the truth about high speed machining

[jwvica01]

Haas literature touts cutting feeds up to 500ipm but this seems impossible to attain accept with the simplest of toolpaths or programs designed specifically to demonstrate high speed machining, rarely applicable to "real" parts.

Realistically the upper limit for smooth finishing seems to be around 100-150 ipm in my experience.

What is the truth about the max speed attainable with finish 3D toolpaths with small straight line segments on the order of .001" - .010" line lenght?

Are there other machines/manufacturers that can attain this finish speed with a different processor or look ahead algorithm, or is this purely a function of programming?

I am talking about finish 3D contouring with like .0002" cusp height, not high speed roughing which I have been able to attain much higher feeds.

Thanks

[ktm666]

other machines can feed much faster than the haas and still whip the haas' surface finish. nothing about the haas machine is consisant enough for glorious finishes at high feeds. dont get me wrong, the haas is a fine machine, and capable of nice finishes. a good machinist can make excellent finishes, other machines can just do it faster.

500ipm finishes on a haas is just a pipe dream.

[impact]

ktm666 speaks the truth.

Keep in mind finishing speeds are generally slower than your roughing speeds....

Were you hoping for just a little more?
What sort of tooling are you running? You may want to look into shrink fit or other super holding, low run-out tooling, collets don't quite cut it at those speeds.

I have a Matsuura ra-2g at work with HSM and a 20,000 rpm hydraulic spindle. Running 3 Flute high helix angle CGS cutters in shrink fit holders. It hauls out material :P

[Donkey Hotey]

High Speed Machining and surface finish are going to be as limited by the spindle RPM as anything else.

My largest attempt at surface contouring was the 4x5 contoured foot. I generated a waterline finish path in Mastercam. The path ran circles around the part, at changing Z values. I think this run was 10K RPM, 0.010" stepover and 0.002 chip load.

If you look closely at the highlight, you'll notice the actual facets Mastercam generated to represent the surface. The problem is that because I used linear conversion of the contours, the motions ended up being line segments in the finished part and the file was huge (600K for just this small part).


I've since learned that Mastercam can do G02/G03 conversion to the cutter paths (instead of G01 linear moves). Basically, it looks at the points and tries to run longer arc segments though the same points, within a tolerance you specify. Instead of thousands of tiny line segments, you end up with fewer arc motions, strung through the same points. It allows for much more rapid execution in the control, reduces the file size and creates a better finish.

I should note that in both cases, the marks were able to be removed with light, wet-sanding (320-400 grit). They're more visible than they felt. A pre-sand and a few hours in a tumbler removed all of the marks, leaving a nice matte finish.

The reason I share this is: the success or failure of the paths is as dependent on the CAM system you use and how you use it. I was limited by my spindle RPM and desired chip load (0.002x2 flutesx10K=40 IPM) but my choice of surface interpolation also dramatically affected the quality of the part.

I should also add that I did override the feed on a few of them. I ran the machine as high as 300 IPM. It was impressive to watch but the chip load at that speed was 0.015". Even with a 0.010" stepover, they looked bad enough, that I ran the rest at the lower speed. Without a 30K spindle, I don't know how much 'high speed machining' you can really accomplish.

[Geof]

Originally Posted by Donkey Hotey ...I was limited by my spindle RPM and desired chip load (0.002x10K=20 IPM)....

How many flutes? Your calculation implies 0.001 per tooth for two flute and 0.0005 for four flute; that is a very low chip load. Did you try anything between 20 and 300, they are very widely separated limits.

[Donkey Hotey]

I'm sorry, Geof, ya' caught me (I wondered why that sounded low).

It was 40 IPM, two-flute, 1/4" ball mill. I'll edit my post so the math works.

Yes, as I increased the chip load, the surface deteriorated. I did one experiment where I would let it run a few laps, then I'd bump the feed by 50%. It created bands around the part that I could compare. It was noticeable. I was hoping to find a sweet spot but it seemed like a linear relationship between speed and finish.

[Astonlee]

Like all thing size matters, and yes it you are manufacturing small parts, a few inches square, the very high feed rates like you mention are feasible, couple with 40/50,000 rpm spindles etc.
However the other thing you need with high-speed machining is cast-iron for rigidity, the right control with good look-ahead, and good programming software like Powermill from Delcam.
As I have done 100’s of high-speed machining trials on all types of materials, what you quickly learn is not to waste your time & tools on the cheaper type of machine centres.

[dertsap]

the hass proscess speed is slow for a modern machine , ive found it to be comparable to old mori's i've run , most of my programming is hand coded but the other day i was creating a funky toolpath which needed to be processed in cam , the short line segments kept the machine at a very low feedrate because it couldn t process the code quick enough and it was so clunky in the motion that i had to pull the program and resort to another alternative
I like the hass and they are a good machine but they still need work if they are ever to be up to snuff with japanese machines

[Donkey Hotey]

Originally Posted by dertsap the hass proscess speed is slow for a modern machine , ive found it to be comparable to old mori's i've run

How old is the Haas? Did it have the HSM option?

[Geof]

Originally Posted by Donkey Hotey ....It was 40 IPM, two-flute, 1/4" ball mill. I'll edit my post so the math works....

Okay 'nother question. But first an admission; I am considering getting into using Mastercam....only considering it!!! and it would not be me, more correctly I am planning ahead for future products that may not be easily programmed by hand; it is your brain getting picked this time.

Why such a small cutter and why two-flute? Your cusp height depends on your ball nose radius and step over, your feed rate depends on chipload, number of teeth and rpm. With a large diameter ball nose you could maintain the same cusp height at a larger step over, and with four flutes you can double the feed for the same rpm. Go to a 1/2" four flute at 0.02 stepover and you should divide the machining time by 4 and still get the same finish???

[Donkey Hotey]

Geof, you are having exactly the same thoughts I had. I started out trying to use a 3/4" ballmill for exactly the reason you're citing: cusp height. I reasoned that unless I had a concave area, that had a smaller radius than the cutter, bigger should be better.

In practice, it didn't quite work out that way. I'm not sure why. I got much better surface finishes with the little 1/4" endmill. I even tried 1/2" to split the difference. In the end, I roughed with a 1/2" ball, then finished with the 1/4".

Admittedly, I'm sure that better or different cutters might improve things dramatically. I had to get the job done so I did the experimenting with what I had on hand.

In any case, if this is for end-item products, it's still a slow process and will tie your machine up for longer cycle times than basic profiling tools will. It may also present you some part finishing challenges (same issue I had: getting the cusps down to where they could be removed by tumble finishing).

Edit: I forgot one other thing. I used two-flute because of chip clearance. The tip of a two-flute, ball-nose endmill has greatly reduced clearance. Four-flute are even worse. Aluminum would just pack up in that small area and eventually weld itself to the edge. Two-flutes still had a chance to get the chips out. Now that I type this, that might also have been the problem with the larger radius endmills. There was almost nowhere for the chips to go, down in the cutting zone.

[dertsap]

Originally Posted by Donkey Hotey How old is the Haas? Did it have the HSM option?

its a fairly new machine
no it doesn t have the option but neither did the old mori's i was comparing to , ive worked with many types of machines and i was genuinely surprised , id say the fastest it was moving was 50 ipm , I'm not complaining but i was surprised