HSM - High Speed machining

Help Support HMEM:

Swede

Well-Known Member
Joined
Apr 7, 2011
Messages
460
Reaction score
9
^^ That's my tricky title for yet another feeds & speeds question!

I've never been big on mathematically-derived feeds/speeds for manual work. I usually speed things up until I can physically feel a bit of laboring going on, or the cut doesn't work out right, but under NC, there is no feel, and I must program in the correct parameters.

What I am doing is leaning towards the traditional definition of HSM... high spindle speeds and feeds, with a "bite" appropriate for the spindle wattage and the cutters in use. I want to mill several small but complex 3D parts from 7075 aluminum, using both 1/8" and 1/4" carbide mills. My spindle is only 600 watts, but I can dial upwards of 50,000 RPM.

Can anyone point to a good online speed/feed calculator, or suggest basic parameters for light but fast cuts in aluminum? As always, thanks.
 

kustomkb

Project of the Month Winner!!!
Project of the Month Winner
Joined
Dec 14, 2007
Messages
1,181
Reaction score
31

I believe high speed machining is in reference to the cutter path rather than RPM's. IE the cutter is always climb milling while continuously maintaining the same amount of material engagement.

50,000 rpm is nice but can your feed rates match it?

A general rule for depth of cut is 10% of the cutter diameter.

1/8 roughing, I use .0025" per tooth and .0013" for finishing.

1/4 roughing, .0036" per tooth and .0015" for finishing.

I generally will run a 1/4, 4 flute end mill at 7000 rpm and 100 inches per minute.

At 50,000 rpm I would have to feed at 720 IPM.

 

dieselpilot

Well-Known Member
Joined
Jan 17, 2009
Messages
1,349
Reaction score
109
You have to be careful with this idea. Real HSM CAM software looks at tool engagement in every move. Most anything else does not. It's easy to overload the tool on an inside corner or scallop if the software doesn't look for it. The key to HSM is mostly toolpath.

I arrived at acceptable feeds and speeds for my low power high rpm setup by trial and error. I use VisualMill and there is no way to trust it to make toolpaths acceptable for very high feedrates. It occasionally makes moves that leave me shaking my head, but the step up to a better CAM software is pretty large. Even with very small feed per tooth my endmills seem to last a very long in aluminum. 7075 cuts extremely well. I suggest you just see what your machine is actually capable of, just watch out for those killer moves.

I too have seen the DOC=10%diameter, but there is no shortage of videos on youtube with 100% DOC.

[ame]http://www.youtube.com/watch?v=j0SZg0WH6DA[/ame]

Greg
 

kvom

Administrator
Staff member
Administrator
Global Moderator
Joined
Jun 4, 2008
Messages
3,164
Reaction score
592
I use G-wizard for F&S calculation.
 

Swede

Well-Known Member
Joined
Apr 7, 2011
Messages
460
Reaction score
9
Thanks for the replies, everybody.

When I say "HSM" I speak in terms like "It's something I'd like to approach or emulate, but the hardware and software will be out of reach." diesel, I also use Visualmill, and I like it, but for something considered kind of low-end, it's expensive, and there's no way I can justify anything more costly.

I did some tests the other day. My system had no problems milling 7075 at 30,000 rpm, 40 IPM, with a 0.030" depth of cut. Not high speed, but I'm kind of chicken. I hate breaking cutters, but at the same time, high RPM is useless or detrimental with a slower feed. I also have problems with clearing chips. I don't use flood, so I need to either set up a vacuum or air blower, and I am leaning towards a vacuum with a thin tip probe, close to the cutter.
 

Swede

Well-Known Member
Joined
Apr 7, 2011
Messages
460
Reaction score
9
I did find an easy to use calculator:

Feed Rate Calculator

http://www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml

I am using SFM = 1,000 for carbide end mills in 7075. This produces a 30,000 RPM for a 1/8" EM. Using a light feed load/tooth of 0.000,6 creates feed rates of about 90 and 45 for 4 and 2 flute cutters, respectively. If the tooth load is increased to more normal values like 0.001 and more, the feed rates skyrocket.

Let me ask a question - what harm would result from extremely low tooth loads like 0.000,2? I assume rubbing/dulling of cutters, but anything else? The surface finish should improve (to a point) and honestly, if I'm working a small, complex part, I don't mind sacrificing a $2 eBay carbide end mill, if the part created exhibits superior finish.

My servo system can do 120 IPM, but this seems insanely fast and it just gives me the creeps!
 

kvom

Administrator
Staff member
Administrator
Global Moderator
Joined
Jun 4, 2008
Messages
3,164
Reaction score
592
I played with your numbers a bit in G-Wizard. With such a low chip load your feed would drop significantly, and I imagine the finish would not be better if that rubbing dulled the cutter.

If finish is the concern I'd want separate roughing/finish passes.
 

MachineTom

Senior Member
HMEM Supporter
Joined
Oct 20, 2010
Messages
900
Reaction score
124
You have to be able to clear the chips, climb milling, recutting chips = poor finish, broken cutters.
 

dieselpilot

Well-Known Member
Joined
Jan 17, 2009
Messages
1,349
Reaction score
109
I use 2 flute endmills if at all possible. Though I have been doing a lot of work with 3 flute 1/8" tools. I feed pretty slow, never more than 20ipm. My RPM is probably a bit lower, near 20k, but I also never see more than 100W into my spindle. Last part I was cutting with 1/8" 3FL, .22" DOC, 25% step over, at only 7.5ipm in 6061. I never had much luck feeding faster than 20ipm, regardless of any other setting. But, I see now my spindle could have been the issue, and may have been loading only one cutting edge due to runout. I hope my new setup works better. Even so, tools don't seem to wear out. I break them before that happens. I usually only leave 0.2mm for the finish pass. Everything will be new again after I get the new spindle going, hopefully for the better.

Unless your acceleration rates are very high you'd probably never see 120ipm on a small part or short move anyhow. I can also do 120ipm, but have very mild accel, and I can see the machine reaching this limit at times during 3D surfacing at only 20ipm.

The vacuum is your friend. For a long job I clamp the shop vac hose to the table near the part. A small tip on the vacuum won't catch many chips. If you want to keep it small compressed air might be more effective.

Visualmill is fine, and I'm not really complaining. The only real problem I had with it, is their thread milling is incorrectly labeled and set up for multi point tools. It can't singlepoint. Once you figure out how each machining op works you can do quit a bit with VM. I often use parallel finishing to rough.

 

BobWarfield

Well-Known Member
Joined
Dec 27, 2007
Messages
1,151
Reaction score
1
Swede said:
I am using SFM = 1,000 for carbide end mills in 7075. This produces a 30,000 RPM for a 1/8" EM. Using a light feed load/tooth of 0.000,6 creates feed rates of about 90 and 45 for 4 and 2 flute cutters, respectively. If the tooth load is increased to more normal values like 0.001 and more, the feed rates skyrocket.

Let me ask a question - what harm would result from extremely low tooth loads like 0.000,2? I assume rubbing/dulling of cutters, but anything else? The surface finish should improve (to a point) and honestly, if I'm working a small, complex part, I don't mind sacrificing a $2 eBay carbide end mill, if the part created exhibits superior finish.

My servo system can do 120 IPM, but this seems insanely fast and it just gives me the creeps!
Howdy fellas, long time since I've been on this board. Not sure why I visited tonight, but glad I did. Maybe my ears were burning with these feeds and speeds questions, LOL.

The feeds and speeds you describe are probably okay. The onset of "rubbing" happens when the radius of your cutting edge is larger than the chipload. If you could look at the cutting edge with enough magnification, you'd see that even though it feels real sharp, it is rounded and has a radius. How much is that radius? Herein lies a problem: you don't know. HSS is sharper than carbide a bit. I go by the rule of thumb of 0.001" is fine for a chipload that won't rub (unless I'm using an insert intended for really tough work, some of those have bigger radii so the edges are tougher). For a smaller cutter, like you're 1/8", maybe 0.0005. Even smaller cutters can get by with less. You're within that range.

The challenge for you is to run with a lot of rpms without exceeding the feedrates your comfortable with and that your machine can cut accurately with. I'd use no more than 2 flutes, because the flutes multiply the feedrate. You can even by single flute cutters if you really want to back it down, but probably not the cheap ones you're enjoying from eBay.

The other thing is to keep the width of cut up to 1/2 the cutter diameter or a little more. The reason is radial chip thinning will make the effective chipload much less if you're taking light cuts. A lot of guys think if they take a light cut and really baby the feedrate they're taking it easy on the cutter. Not true. You're maximizing the rubbing which heats and rapidly dulls the cutter. You'll know when that's happening as your wear rate will go to pot.

G-Wizard will figure all that stuff out for you as kvom says. You can also check out my feeds and speeds cookbook to learn more about things like radial chip thinning and that rubbing:

http://www.cnccookbook.com/CCCNCMillFeedsSpeeds.htm

Cheers,

BW
 

Swede

Well-Known Member
Joined
Apr 7, 2011
Messages
460
Reaction score
9
Hey there Bob, good to hear from you. The "$2 eBay end mills" really were $2, but they are very high quality NOS carbide... got lucky and picked up a handfull for cheap. My HF spindle is a good one, and should be cutting evenly on all the flutes.

Chip clearance really is going to be a challenge for some of the projects I have in mind, and I need to work on getting some sort of system in place that works. I have a Trico micro-drop unit that is actually pretty nice for many machining operations, but is useless for clearing the chips that especially result from pocketing. I am going to try the as-suggested shop vac with a vinyl tube clamped into some sort of holder. The swarf that results from a 1/8" end mill at higher speeds is like fine glitter more than chip, for me at least. The stuff sprays all over the place, but would inevitably pack into work piece pockets and the cutter flutes themselves.

My spindle can take only 1/8" and 1/4" cutters unless I want to go metric and pick up some more collets, which are unfortunately over $100 each. I wish I could get a 3/16" collet, but they (KaVo) do not make them for this spindle. 3/16" would be a nice size for the work I am doing. Anyway, I picked up some nice 1/4" carbide roughers which should help a lot.

I've been machining manually for 25 years now, and I REALLY need to up my skill set with CNC, and CAD-CAM in general.
 

Latest posts

Group Builder
Top