New video of Super Minimill Cutting 600+IPM

[MKproto]

THought you guys might like to see what you can do with a minimill and a little RPM.. Tool load was almost a perfect constant at 60%.

YouTube - Test cutting
new VM2 coming in a few weeks to help this machine keep up with work flow.

[Donkey Hotey]

So you're obviously using some variation of constant step-over toolpath. What kind of cutter, flutes, RPM, step-over and feed rate are you using?

By my math, that's gotta' be a 4-flute, running at 10K and around 0.015 per tooth. The only way that would seem to work at that depth of cut would be due to chip thinning with a shallow step-over. Any more and I'd expect it to be howling like crazy.

How close am I?

[Delw]

I am betting the RPm is 15k+

those cuts looked pretty close to around .025-.030 step over by the size of the chip coming off.
My 3/8" 3 fluter from GARR( for aluminum) wiil do that at 250 ipm up to .050 step over, at 12k with no noise, I havent tried it more than that it might work at more.?

Delw

[Delw]

Oh I just saw a post with the details

Originally Posted by MKproto Well Here it is guys this is the video I was telling you about. YouTube - Test cutting 3/8"-5 FLute accupro Endmill Iscar ER-32 Collet chuck and Collet 6061t-651 Aluminum Machined on a 2004 Haas SUperminimill with the 15k RPM spindle and HSM. Programming took about 5mins. (added below) Feed rate was set to a max off 634 IPM, tool never comes out of part. Corner rounding on the machine is set to .0002" G187 is set to finishing. Spindle speed 14,900 RPM DOC .700" Chip load was set to .0035" Enjoy.

[Donkey Hotey]

Well, by that math, the feed is 260 IPM. No slouch but, not 600 IPM either. I'd also question if the machine is actually getting anywhere near any of those speeds with all the direction changing going on. It takes some time to get up to speed and I'd bet it would be in constant acceleration with those kinds of moves.

I'm not knocking the process...just trying to understand the real results. I'm tempted to try a similar method on a part I have to make today.

[Delw]

Originally Posted by Donkey Hotey Well, by that math, the feed is 260 IPM. No slouch but, not 600 IPM either. I'd also question if the machine is actually getting anywhere near any of those speeds with all the direction changing going on. It takes some time to get up to speed and I'd bet it would be in constant acceleration with those kinds of moves. I'm not knocking the process...just trying to understand the real results. I'm tempted to try a similar method on a part I have to make today.

I know what you mean , that small of part things look faster than they actually are to begin with. it does look cooler than crap, I would love to see what the face of that part looks like cause at that speed its definatly not flat and has steps from tool flex especially on a mini mill.
I think I am going to order one of those aluminum 5 fluters next week just to see what I can do with it.
My machine on alum will scream loud with anything that isnt a alum cutting endmill in any flute number and give a crappy finish, no matter what speeds and feeds I plug into it

Delw

[cygnus x-1]

Notice it says "...Feed rate was set to a max off 634 IPM". So the feed rate probably varies depending on chipload. At least that's what it looks like to me. It's damn cool whatever it is. I would really like to know what cam program that was done with.


C|

[Delw]

Solidcam I machining I think.
click on his name and view Posts

its definatly bad ass

[pit202]

It is a volumill or truemill strategy , see it on YT :

YouTube - Swift Carb RampMill with Truemill Cutter Path - Heavy ramping, helical entry

[MKproto]

It was programmed in Solidcam 2011 with I-Machining. I dont know every little bit about it yet, but basically some chips are heavier, and some thininer. Step overs vary, and it calculats the best path. Just about everything is taken into account. Machine Horspower, spindle speed, max feed rate of machine etc. Feed rate can vary wildly depending on tool engagement. The one part is the engagement angle is almost constant which is why they machine is not making wierd crazy noises. I will get a picture of the part tomorrow and you can see some of the facets on the base to show you have the tools path varies step overs etc.

[MKproto]

When the new machine comes in and is up and running (2010 Haas VM2 12k, HSM etc) I will see what the 1/2" 5fl can do with more power. The minimill is a tinker toy in comparison. I would like to run it on a mikron, or a liner motor machine for faster dymanic transients, and a 24-40 k spindle..

[MBG]

Just curious, why do you need anything over 15k? My place I work at doesn't have anything over 15k and that is hauling..