce any stress into the part as we cant have them bending and warping.
to give you an idea the sandvik r390 series 3/4" indexables lasted 2 parts roughing at the most. the last part of the run we were able to get 4-5 rough cycles out however it put a bunch of stress into the part.
one endmill a solid carbide regrind no coating and ground very sharp with a .030rad lasted almost 40parts rough and then then finish with full width cuts at .200 doc 5 slots each one, 4 .200 DOC. pass's. dump the collet holder side locks worked better in my case and we ground a flat into the carbide.

dont get me wrong I'm not bashing the hass as we use what we have avail. they just dont like those indexable inserts on stainless.

Matt@RFR said:

Stick with the sidelock, stick with 600SFM, go up to .006IPT (still on the light side), and I would be more like 6-7% stepover. 4% is very light. Keep increasing the stepover until you don't like tool life or the machine complains. Then go back to a good stepover and start increasing the feedrate. Adjust for tool life, season to taste.

Make sure your machine is actually feeding somewhere around what you programmed. If, for example, you program 400IPM but it's only actually cutting at 200IPM, you're going to rub the tool to death and have no idea why.

Next, start learning about G187 and how you can adjust it to get the feedrate up to programmed speed.

Click to expand...

Matt
what type of HSM path do you use? the circle one? tric something?

Delw said:

Matt
what type of HSM path do you use? the circle one? tric something?

Click to expand...

Mastercam's Dynamic paths, but it shouldn't matter. WOC is WOC.

Matt@RFR said:

Mastercam's Dynamic paths, but it shouldn't matter. WOC is WOC.

Click to expand...

Thanks
I've used the peel mill one quite a few times a few years back, never played with high speed machining very much.

tool length sticking out is a important factor in tool vibration and tool life. as well as part shapes that might vibrate under heavy load.
.
just saying what you can do with a 0.5"dia end mill sticking out 1" and what you can do with it sticking out 2" is quite different. basically 2x2x2 or 8x different. its a cube law of deflection to length
.
in general the thicker the chip usually better until sudden tool failures or cutting edges start breaking off. if i turn 100lbs into .001 thick chips its different than .010 chips. if i shear a 6 foot by 10 foot 1/2" thick steel plate in half with a shear its more efficient than turning 6by5 foot of plate into .001" thick chips
.
one advantage with bigger diameter insert mills with big thick carbide inserts is often the ipt is in the .010 to .020" range which a little 1/2 dia end mill cannot take without edges breaking off.

Toolslinger said:

should I even be bothering with roughers, or just go to a regular cutter? Does anyone even run roughers with HSM paths? I have found exactly zero posts here or elsewhere talking about that...

Click to expand...

The ONLY time I use an endmill that has a chipbreaker is when I'm removing so much material that the augers can't keep up with the big thick chips.
Get yourself a good 4-5 flute variable helix end mill similar to this one:
GARR TOOL

And get a copy of HSM Advisor for your speeds and feeds, it's invaluable.

Toolslinger said:

The next question is, should I even be bothering with roughers, or just go to a regular cutter? Does anyone even run roughers with HSM paths? I have found exactly zero posts here or elsewhere talking about that...

Click to expand...

I like roughers myself, and run them in all forms of steel. I typically run a 10% step over for roughers and do a quick skim pass for finish and size. I really like Micro 100's website for feeds and speeds (HSM Advisor). Though at times it can be a bit confusing what it outputs. Sometimes it is REALLY conservative. Sometimes it is FAR higher SFM or CPT than the manufacturer recommends. Sometimes that is OK, sometimes it is not.

I have one of the Garr tools mentioned above on the way to do some testing with. I use YG X-power mills 6fl, for my finishers, and absolutely love them. Last a Looooong time and I can run them at REALLY high speeds and feeds. If the Garr tools run just as well, I will switch to them. IF they run as well, I may start using a worn finisher as a rougher like what MtnDew suggested.

Matt@RFR said:

Make sure your machine is actually feeding somewhere around what you programmed. If, for example, you program 400IPM but it's only actually cutting at 200IPM, you're going to rub the tool to death and have no idea why.

Click to expand...

I had/still have an '08 VF2ss that was running a 3/8" solid carbide em at something like 250ipm (MasterCAM "dynamic mill")...at the time it was the fastest I'd ever seen a machine feed.) Then I got a Brother S2Dn to run the same part with the same program (minus the "%'s" ) and was worried because something was "wrong" - the Brother was feeding "WAY too fast!" The Brother salesman (who I think I trust more than anyone I've ever met in the biz) explained that the Brother was actually feeding at (or at least "closer to") the programmed feed rate and the Haas was not, regardless of what the "POS" screen on the Haas was saying.

I am NOT turning this into a Brother vs. Haas thing. I am just saying it is worth putting some effort into figuring out how fast your machine is actually moving so you can compensate for it with your cutting parameters.

I use SGS(/Kyocera now) V-Carbs for my steel.

Cheers!

I use chipbreaking roughers just to minimize chip volume. They make such a huge difference in the volume of chips that it's hard to describe. A quick estimate was that my chip volume is 1/10 to 1/15 that in a similar program with chipbreakers vs using standard end mills. They pack down so much nicer. Only downside is they seem to carry more coolant away in the chips but it's well worth it for the reduced volume.

Thanks to all... Lots to look in to, and now another rabbit hole of actual feed rate to fall down...

At least once I get parts running, I have time for research...

And just because I hate when threads don't have a wrapup....

I ended up going to Lakeshore variable 5 flute stub length cutters rather than the Kennametal 4 flute stub length roughers I was using. I went from getting 2 parts per cutter to 4.5 parts before there was enough wear to cause issues. Cycle time dropped as well with that extra flute, which was nice... I also found I just couldn't do the HSM paths on the second side without pulling the piece out of the vise. Regular paths were ok, but once that cutter got just a little dull, it was time to swap. By the time the part is done it went from 7x7x3/4 to basicly two 1/8" flat sections spaced apart by 3 - 3/8" square sticks... Nothing but opportunity for vibration...Ugh.

Thanks again all.

Oh and additional thanks to Delw... I should have read that bit about the indexables better... Next project bit me on that... Reached for a 3 flute indexable to bore out a blank (wish we had a lathe for this) and man did that beat the crap out everything... Quickly ended that folly, and sent it off to have most of it hogged out elsewhere...

Mtndew said:

The ONLY time I use an endmill that has a chipbreaker is when I'm removing so much material that the augers can't keep up with the big thick chips.
Get yourself a good 4-5 flute variable helix end mill similar to this one:
GARR TOOL

And get a copy of HSM Advisor for your speeds and feeds, it's invaluable.

Click to expand...

HSM advisor is one of the best "cheap" investments ive made.
Hands down.

Mtndew said:

The ONLY time I use an endmill that has a chipbreaker is when I'm removing so much material that the augers can't keep up with the big thick chips.
Get yourself a good 4-5 flute variable helix end mill similar to this one:
GARR TOOL

And get a copy of HSM Advisor for your speeds and feeds, it's invaluable.

Click to expand...

Oh, regarding the chipbreaker tools... I wish I had one for this job

High flow coolant goes a long way towards chip management. Get a better coolant pump on there and you'll get those chips off the table. The pump on my machine is 100L/min and it's very good at getting chips out of the machine. I wish it had more pressure for clearing chips from deep slots but otherwise it's very nice to have a lot of flow.