Solid Carbide or Inserts?

Nerdlinger · Dec 3, 2015

I need to mill a .562" wide slot about .813" deep in .875" thick annealed 4140. I want to use something like a .500" wide mill going through the center at .25" depth of cut (so four Z moves), which leaves about .031" on each wall for a finish cut. Should I use an indexible cutter or solid carbide end mill? Is it just a matter of what's cheaper? I imagine inserts would pay for themselves pretty quickly over $50 solid carbide cutters...

PHDesigns · Dec 3, 2015

Not sure what's out there for that small indexable. I do use a K-Tool at times. For that job I think a solid carbide end mill would be the way to go.

Hazzert · Dec 3, 2015

I'd use a 3/8" solid carbide, full depth of cut with HSM. Most of the 1/2" indexables are single flute and a waste of time IMO.

Nerdlinger · Dec 3, 2015

You're probably right...I'll have to look at the Iscar catalog tomorrow but maybe only a one or two insert holder...

Trevor34 · Dec 3, 2015

I second Hazzert. 3/8" solid carbide at full depth.

Nerdlinger · Dec 3, 2015

Hazzert said:
I'd use a 3/8" solid carbide, full depth of cut with HSM. Most of the 1/2" indexables are single flute and a waste of time IMO.

I would, too, but the machine I have is a '96 VF2 with only 7500 RPM and no HSM option (at least not activated) so I've got to keep the tool path very basic.

dstryr · Dec 3, 2015

How many do you have to do?
I'd try to full slot it with a 1/2 to utilize the whole cutter since your machine is older and will take 10x longer to trichodial cut it with a 3/8. 4 flute for chip clearance.

If you are worried about it go 2x. I think going 4 depths is overkill.

You could also look into a solid carbide feed mill and take small depths and high feed (your machine should be fine since its a straight line).
They are a lot more than $50 4fl 1/2 though.

nofxz · Dec 3, 2015

Sandvik released the 390 with a 7mm insert height. 2 flute 3/8s or 2 or 3 flute 1/2s. I have had good luck using HSM and 390 tools.
So 3 depths cuts with a 7mm insert.

Hertz · Dec 4, 2015

You can get mills like this from Iscar. ISCAR Cutting Tools - Metal Working Tools - MM S-A (stepped shanks) : 3102476 - MM S-A-L3.50-C.500-T08
Here's my opinion. If you are using a solid carbide endmill, do not take multiple z depths. Waste of time and waste of flutes. You'll only wear out the bottom of the endmill. I can't believe people still mill this way with endmills.
The link I put above is for those times you are hard up to run multiple depths. The tips are replaceable. Use that type of tool for multiple depths, use a solid carbide for full depth.
Use small WOC's, higher RPM, higher IPT. If you need a pilot hole, use a drill. They are the fastest metal removal tools. If you helix down, it's slower and again you wear out the bottom of the tool quicker. What are you using for programming?

Hertz · Dec 4, 2015

Nerdlinger said:
I would, too, but the machine I have is a '96 VF2 with only 7500 RPM and no HSM option (at least not activated) so I've got to keep the tool path very basic.

Your machine does not need to have a HSM option. You make the machine move in that type of toolpath with your code you feed it. 7500 RPM is plenty RPM for 4140.

Mtndew · Dec 4, 2015

Hertz said:
Your machine does not need to have a HSM option. You make the machine move in that type of toolpath with your code you feed it. 7500 RPM is plenty RPM for 4140.

This
You don't need to go 400ipm in order to do a hsm path.
It's all in HOW it cuts.
Use a 3/8 endmill and make some chips!

Slippery Panda · Dec 4, 2015

Iscar makes indexable solid carbide endmills with multiple flutes and thru coolant. I would also recommend going 3/8"

Solid Carbide & MULTI-MASTER

Big B · Dec 4, 2015

.813 deep with a 3/8 end mill seems like a little much. I would use a 1/2" solid carbide end mill. Flex shouldn't be a problem with .030 on a side for cleanup. Use air blast to evacuate the chips if you have it.

Hertz · Dec 4, 2015

Big B said:
.813 deep with a 3/8 end mill seems like a little much. I would use a 1/2" solid carbide end mill. Flex shouldn't be a problem with .030 on a side for cleanup. Use air blast to evacuate the chips if you have it.

That's the point. If the flutes are there, it's not too much. Adjust width, speed and feed to suit. Bury the cutter, otherwise there is no point in using that endmill. If the endmill only has 1/2 or 3/4 of flute length, then that's a different story.

Orange Vise · Dec 4, 2015

Big B said:
.813 deep with a 3/8 end mill seems like a little much. I would use a 1/2" solid carbide end mill. Flex shouldn't be a problem with .030 on a side for cleanup. Use air blast to evacuate the chips if you have it.

For an HSM path (trochoidal-style entry) at 5-10% stepover, anything up to 3xD is typically quite reliable.

A 1/2" EM won't work well in a .562 HSM slotting toolpath because it'll only have .062 of available movement, less with cleanup allowance, hence the recommendation for the 3/8 EM.

Orange Vise · Dec 4, 2015

Nerdlinger said:
I need to mill a .562" wide slot about .813" deep in .875" thick annealed 4140. I want to use something like a .500" wide mill going through the center at .25" depth of cut (so four Z moves), which leaves about .031" on each wall for a finish cut. Should I use an indexible cutter or solid carbide end mill? Is it just a matter of what's cheaper? I imagine inserts would pay for themselves pretty quickly over $50 solid carbide cutters...

Solid carbide tends to me more practical for most applications under 1" diameter. The exception would be deep, narrow pocketing operations with 5/8 and 3/4 indexable feedmills.

m98custom1212 · Dec 4, 2015

Nerdlinger said:
I need to mill a .562" wide slot about .813" deep in .875" thick annealed 4140. I want to use something like a .500" wide mill going through the center at .25" depth of cut (so four Z moves), which leaves about .031" on each wall for a finish cut. Should I use an indexible cutter or solid carbide end mill? Is it just a matter of what's cheaper? I imagine inserts would pay for themselves pretty quickly over $50 solid carbide cutters...

I use to think that way also biggest cuter possible and using z steps..

Use 3/8 Endmill and HSM style toolpath you will be amazed

DMF_TomB · Dec 4, 2015

Nerdlinger said:
I need to mill a .562" wide slot about .813" deep in .875" thick annealed 4140. I want to use something like a .500" wide mill going through the center at .25" depth of cut (so four Z moves), which leaves about .031" on each wall for a finish cut. Should I use an indexible cutter or solid carbide end mill? Is it just a matter of what's cheaper? I imagine inserts would pay for themselves pretty quickly over $50 solid carbide cutters...

.
a 1.0" dia 3" flute carbide end mill is over $300. sure even with resharpening cost savings when size get above a certain point inserts are cheaper and usually can run at higher sfpm or higher metal removal rate.
.
i often use a 3.0" dia carbide insert mill at over 12" long. they do not make solid end mills that big obviously costs too much. i believe even a 2.0" dia hss roughing end mill with 10" long flutes is over $1000.
.
tooling decision is usually also based on length of cut and length of cutter and tool holder combination. many horizontal mills and 5 axis mills need longer length to reach different part sections

dstryr · Dec 4, 2015

DMF_TomB said:
.
a 1.0" dia 3" flute carbide end mill is over $300. sure even with resharpening cost savings when size get above a certain point inserts are cheaper and usually can run at higher sfpm or higher metal removal rate.
.
i often use a 3.0" dia carbide insert mill at over 12" long. they do not make solid end mills that big obviously costs too much. i believe even a 2.0" dia hss roughing end mill with 10" long flutes is over $1000.
.
tooling decision is usually also based on length of cut and length of cutter and tool holder combination. many horizontal mills and 5 axis mills need longer length to reach different part sections

do you know how to read??

Atomkinder · Dec 4, 2015

Another vote for 3/8" and HSM toolpaths. Our 3/8" generic 4-flute AlTiN cutters (Redline) have just about an inch of flute length, and it's save my ass a couple times in this sort of application exactly.

DMF_TomB said:
.
a 1.0" dia 3" flute carbide end mill is over $300. <snip>

What does this have to do with the OP's question, Tom?

Solid Carbide or Inserts?

Stainless

Hot Rolled

Stainless

Stainless

Plastic

Stainless

Diamond

Aluminum

Stainless

Stainless

Diamond

Aluminum

Diamond

Stainless

Titanium

Titanium

Stainless

Diamond

Diamond

Titanium

Similar threads