Getting my Butt Kicked with Speeds & Feeds on 4140

LockTech · May 4, 2019

I'm looking for some guidance on speeds and feeds on 4140. I usually cut aluminum and brass so my knowledge cutting harder materials is very limited.

I'm currently using the following;

2in. 45 degree face mill 4 flutes with the following settings;
1400 RPM
733 Surface Speed
25 feed rate
.004 per tooth
Depth of cut .04

.75 End mill 4 flute with the following settings;
1145 RPM
225 Surface Speed
18 feed rate
.004 per tooth
Depth of Cut .5
.01 step over

.375 End Mill 4 Flute with the following settings;
2500 RPM
245 Surface Speed
20 feed rate
.002 per tooth
Depth of cut .04
Adaptive tool path .15 optimal load

Using flood coolant.
Using Climb on everything.
Haas Mini Mill 7.5
HP
I have experimented up and down from these settings with very little if any progress. Seems like no matter what I do, the machine sounds like crap and tips are breaking off the end mills.

Any help on this would be great before I am bald, haha

Thanks

Keith

HuFlungDung · May 4, 2019

Did you start at 1 sfpm and work your way up, or 1000 sfpm and work your way down?

Where did you get your starting data for working aluminum and brass?

huleo · May 4, 2019

Uh Haas mini with those size cutters in steel did not concern you?

LockTech · May 4, 2019

HuFlungDung said:
Did you start at 1 sfpm and work your way up, or 1000 sfpm and work your way down?

Where did you get your starting data for working aluminum and brass?

The data for brass and aluminum was from online calculators and forums, as was the data for the 4140.

LockTech · May 4, 2019

huleo said:
Uh Haas mini with those size cutters in steel did not concern you?

Actually, no it wasn't because the well under the tool weight and the load only gets up to 30ish %. Is your question referring to rigidity of the machine?

Hazzert · May 4, 2019

-Variable flutes with corner rads for roughing.

-Stop using a 3/4” in a minimill. They’re expensive and you probably don’t need it.

-I’d be spinning that 2” at 1000 rpm (500 sfm) and 8-10 thou per tooth

-Stop reducing your depth of cut and reduce your radial step over. A fully engaged tool is more rigid than one just working the tip.

-Your SFM is way off for HSM strategies, I would be starting 450-500 and increasing from there.

-A strong airblast may be a better option than flood coolant. If it’s a pissant stream you might be thermal shocking your tool and causing its premature edge failure.

-Are your feedrates and chiploads adjusted for radial chip thinning?

I think you need to take a look at HSM advisor or G-wizard. You’re doing a lot wrong and a proper piece of software would at least get you in the right area code rather than what you’re doing right now.

LockTech · May 4, 2019

Hazzert said:
-Variable flutes with corner rads for roughing.

-Stop using a 3/4” in a minimill. They’re expensive and you probably don’t need it.

-I’d be spinning that 2” at 1000 rpm (500 sfm) and 8-10 thou per tooth

-Stop reducing your depth of cut and reduce your radial step over. A fully engaged tool is more rigid than one just working the tip.

-Your SFM is way off for HSM strategies, I would be starting 450-50p and increasing from there.

-A strong airblast may be a better option than flood coolant. If it’s a pissant stream you might be thermal shocking your tool and cause it premature edge failure.

-Are your feedrates and chiploads adjusted for radial chip thinning?

I think you need to take a look at HSM advisor or G-wizard. You’re doing a lot wrong and a proper piece of software would at least get you in the right area code rather than what you’re doing right now.

Thanks for the info, I will definitely look into those two software programs. As for chip thinning, I'm not sure what it does or means.

I have seen a lot of people talking positively about the airblast, I will look into that as well.

I had been under the impression the bigger the bit the more rigidity it has so that is what made me go with the bigger is better mentality.

Hazzert · May 4, 2019

A bigger tool is more rigid but in your case you do not want the most rigid thing to be the tool...

For chip thinning

If you take a cut at exactly 50% stepover or more then the feed per tooth is as programmed. As you decrease the radial width of cut the actual chip thickness decreases because most of the advancement is happening outside of the material. What this means is that a .01 FPT at 50+% stepover might only be .003 at 10% and you are rubbing the material to death and need to increase the feedrate to compensate for the thinner chips.

When you watch a machining video where they are hauling ass it isn’t (always) because they have some monster machine or some amazing tool but are using a bit of math and science to their advantage.

LockTech · May 4, 2019

Hazzert said:
A bigger tool is more rigid but in your case you do not want the most rigid thing to be the tool...

For chip thinning

If you take a cut at exactly 50% stepover or more then the feed per tooth is as programmed. As you decrease the radial width of cut the actual chip thickness decreases because most of the advancement is happening outside of the material. What this means is that a .01 FPT at 50+% stepover might only be .003 at 10% and you are rubbing the material to death and need to increase the feedrate to compensate for the thinner chips.

When you watch a machining video where they are hauling ass it isn’t (always) because they have some monster machine or some amazing tool but are using a bit of math and science to their advantage.

For someone who is self taught which which program would you recommend? Also is one more advanced than the other?

Hazzert · May 4, 2019

LockTech said:
For someone who is self taught which which program would you recommend? Also is one more advanced than the other?

Both have free versions or trials, take a look at both and see which that you prefer. I have a seat of G-Wizard and it works for the few things I do with it.

Generic Default · May 4, 2019

LockTech,

Use 1/2" carbide AlTiN coated endmills and run them dry or with air blast if you can. Use the full depth of cut of the endmill when possible, and keep your radial step over at 0.05" (10%) for general purpose stuff, this number seems to work every time. With AlTiN the speed limit is above what your spindle can do. Watch this video, action starts around 1:20 into it.

YouTube

DMF_TomB · May 4, 2019

the most important factors
1) length tool sticking out of tool holder
2) length of tool holder
.
speeds feeds depth width of cut are adjusted for longer tools and holders. what is rigid on softer metal can easily be not rigid enough for harder metals. the machinability rating on aluminum is 2.0 to 6.0 cubic inches per minute per hp
4140 depending on heat treatment closer to 0.4 to 0.8, basically cutting forces are like 500% to 1500% more cutting forces
.....if i have a 4" dia mill thats 25.0" gage length obviously its limits are different than a 5" gage length tool

Hillside Fab · May 4, 2019

For 28-32Rc 4140, I generally use same DOC and FPT as mild steel, but cut the SFM by ~1/2, and work up a bit from there (SFM only).

Not sure if that will help, since you only listed experience with aluminum and brass. I tend to not get or go after much of that work.

Hazzert · May 4, 2019

DMF_TomB said:
the most important factors
1) length tool sticking out of tool holder
2) length of tool holder
.
speeds feeds depth width of cut are adjusted for longer tools and holders. what is rigid on softer metal can easily be not rigid enough for harder metals. the machinability rating on aluminum is 2.0 to 6.0 cubic inches per minute per hp
4140 depending on heat treatment closer to 0.4 to 0.8, basically cutting forces are like 500% to 1500% more cutting forces
.....if i have a 4" dia mill thats 25.0" gage length obviously its limits are different than a 5" gage length tool

Damnit Tom, his minimill would comfortably fit on the table of your machine.

Hillside Fab · May 4, 2019

Hazzert said:
Damnit Tom, his minimill would comfortably fit on the table of your machine.

lol probably a bakers dozen would

Ox · May 5, 2019

^^^ LOL!

As for the coolant issue...

10 yrs ago I was dooing a lot of roughing on 4140 with the 2" 45* face mill like in this thread, and I tried it with and without coolant with a cpl of different inserts, and I saw no tool life differences at all. All I got was hot parts/chips/tool with chips/fines all over the table - AND all around the mouth of the spindle taper - that the coolant would have worshed away or kept under control for me otherwise.

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

Think Snow Eh!
Ox

G00 Proto · May 5, 2019

Another thing to consider with the minimill style of tool, is that it is a belt drive with a rinky dink spindle motor (still my favorite machine). As such, it is my opinion that aggressive cutting in 4140 or any of the stainless steels cause the belt to slip minutely and cause the chug chug noise that you are probably hearing. I have a bad habit of dropping the radial stepover and increasing the RPMs to get around this. I always take the max depth of cut that the cutter and part will allow, and adjust the radial to get the spindle load and noise that I want. Shallow depths of cut just cause my cutters to wear faster in that area. As a matter of opinion, I feel that the deeper depth of cut with shallower radial depth of cut results in less heat being conveyed to the cutter and results in far superior tool life/ metal removed.

I would hate to think how many tons of 4140, O1 and Titanium I have machined on those poor little Haas MiniMills. Get the cutting conditions down to where it isn't making objectional noise and they will run and run like the Energizer bunny.

LockTech · May 5, 2019

Hazzert said:
Damnit Tom, his minimill would comfortably fit on the table of your machine.

lol, now thats funny.

litlerob1 · May 5, 2019

I love it when the solution to F&S is HSM and air. :skep:

Posting videos of Titan Gilroy's strategies is basically nullifying. Proven out 50x before it's recorded. Sponsored by KM and DMGM, imagine if he posted a fuck up, with their Tools! Ze Germans would weinen viel.

R

Hazzert · May 5, 2019

litlerob1 said:
I love it when the solution to F&S is HSM and air. Posting videos of Titan Gilroy's strategies is basically nullifying. Proven out 50x before it's recorded. Sponsored by KM and DMGM, imagine if he posted a fuck up, with their Tools! Ze Germans would weinen viel.

R

It gets even better. He posted a video of roughing with a 3 in Kennametal shouldermill and bragged that he was going to get it up to 800ipm. His initial setting were .1 DoC and 2.1 or something stepover and the machine stalled out at 600 “IPM”. His solution was to cut the stepover to 1.5” and increase the feedrate to 800 IPM giving him a MRR that was achieved at his original parameters back at 450IPM...

Getting my Butt Kicked with Speeds & Feeds on 4140

Plastic

Diamond

Hot Rolled

Plastic

Plastic

Stainless

Plastic

Stainless

Plastic

Stainless

Aluminum

Diamond

Cast Iron

Stainless

Cast Iron

Diamond

Hot Rolled

Plastic

Diamond

Stainless

Similar threads