What's new
What's new

1/8" Roughing End Mill?

dalt.deuel

New member
Hey guys (and gals) I am cutting 4140 Steel 28 Rockwell C-Scale Hardness. Unfortunately I have to use an 1/8" EM for roughing and to no surprise I am having a lot of trouble breaking End Mills.

I am curious as to what style End Mill I should be using?

Currently I am using a:

GARR Carbide 4-Flute 1/8" SQ x 1/2 F/L *TiALN*

My gut is telling me this is 100% the wrong type of End Mill to be using.

I was thinking something more along the lines of

Carbide 2 Flute (or 3 Flute) 1/8" .030 Rad x 1/2 F/L (Not sure coating matter?)


My DOC is .020" with S7500 F3. (Max RPM for my Haas) the pocket I am running is .180". The tool will break mid-cut, also sometimes right when it makes contact with the steel, it varies. Some tooling will last for 15 parts and other tooling breaks on the first tool.

I have slowed it to a F3. from F7. b/c I continue to break the tool.


Anything helps!

P.S. I am getting ample amount of coolant on the tool!
 

D Nelson

New member
How deep are you going? Is it a pocket ? Are you using dynamic tool paths?
Don


Sent from my iPhone using Tapatalk Pro
 

litlerob1

New member
You don't want square corners for sure. But you've slowed down to .0001" chipload!!!! That's the problem, you're re-cutting tiny chips. Make a chip, .002". Your SFM is okay if you're making a chip, but you aren't. So either the RPM needs to come waay down, or Feeds need to go up.

I wouldn't use a 1/2" LOC on an 1/8" Endmill that's for Roughing-ever. Use a 1/4" LOC.

R
 

Mike1974

Active member
it is a pocket, and the pocket depth is .180". and I don't know if it is using dynamic tool paths??

Dynamic toolpaths will generally be long lines of code, full depth, light radial stepovers (10% or so). I would helix into the pocket, than use a dynamic pocketing type path. What software are you using? Need a little more inof. Also, get a 3/16" or 1/4" LOC tool, that will go a long ways in reducing breakage.

Something like this
https://www.mscdirect.com/product/details/44194603
 

Mtndew

Active member
Currently I am using a:

GARR Carbide 4-Flute 1/8" SQ x 1/2 F/L *TiALN*

My gut is telling me this is 100% the wrong type of End Mill to be using.

I was thinking something more along the lines of

Carbide 2 Flute (or 3 Flute) 1/8" .030 Rad x 1/2 F/L (Not sure coating matter?)


My DOC is .020" with S7500 F3. (Max RPM for my Haas) the pocket I am running is .180". The tool will break mid-cut, also sometimes right when it makes contact with the steel, it varies. Some tooling will last for 15 parts and other tooling breaks on the first tool.
WHICH Garr end mill are you using?
.02 d.o.c. and you're busting them? Something isn't right then.
How much of the tool is hanging out from your holder?
Is it running concentric?
What kind of toolpath are you doing?
How deep is the pocket?
What radius is in the pocket corners, is the end mill is just ramming into the corners... they don't like that. Can you program a radius larger than the end mill?

Garr does make a high feed end mill that small, I've used them a few times no issue.

Here is Garr end mill I would suggest:
GARR TOOL - Product Details
 

dalt.deuel

New member
should I change to a 2 or 3 flute with a .030 rad? typically what I run an 1/8" EM 4FL is S3361 F6.7 should I go back to that S and F? we have our sister company programming these tools down in Illinois and I have been proofing it out and it has NOT been good.
 

D Nelson

New member
If it was dynamic it would be all the way down and running sweeping moves climb milling only with probably a 7 percent step over. No problem to cut
Don


Sent from my iPhone using Tapatalk Pro
 

Milland

Active member
From this line Z-Carb HPR | Series Z5 | KYOCERA SGS Precision Tools chose a four flute stub (1/4" length of cut) endmill, and get their recommendations for speed and feed to start. Don't use 1/2" LOC if you're just going .180" deep.

Rough out material (and give yourself a starting point) using a screw machine length cobalt drill. Make sure the drill stays sharp, replace before it dulls. If you must plunge in with the carbide endmill, using a shallow helix to spiral in, at least 1.5 hole diameter to endmill diameter.

Ask SGS whether you'll be better off with an air blast over coolant. Sometimes air will help the coatings to function the way they're designed to, when coolant keeps the temps too low.
 

dalt.deuel

New member
we are using dynamic toolpaths. the code is super long. Would you recommend a 2 or 3 flute with radius for the roughing?
 

Larry Dickman

Active member
I'd say your flute length is your biggest problem. Way too long. Also, your DOC sucks. You're just wearing the corners off the tool. You don't know if you're using dynamic roughing? How do you not know? Go full depth with high speed roughing, 10% stepover. Garr are good tools, but you might want to try Imco for that.
 

litlerob1

New member
I'd say your flute length is your biggest problem. Way too long. Also, your DOC sucks. You're just wearing the corners off the tool. You don't know if you're using dynamic roughing? How do you not know? Go full depth with high speed roughing, 10% stepover. Garr are good tools, but you might want to try Imco for that.

Someone else is generating code for him.
 

litlerob1

New member
OP, I would take every recommendation thus far. You'll have a better time at it. If it's a huge pain to get a new program, just affect your feeds and speeds at the control, until it's proven out.

Mtndew asked a good question..."how far is the Endmill hanging out of the Holder"?

Also how are you holding an 1/8" Endmill?

R
 

G00 Proto

New member
You need to have this reprogrammed. Do a dynamic toolpath with .180" depth of cut. I would start at 12% radial stepover. Your RPMs may still be to high depending on the 4140's mood that day. My guess is I would be around 6000 RPM and 12 inches a minute.

Your tool is only part of the problem. .020" depth of cut leaves no where for the heat to go expect the corners of the tool. A corner radius will help, but the program is the issue.

1/4" length of cut endmill will also help with the chatter that could be killing your endmills.
 

dalt.deuel

New member
My tool is only hanging out of the collet about .550" practically as short as I can get the stickout without tightening on the flutes (obviously b/c the flutes are 1/2). I just ran up to a local tool supplier and I have gotten 2 Flute 1/8 End Mills on my lunch break. I am not trying to be vague in my post. I do not have the option to just rewrite the program, unfortunately. I appreciate you trying to help me out and the others that are trying to help me out. With that said, this is what I am going to try:

S3361 F3.5 using 2FL 1/8" .015 Radius. I did not see the post about Flute length being to long until I got back from lunch. Do these speeds and feeds seem acceptable to you Rob? Thanks in advance. I am at the mercy of our sister company, this is how they program and these are their parts that need to get finished ASAP. Like you said, all I can really do is change the speeds and feeds without manually writing and editing code that is a mile long.
 








 
Top