Al. Speed, Feed, Depth of cut

[Rick Henrickson 65]

Ok I was told you can run a 3/4 carbide EM 2.25 flute length at 20000 rpm 550 ipm .25 depth of cut.

anyone doing this, I have always ran carbide at a max 0f 2500 SFM on AL witch would be 12733 rpm for the 3/4 and .008 per flute at .375 DOC

[somename75]

I am no expert, but that sounds pretty fast for that much flute length.

[Jerosu]

I think now SFM is only limited to your max RPM if you have the proper tools. The cut you refer to would sound reasonable to me depending on the rigidity of all the components and if you had enough torque and didn't try too much overlap.

[Walt R]

I am not sure about the rpm, but at my last job we made housings out of 5 and 6 inch thick MIC6 plate. Our Toyoda horizontals only had 12000 and 14000 rpm but I was using Ford 3/4 and 1.0 carbide end mills with a short flute length and relieved shank 4 inches out of the holder at .025 to .030 per tooth and a maximum depth of cut of .400. The depth was adjusted to devide evenly into the total depth. If I had more rpm I think I could have used it. By the way these end mills cost over 300.00 and every company selling carbide said they had a better tool but none of them could match this. More than one salesman tucked his tail and left with a broken end mill.

 

Walt

[Psychomill]

Rick, what type of tool geometry? To answer your question loosely,... Yes, you can cut like that. But you can't just use some arbitrary endmill. Also, depending on the tool, radial DOC will vary.

 

The numbers you were told is really not that extreme, but I do question it considering the flute length. As comparison, I do have a 3/4 em, 2.50 neck back running 22,000 rpm at 790ipm. Same tool in a different part is going 990ipm (shallower DOC). But as I said, its a neck back, not all flute (Dataflute HVM). As with Walt's post, you can hit high numbers with the right stuff.

 

As far as SFM, the sky is the limit provided you have good chip evacuation, gobs of coolant etc.

[Rick Henrickson 65]

that is almost exactly the tool I am using on the other op, it is a 3flute 1 inch loc releived 4.125 back in a haimen shrink fit.

[HevyMetl]

Watch the shrink fit in roughing applications. Your highend collets will help you dampen some of the vibration where the rigid shrink fit will translate it right up into your spindle. The shrinkfit is wonderful for finishing, but I would rough in a centerdraw collet from Haimer or Lyndex Nikken.

[MLS]

+1 Psycho

 

We run a 1.0 inch carbide in excess of 7000 SFM, but short LOC solid relieved shank...shrink fit...etc.

 

Lots of variables. We spent some time expirementing and found the limits...then backed off a bit. Heh

 

It has saved countless hours of machine time.

[Rick Henrickson 65]

it is a helical .75 dia 1" flute length 4.125 length below shank that is a 30 degree helix.

would a 45 deg helix be better and should I take it out of the shrink fit?

I moved the DOC to .175 from .25 it is ramping in at 3 degrees the step over is 75%

I broke the endmill at .25 DOC

it ramped in fine steped over and when it got back to the start of the ramp full .25 DOC it snapped off.

the first tool I rough 2.25 deep is also a helical 30 deg helix 3/4 2.25 flute and it worked pretty well though I think the 45 deg helix would have left a better finish.

[Rick Henrickson 65]

bump

[Psychomill]

One of two things could be happening. Maybe three...

1) 30 deg tools are a little more tempermental. You can run them at high speeds/feeds but you might have to play with it a little. 37 to 45 (even 50) are alot more forgiving, and can take a better beating. Just a "rule of thumb", not fact. Quite a few variables here too.

 

2) The tool data was exagerated by a sales guy. Not like that ever happens... If you're up to it, play with the DOC, both radial and axial to see what this tool "likes".

 

3) Programmed toolpath. In general pocketing routines, sharp cornered toolpaths cause your engagement to increase significantly. In many cases, with a large stepover, the corners are actually full diameter. So, its possible that the tool might take it ok in a linear or arc motion, just not at "slotting". To compensate, you can try Highfeed type toolpathing or feedrate adjustments to see if the tool will survive.

 

Basically you can try different things and settings to get the tool to overcome the problems. Then, you'll either like it cause you got it to work, or the cycle ends up being ridiculous and there are other tools that will work for you.

 

[Chris Rizzo]

Are you talking about "Helical" brand tools? If so, from my experiences with them, they suck. Specifically all sorts of galling and chip evacuation problems. A tool with a big wad of welded aluminum in the gullets sure will snap (which sounds like what may have happended to you). If I backed out the d.o.c. about 30-50% from my usual tool's paramaters (Destiny Diamond Back) they would not gall.

 

I told the salesman they should put that in their advertising campaign... "Reduce your d.o.c. by nearly 50%!!

 

The finishing tools are not so great either, imho.

[Bruce Caulley]

We run 45deg helix Garr and Iscar at 25000RPM and would go faster if we could. I was told by a tooling guro a while back that above 25000 37 degrees should be considered, below that 45 degrees is preferable.

 

Bruce

[Rick Henrickson 65]

thanks for all your help guys, Yes they are Helical brand I have never used them tell I came here. I have always used duramill AC45 with releived necks and they seem to be far better than these.

any more input would be great.

Colin do you use these helical brands?

[mtnflyr]

cascade,

I'm with Walt R on the M.A. Ford tools. We've been playing around with them for a couple of years. They seem to be limited only by our spindle speed. They last a long time as well. I've using some of the same endmills for those couple of years. Holding them in a milling chuck works the best for us.