What's new
What's new

Machining with long endmills

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
I seem to run into quite a bit of parts with longish tooling necessary, but never have much luck with it. For instance, right now I'm using a Helical 82856 in 6061. .375", 3" flute length, 45 degree endmill. MAP says .020" WOC, 15K rpm, and .0029ipt. HSM Advisor says .005" WOC, 15K rpm, .0045ipt. Realistically though, I always end up with my SFM on the floor. Then I see Youtube videos and stuff, and they're moving at speeds similar to what I posted. So what gives? What could I be doing wrong? I'm almost always using high quality holders on a very new, high end machine, and all I seem to get at those speeds is chatter and vibrations.
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
For a given diameter, deflection increases with the third or fourth power of length, I forget which. So:

1. Minimize stickout as much as possible, every little bit shorter helps.
2. Cut partway down with a shorter cutter, it will be faster and more rigid.
3. Use "extended" cutters for the deep sections, with a short flute length and a solid, relieved section. They're significantly more rigid than a long flute length cutter. You can skim the upper wall with the extended cutter to blend if needed.
4. Put that extended cutter in the most rigid holder you can get. I like shrink fit, others prefer sidelock. No ER holders for this application.
 

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
I usually use SK holders, for this I'd have probably used an SK16. Would I be better to use a sidelock? Hydraulic? Milling Chuck?

Also, for an instance when that L/D tool IS necessary, are those recommend speeds and feeds just a pipe dream? Or is there something else to that?
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
I usually use SK holders, for this I'd have probably used an SK16. Would I be better to use a sidelock? Hydraulic? Milling Chuck?

Also, for an instance when that L/D tool IS necessary, are those recommend speeds and feeds just a pipe dream? Or is there something else to that?

SK should be better than ER, but I'd still prefer a shrink fit or sidelock. Hydraulics are good for finishing, but not as rigid for roughing. Milling chucks can be ok, but they often have more gauge length than other solutions, and a short holder length is almost as important as cutter stickout.

I've run a 3/8" Helical extended endmill in 17-4 H900, sticking out 4" from a shrink fit, in a VF-3SS. The MAP numbers were a good starting point, and I tweaked it a bit to find an anti-harmonic point. It wasn't fast, but it worked.

Edit:
You don't need an induction machine top dabble in shrink fits. Heat it with a MAPP gas torch, rotating it in your hand to heat it evenly. Pop in the tool (I use a shaft collar to set the length) and let it cool.
 

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
I should have mentioned, this is a Cat50 dual contact machine, which I would THINK helps with the negatives of gage length to some extent, since even a milling chuck is less than an inch shorter than a 3/8 sidelock holder. That being said, if cost weren't an option, and shrink wasn't available, would you still prefer a side lock over hydraulic, milling chuck, or VC collets?
 

Ianagos

Stainless
Joined
Sep 23, 2014
Location
Atlanta
Can you use reduced neck tooling? Instead of a 3” long flute for a 1/2 or 3/4 flute with a long neck?
 

13engines

Hot Rolled
Joined
Jun 30, 2015
Location
Saint Paul
You might try smaller helix angles. The smaller the angle the stiffer the tool. Sounds like you have a machine that will take them as stiff as they get.

My last experience that I can think of with this long tool concept was in acetyl plastic. (1/2 X 2LOC) Semi-roughing with a 37 degree 3fl Accupro played nice. No problems at all. The 45 degree YG 3fl Alu-Power would have none of it. (Was fine for finishing.) Same holder, same everything. This was on an older YGM Supermax and ER collets, but my point is that it was an apples to apples comparison. Although sometimes results like this can also be attributed to the relief angles of the cutter.
 

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
Can you use reduced neck tooling? Instead of a 3” long flute for a 1/2 or 3/4 flute with a long neck?

You might try smaller helix angles. The smaller the angle the stiffer the tool. Sounds like you have a machine that will take them as stiff as they get.

My last experience that I can think of with this long tool concept was in acetyl plastic. (1/2 X 2LOC) Semi-roughing with a 37 degree 3fl Accupro played nice. No problems at all. The 45 degree YG 3fl Alu-Power would have none of it. (Was fine for finishing.) Same holder, same everything. This was on an older YGM Supermax and ER collets, but my point is that it was an apples to apples comparison. Although sometimes results like this can also be attributed to the relief angles of the cutter.

This is in fact, a finishing operation. And I've honestly never had much luck finishing a wall at multiple z depths without getting steps in the finish. Maybe there's a trick to that too, lol. I've got lots of tricks to learn. :D:eek:
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
I seem to run into quite a bit of parts with longish tooling necessary, but never have much luck with it. For instance, right now I'm using a Helical 82856 in 6061. .375", 3" flute length, 45 degree endmill. MAP says .020" WOC, 15K rpm, and .0029ipt. HSM Advisor says .005" WOC, 15K rpm, .0045ipt. Realistically though, I always end up with my SFM on the floor. Then I see Youtube videos and stuff, and they're moving at speeds similar to what I posted. So what gives? What could I be doing wrong? I'm almost always using high quality holders on a very new, high end machine, and all I seem to get at those speeds is chatter and vibrations.
Way too fast on the rpm's for that long of a d.o.c.
Slow it down to about 5k rpm, using the same ipt and it should cut a lot better.
Since you asked, yes I would use a hydraulic if you can since this is for finishing.
HSM Advisor only gives you numbers based on the "default manufacturer" speeds and feeds that you give it (on the right hand side). If you give it high values as a default it will take those into consideration when calculating the HSM speeds and feeds. You have to find the sweet spot, it just takes a little trial and error on your part.
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
What is the Stickout?
If you are getting chatter finishing walls, the only solution often us to reduce the RPM on the machine until it goes away.
 

Orange Vise

Stainless
Joined
Feb 10, 2012
Location
California
This is in fact, a finishing operation. And I've honestly never had much luck finishing a wall at multiple z depths without getting steps in the finish. Maybe there's a trick to that too, lol. I've got lots of tricks to learn. :D:eek:

Your Z depth passes should be significantly less than the flute length of the cutter. For example, even if the cutter has an .875 flute length, I'd program a Z-stepover to 0.250-0.375. If you program Z-stepover to 0.8125, for instance, you're going to get steps. The idea is that each pass is cleaning up the previous two passes. This is with a reduced shanked cutter.

Yes, it's going to cost you cycle time, but you end up with a nicely finished wall with virtually no taper and no chatter.
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
I should have mentioned, this is a Cat50 dual contact machine, which I would THINK helps with the negatives of gage length to some extent, since even a milling chuck is less than an inch shorter than a 3/8 sidelock holder. That being said, if cost weren't an option, and shrink wasn't available, would you still prefer a side lock over hydraulic, milling chuck, or VC collets?

Yes, I'd still prefer sidelock. A quality sidelock, torqued to spec, will be nicely concentric and very rigid. But IMO shrink is better. Hydraulics can be about as good as a shrink fit for finishing cuts only.

Why is a shrink fit holder not an option? It's a lot cheaper than a milling chuck or hydraulic, and as I said above, you don't need an induction machine for occasional use.

More on the subject:
milling chuck VS sidelock
 

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
Yes, I'd still prefer sidelock. A quality sidelock, torqued to spec, will be nicely concentric and very rigid. But IMO shrink is better. Hydraulics can be about as good as a shrink fit for finishing cuts only.

Why is a shrink fit holder not an option? It's a lot cheaper than a milling chuck or hydraulic, and as I said above, you don't need an induction machine for occasional use.

More on the subject:
milling chuck VS sidelock

The company has recently gotten more "corporate" and management wouldn't accept using a torch to change tools (though I see nothing wrong with it) and our tooling sales guy has mgmt pretty much convinced that using a torch for shrink fit destroys the holders, which I'm aware, isn't an issue with common sense.

Your Z depth passes should be significantly less than the flute length of the cutter. For example, even if the cutter has an .875 flute length, I'd program a Z-stepover to 0.250-0.375. If you program Z-stepover to 0.8125, for instance, you're going to get steps. The idea is that each pass is cleaning up the previous two passes. This is with a reduced shanked cutter.

Yes, it's going to cost you cycle time, but you end up with a nicely finished wall with virtually no taper and no chatter.

I've always done less than the flute length, but not by that much. I've usually used, maybe 75% of the length, so I'll definitely try your suggestion.

What is the Stickout?
If you are getting chatter finishing walls, the only solution often us to reduce the RPM on the machine until it goes away.

Just beyond the flutes, so about 3.125"

Way too fast on the rpm's for that long of a d.o.c.
Slow it down to about 5k rpm, using the same ipt and it should cut a lot better.

Yes, that's what I usually end up doing. It just seems that suggestions, and demos I see are always way beyond that, so I thought maybe I'm missing something.
 

CarbideBob

Diamond
Joined
Jan 14, 2007
Location
Flushing/Flint, Michigan
You might try smaller helix angles. The smaller the angle the stiffer the tool. Sounds like you have a machine that will take them as stiff as they get.

^This^
Not so much that they are stiffer but the entrance/exit times of the top and the bottom of tool change when you are going deep with different helixes.
Sync this wrong and not so good things happen.
Sometimes a higher helix will work better. I did not model your cut so unsure if this applies or not.
Seems mysterious and related to why deep cutting endmills squeal if forced into a corner.
All the fancy holders or stiff machines in the world will not help if the basics ignored.
All of this bandaids, some of them tight enough so they work and people swear by them.
Perhaps it is easier to spend money rather than understand a cutting tool.
Then you can brag to all others about how much your machine, spindle joint, holders and tools cost and be so proud. This is everywhere.
Know what I see walking into this sort of shop? Keep my mouth shut and do not try to explain.
The customer is always, always right.
Bob
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
The company has recently gotten more "corporate" and management wouldn't accept using a torch to change tools (though I see nothing wrong with it) and our tooling sales guy has mgmt pretty much convinced that using a torch for shrink fit destroys the holders, which I'm aware, isn't an issue with common sense.

Well if torches are out, the next step up is this:

Induction Heat Machine for Shrink Fit Tools MariTool

Was $3500 when I got one, price has gone up.
 

MCritchley

Hot Rolled
Joined
Mar 22, 2007
Location
Milwaukee
I am currently in the same boat, deep pocket with a .125 corner radius. My solution was to get a custom .210" dia cutter with a very short flute length and reduced shank for max rigidity. I started with the recommended 12k rpm and slowed it down to 25% of that and finally got a great finish. For a holder I am using a Nikken SK-16 that has less than .0004 run out 1.4" from the nose of the tool. It took a bit of messing around to dial it in and am living with a pocket that takes 25 minutes to finish.
The old saying of just slow your revs down is still very pertinent in a modern 3 axis machine
 

JBethell

Aluminum
Joined
Jun 12, 2009
Location
Clearwater, FL
^This^
Not so much that they are stiffer but the entrance/exit times of the top and the bottom of tool change when you are going deep with different helixes.
Sync this wrong and not so good things happen.
Sometimes a higher helix will work better. I did not model your cut so unsure if this applies or not.
Seems mysterious and related to why deep cutting endmills squeal if forced into a corner.
All the fancy holders or stiff machines in the world will not help if the basics ignored.
All of this bandaids, some of them tight enough so they work and people swear by them.
Perhaps it is easier to spend money rather than understand a cutting tool.
Then you can brag to all others about how much your machine, spindle joint, holders and tools cost and be so proud. This is everywhere.
Know what I see walking into this sort of shop? Keep my mouth shut and do not try to explain.
The customer is always, always right.
Bob
Could you explain what you mean by modeling the cut? What are you looking for to compare helix angles?
 

CarbideBob

Diamond
Joined
Jan 14, 2007
Location
Flushing/Flint, Michigan
Could you explain what you mean by modeling the cut? What are you looking for to compare helix angles?


When one gets deep the bottom tip load and exit and the upper end are different points in a rev.
This makes for deflection or bending in the tool, more at bottom and less at top but that not the big deal.
Done wrong the top releases at a bad point so the bottom bites more than it should so whoppie chatter.
This is way over simplified.
 

Luke.kerbey

Cast Iron
Joined
Mar 2, 2019
Speed, speed, speed, turn it down. It’s the single most important factor to reduce vibration and chatter. Then turn your feed up to compensate.
 








 
Top