Need Better Finish with Long Endmill

rbinmt · Aug 16, 2018

In need of suggestions. Here is what I am dealing with:

Material: 4140 Steel
Tooling: 1.50" 6FL HSS Endmill with 8.0LOC
Depth of Cut: 7.8" (Must all be finished in one pass to avoid any steps)
Machining Parameters (Finish Pass): 70SFM (180RPM) .004 Chipload (4.3 IPM) .01 Left for Finish Pass
Problem: Chatter

The workpiece is clamped with the maxiumum amount of rigidity possible (I'd call it moderate rigidity). I have tried anywhere from 50SFM to 120 SFM and 70 seems to give me the best finish. I have also tried adjusting the chipload and .004 seems to be the best.I have tried leaving anywhere from .005-.03 for the finish pass with no notable differences (currently leaving .01). I am currently performing one spring pass and it seems to help, but still getting more chatter than is acceptable. Any suggestions?

Bobw · Aug 16, 2018

How are you holding the endmill?

What machine is it?

Have you checked your tool retention lately??

One trick I've used successfully on occasion. Leave more stock down at the bottom..
My pet theory on why this works, it gives the endmill something to do so that it
doesn't have the opportunity to bounce around..

Another trick that can help break up your harmonics, grind a big ass chamfer on a flute or
2.. I'd probably go with 2 since its a 6 fluter, and NOT opposite of each other..

Milland · Aug 16, 2018

Costly is to get the boss to spring for a carbide finish cutter, that's ONLY used for this final pass. Make sure it's a variable helix, variable pitch tool, may have to be custom ground. Five or seven flute, not an even number.

Easy is to program in some variable for RPM, to knock down vibrations from constant feeds/speeds.

You can try contacting BlueSwarf (BlueSwarf - Home) to see if they think their technology can help minimize vibration, can't tell you how much the testing will cost.

rbinmt · Aug 16, 2018

Bobw said:
How are you holding the endmill?

What machine is it?

Have you checked your tool retention lately??

One trick I've used successfully on occasion. Leave more stock down at the bottom..
My pet theory on why this works, it gives the endmill something to do so that it
doesn't have the opportunity to bounce around..

Another trick that can help break up your harmonics, grind a big ass chamfer on a flute or
2.. I'd probably go with 2 since its a 6 fluter, and NOT opposite of each other..

Bobw,

Thanks for the suggestions. We are currently holding the endmill in a 1-1/4" set screw style endmill CAT40 holder. We don't really have the equipment to check tool retention, but we do some pretty good hogging and it seems to handle that fine. Is there a trick to checking tool retention without an actual gage?

Grinding the flutes is an interesting idea. My boss might flip out if he saw me grinding on the endmill though! We are only using the 6FL endmill because it was the most cost effective endmill that we found in our searching.

rbinmt · Aug 16, 2018

Milland said:
Costly is to get the boss to spring for a carbide finish cutter, that's ONLY used for this final pass. Make sure it's a variable helix, variable pitch tool, may have to be custom ground. Five or seven flute, not an even number.

Easy is to program in some variable for RPM, to knock down vibrations from constant feeds/speeds.

You can try contacting BlueSwarf (BlueSwarf - Home) to see if they think their technology can help minimize vibration, can't tell you how much the testing will cost.

Milland,

Thanks for the reply. I'll try the variable RPM trick. I mentioned carbide to the boss and he is convinced that we can get an acceptable finish with the HSS. We work on a pretty tight budget here. I'd better try a little longer before approaching him with higher cost options.

Milland · Aug 16, 2018

This might be an application where a collet is better than set screw holder. It should improve damping a little bit, and the forces should be low enough that it won't pull out. And you can rotate the tool for best TIR, not really possible with a set screw holder.

I'd check the taper on the toolholder and machine spindle for signs of fretting or wear, just to be sure that's not an instigator of movement. And you can Qick-N-Durty the drawbar tension by trying to pry on the gap between spindle face and toolholder flange with a big screwdriver, should take some real effort to move.

40 taper is pretty marginal for the size of cutter you're using, is this a Haas or something with some mass behind it?

rbinmt · Aug 16, 2018

Milland said:
This might be an application where a collet is better than set screw holder. It should improve damping a little bit, and the forces should be low enough that it won't pull out. And you can rotate the tool for best TIR, not really possible with a set screw holder.

I'd check the taper on the toolholder and machine spindle for signs of fretting or wear, just to be sure that's not an instigator of movement. And you can Qick-N-Durty the drawbar tension by trying to pry on the gap between spindle face and toolholder flange with a big screwdriver, should take some real effort to move.

40 taper is pretty marginal for the size of cutter you're using, is this a Haas or something with some mass behind it?

We don't have a collet holder big enough for the 1-1/4" shank, but I will definitely cost one out. The taper looks good and I don't get any movement at all with a screwdriver pry so I think we're good there.

We are using a Doosan Horizontal mill for this. I have been really impressed with its rigidity to this point. We actually have a 50 taper Doosan that I would love to use, but it is loaded up (6 pallets) on aluminum jobs that we run and the boss doesn't want to put any steel jobs on it which is understandable.

litlerob1 · Aug 16, 2018

General rule of thumb for overhang ratio is; 4:1 Steel, 6:1 Carbide, 10:1 De-vibe you are in the Carbide category. Obviously you can push that, I believe you can get through the part with the Tool you have, but it isn't going to be easy.

Per Bob; keep enough material on the Floor to keep the Endmill from just bouncing around, keep enough material on the Walls to keep it from just pushing away, Feed it hard enough that the Tool is biting into the cut. It's sometimes a lot of trial and error to find the sweet spot.

Sounds like you'll get there. Run an Indicator on the Bore of your Endmill holder, and check Bore size, you might find a better one of the same design. Check the Taper of the Holder and the cleanliness of the the Machines Taper. Don't let the boss see you grinding on the bloody thing!!! Just do it anyway

.

Bottomline is, you are not going to get a 32 finish with that Tool. But I have seen some pretty fine Finishes while programming steps and undercuts. Imperceptible to the common eye.

R

Larry Dickman · Aug 16, 2018

You could also try a reverse helix end mill. Your application is what they were invented for.

Matt@RFR · Aug 16, 2018

rbinmt said:
Grinding the flutes is an interesting idea. My boss might flip out if he saw me grinding on the endmill though! We are only using the 6FL endmill because it was the most cost effective endmill that we found in our searching.

"Cost effective" or "Cheap"? If you have done a week of testing with unacceptable results and you make $20/hr (let alone all the overhead you burned up, scrapped material, etc.), you could have damn near paid for a $1,000 carbide endmill, let alone actually making parts you can charge for and not falling behind on this and other jobs. "Cheap" usually equals "Stupid" in the long run.

Also, have you put thought to changing your setup? Without seeing the part it's impossible for anyone to make suggestions, but maybe flip the thing on its side and use a facemill?

I want to commend you on your opening post. For a guy with 4 posts here, you gave us nearly every detail needed to start a real discussion, clearly and concisely, and with good spelling and grammar on follow up posts. This is much, much better than a lot of the members here (new or otherwise) and is appreciated.

Ox · Aug 16, 2018

I have questions for the answers given:

I'm not following how even or odd flutes makes a difference.
How does the machine know?

How would a carbide tool help if he's only got a 40 taper behind it?
I am skeered to even guess at the stick-out on this sucker! :eek:

I trust that there aint no 50 tapers in the shop?
The concensus here seems to be that this is taxing for a 40 taper, but in 4140 it would seem to be well over the top to me.
???

A chamfered (broken?) corner likely could help.
Generally this is a self adjustment that the tool does on it's own to show us how it works.

On a tight CNC, I have had very good luck with taking passes in Z w/o leaving witness lines.
And if you doo git a slight witness, you could likely scotchbrite it away?

-------------------------

I'll put a few Miss Pell's in there for the police...

Ox

Milland · Aug 16, 2018

Ox said:
I have questions for the answers given:

I'm not following how even or odd flutes makes a difference.
How does the machine know?

http://www.conicalendmills.com/wp-content/uploads/2014/12/Performance.compressed.pdf

Page 33 claims "Odd number of flutes reduce harmonics by staggering the entry and exit of the cutting edges" But with a cut this long it may not be a factor.

How would a carbide tool help if he's only got a 40 taper behind it?
I am skeered to even guess at the stick-out on this sucker!

Eh, there's Haas 40 taper, and then there's Okuma or other better/heavier 40 taper. I have some 40 taper spindles here (just spindles, not entire machines) that are roughly three times the size and weight of Haas spindles, thereby lowering the stiffness limitations to just the taper. And a good 40 taper mate with a ~2K lb drawbar force is going to be pretty solid.

Ox · Aug 16, 2018

Milland said:
http://www.conicalendmills.com/wp-content/uploads/2014/12/Performance.compressed.pdf

Page 33 claims "Odd number of flutes reduce harmonics by staggering the entry and exit of the cutting edges" But with a cut this long it may not be a factor.

So you are just running with this claim?
This is not something that you have qualified yourself?

I understand variable flute, and I have had good luck with variable speeds on large diameter lathe parts, but I doubt that this feature/tool is large enough here to have much luck with variable speeds.

60* and 90* incr are bad, but a tooth every 72* or 120* is somehow different?
I'd need to hear personal testimonies on that.
Otherwise - I'm thinkin' it to be more of a sales gimmick.

At least a 50 taper holder can swallow the shank and likely stick out 3" less!
(plus being 2wice the machine)
Of course that doesn't help the part any if that is what is singing...

-----------------------

Think Snow Eh!
Ox

thermite · Aug 16, 2018

Ox said:
So you are just running with this claim?
This is not something that you have qualified yourself?

Odd-count was a huge blessing on reamers where there was a wall all around to push-off of and directly-opposed even-count wanted to chatter, lobe, both, or ugly-worse.

I can't see it making a damn on an endmill once working but the one side, nothing but AIR to push-off opposite, no.

And Oh, BTW .. pulling damned near 8" with an HSS endmill, Weldon holder, in 4XXX on 40-taper ass?

Pilgrim, that ain't complaining.

You be bragging to get away with that s**t at all!

BSCustoms · Aug 17, 2018

You might also consider plunge surfacing it with a neck relieved cutter or back relieved cutter. End mills are more forgiving when loading the Z in high L

ratios. Plunge, move along contour, plunge, etc. Its a little slower but works quite well without spring for the right tooling.

CarbideBob · Aug 17, 2018

Ox said:
I have questions for the answers given:

I'm not following how even or odd flutes makes a difference.
How does the machine know?......

Ox

It doesn't make a difference but works as good myth of odd number, breaks things up. Zip real world math behind it.
Yet any geometry change means different things to different cuts so sometimes it works better.
I sort of cringe and bite my tongue when a customer brings it up.
Bob

Milland · Aug 17, 2018

Buncha cynics. I just have to change from a four flute to a seven flute endmill and the machine cuts a thousand times faster. Angstrom tolerances and mirror polish, too.

OK, you've made your point - no magic to odd number cutters. Got it...

Milland · Aug 17, 2018

So, Bob - now that we have that done and dusted, what would you suggest to help this gentleman in his distress?

Greg White · Aug 17, 2018

leave .005 fur fin., 75 rpm, .004 pur flute feed.
good luck.
fuk da police.
Gw

maxime_qc · Aug 17, 2018

when its possible i put a damper on the part like a quick grip clamp save my ass many times . but not a great option for big production

Need Better Finish with Long Endmill

Plastic

Diamond

Diamond

Plastic

Plastic

Diamond

Plastic

Diamond

Titanium

Titanium

Diamond

Diamond

Diamond

Diamond

Cast Iron

Diamond

Diamond

Diamond

Titanium

Plastic

Similar threads