Using up 3/4 inch carbide endmills too quick

RustyRedneck · Jun 29, 2017

Hey guys, I'm having a little trouble getting more life out my 3/4 inch carbide endmills. I only get to use them about twice before they need to be resharpened. Granted each time is on a 6 to 8 foot brake that I mill. I only have it running at .1 Z depth and it only fully engaged on each part for 200 to 300 inches at about .050 depth. The rest of it is side milling maybe .05. I'm cutting 1145 steel and my endmills are solid carbide. I'm using flood coolant, spinning the endmills at 1790 RPM, and feeding at 30 IPM. This next time I'll try it at 20 IPM. What am I doing wrong? Thanks!

Finegrain · Jun 29, 2017

Sounds like you are using your endmill like a facemill, if it's only .05" deep and 100% engagement. I would try an inserted facemill instead. You can tune the inserts for the material and conditions, and inserts are cheap compared to 3/4" carbide.

If not that, how about stubby 1/2" endmills? You need more passes, but cutters are much cheaper.

Regards.

Mike

Bobw · Jun 29, 2017

What am I doing wrong?

350sfm, is the steel hardened or no???

I'm going to say that your problem is that you are running coolant.
That thermal shock thing..

From too much experimenting, I've found that (at least for me), the break point
from wet to dry is about 300sfm in mild steel.. Lower for harder materials.

Are you coated???

That dark purple stuff gets slicker than snot and hard as hell when it gets HOT!!!
If you are running coolant, you may not be generating a high enough temp to let the
coating work its magic.

Mtndew · Jun 29, 2017

Bobw said:
350sfm, is the steel hardened or no???

I'm going to say that your problem is that you are running coolant.
That thermal shock thing..

From too much experimenting, I've found that (at least for me), the break point
from wet to dry is about 300sfm in mild steel.. Lower for harder materials.

Are you coated???

That dark purple stuff gets slicker than snot and hard as hell when it gets HOT!!!
If you are running coolant, you may not be generating a high enough temp to let the
coating work its magic.

This would be my suggestion as well.
Cut it dry.
And maybe use an indexable shoulder mill for the .100" depth cut.
OR
Or get an endmill with a larger corner radius.

Dan from Oakland · Jun 29, 2017

that's a chip load of .004 on a 4 flute tool and about 350FPM. You don't mention the failure mode of the end mill- wear or chipping or? Is this a coated tool or?? My guess is its thermal shock from your coolant but that's only 1 possibility. I have had good luck with coated tools and an air blast in steel. Blue chips are a good indicator of getting the heat out in the chip and that's a combo of RPM and chip load. Have you consulted the tool manufacturer?

charlie gary · Jun 29, 2017

How is your part fixtured? If it's allowed to bounce around it's going to beat the crap out of your cutter.

RustyRedneck · Jun 29, 2017

The endmills are not coated. The Steel is not hardened. I'm running 350 SFM. The endmills are wearing down on the corner and then starting to chip. I'm roughing out the pocket with a 1.5 inch carbide inserted cutter and going back in and finishing with the 3/4 inch. I'm using endmills with a sharp corner to get the 90 degree edge in the pocket. I don't have air blast capabilities at the moment. The chips are coming off with no color change. I'm running a vertical mill so if I run without coolant the chips should fall away. I'll probably try cutting it without coolant this next time. The part weighs about 800 pounds and is fixtured vertically. I've got it hanging pretty solid. I'll probably try it without coolant next. Thanks for the tips!

zero_divide · Jun 29, 2017

Like others have said.

1) It is not aluminum, so even carbide will wear. If you don't want to wear off the tip, use indexed endmill for facing operations. ALso ditch coolant.

--OR--

1) Use coated carbide.
2) Ditch Coolant

charlie gary · Jun 29, 2017

RustyRedneck said:
The endmills are not coated. The Steel is not hardened. I'm running 350 SFM. The endmills are wearing down on the corner and then starting to chip. I'm roughing out the pocket with a 1.5 inch carbide inserted cutter and going back in and finishing with the 3/4 inch. I'm using endmills with a sharp corner to get the 90 degree edge in the pocket. I don't have air blast capabilities at the moment. The chips are coming off with no color change. I'm running a vertical mill so if I run without coolant the chips should fall away. I'll probably try cutting it without coolant this next time. The part weighs about 800 pounds and is fixtured vertically. I've got it hanging pretty solid. I'll probably try it without coolant next. Thanks for the tips!

In that case it might be more economical to rough with a 3/4" cutter with either radiused or chamfered corners and then come back in with a smaller sharp corner cutter.

DMF_TomB · Jun 30, 2017

RustyRedneck said:
Hey guys, I'm having a little trouble getting more life out my 3/4 inch carbide endmills. I only get to use them about twice before they need to be resharpened. Granted each time is on a 6 to 8 foot brake that I mill. I only have it running at .1 Z depth and it only fully engaged on each part for 200 to 300 inches at about .050 depth. The rest of it is side milling maybe .05. I'm cutting 1145 steel and my endmills are solid carbide. I'm using flood coolant, spinning the endmills at 1790 RPM, and feeding at 30 IPM. This next time I'll try it at 20 IPM. What am I doing wrong? Thanks!

.
usually measure tool life in minutes with 60 minutes often considered normal tool life.
.
tool length and tool holder length can effect cutting parameters easily 100 to 1000% . normally its best to try different cutting parameters and record data. tool life, amount milled, surface finish, any sudden tool failures, normal wear or failure mode.
.
like any scientist you try experiments and record data. then decide on whats better to do.

RustyRedneck · Jul 17, 2017

While I was gone the boss ordered a 3/4 inch inserted endmill and it showed up other day. Programmed for it and away we go. Seems to be working well so far. may have eliminated the carbide endmill from this process.

deadlykitten · Jul 17, 2017

hy / a bit late, but :

... try not changing directions inside the material; improve the toolpath if possible
... check the dwells ?
... plunge @ corners

... what holder is it ?

check for variants for the tool corner : radius, chamfer, sharp

check if the new tool has bigger corner radius ?

RustyRedneck said:
I'm using endmills with a sharp corner to get the 90 degree edge in the pocket

here you are ... finishing tools are better to be carbide integral than with inserts / if you will have problems with the new tool with inserts, consider a smaller integral one

be sure that, when cutting the walls, tool is not cutting @ bottom

Search

Largest Manufacturing Technology Community on the Web

Search

Using up 3/4 inch carbide endmills too quick

RustyRedneck

Aluminum

Finegrain

Diamond

Bobw

Diamond

Mtndew

Diamond

Dan from Oakland

Titanium

charlie gary

Stainless

RustyRedneck

Aluminum

zero_divide

Stainless

charlie gary

Stainless

DMF_TomB

Diamond

RustyRedneck

Aluminum

deadlykitten

Banned

Similar threads