Breaking 1/2" Kennametal HARVI I TE ENDMILL while plunging

tome9999 · Sep 4, 2021

I have a 1/2" Kennametal HARVI I TE endmill in a live tool position on an Emco 365MC lathe. I am short on positions/holders in the turret so want to use this endmill to plunge (i.e., drill) the end of a 4140 part before boring an id. Kennametal has a video demo of the tool showing it plunge/drill 4140 at 1.5D (1.5" deep). They give F&S as 590 SFM, 4500 RPM, .002 IPT. (video is here: HARVI™ I TE - The Magic Solid End Mill From Kennametal - YouTube)

My turret live tools max out at 4000 RPM so 0.002 IPT (4 flute) at 4000 rpm is 32 IPM. Which is 0.008" IPR.

I set my F&S to 3000 RPM, 0.006 IPR (thought I was being a little conservative) and plunged in to a depth of 0.25" with coolant on. Seemed to be going ok at the start but about 1/8" in the endmill stalled. I immediately hit reset (stop) backed the EM out and see I broke two flutes off the end of the endmill. Not really sure why this was a problem or what F&S I should be using?

-Tom

Finegrain · Sep 4, 2021

Those Kennametal parameters seem pretty "Magical" indeed, in 4140. Not saying it can't be done, but I do think everything has to be totally squared away -- toolholding, workholding, everything.

Live tool isn't the most rigid, AFAIK, so there is one problem.

Coolant may be hurting you -- the thermal shock may cause microchipping which leads to macrochipping. The demo shows the tool doing this dry, maybe try that?

BTW, "1.5D" doesn't mean 1.5" deep, it means 1.5 times the diameter, so 3/4".

Regards.

Mike

tome9999 · Sep 4, 2021

Finegrain said:
Those Kennametal parameters seem pretty "Magical" indeed, in 4140. Not saying it can't be done, but I do think everything has to be totally squared away -- toolholding, workholding, everything.

Live tool isn't the most rigid, AFAIK, so there is one problem.

Coolant may be hurting you -- the thermal shock may cause microchipping which leads to macrochipping. The demo shows the tool doing this dry, maybe try that?

So for a live tool that isn't as rigid as one might like does slowing the feed rate help compensate? I don't want to rub either so I am always hesitant to go slow but not sure where the transition is between cutting and rubbing...

Hmm, I suppose coolant causing the failure is possible, but I don't think I want to wager a another tool on that fixing the problem!

Finegrain said:
BTW, "1.5D" doesn't mean 1.5" deep, it means 1.5 times the diameter, so 3/4".

Regards.

Mike

Yes, you are right, thanks for that correction.
-Tom

CarbideBob · Sep 4, 2021

Video is a VMC. How much HP in your live tool?

D Nelson · Sep 4, 2021

Sometimes when you watch videos like that your bullshit meters pegs out. You know that shit is not possible but maybe 1 time and the next time in it’s toast but hey it was in the video.
Don

Sent from my iPhone using Tapatalk Pro

Fancuku · Sep 4, 2021

You can't treat the live tool of a lathe as if it is the same as milling in a VMC. It's nowhere close. I am not surprised that the spindle stalled with a 1/2" endmill trying to just plunge 3/4" in 4140.

tome9999 · Sep 4, 2021

CarbideBob said:
Video is a VMC. How much HP in your live tool?

I believe the live tool is 9 HP.
-Tom

Nagol · Sep 4, 2021

Why not try some helical interpolation using the C axis? Make a bigger hole or use a smaller tool to make the hole. You should be able to ramp at 10-15 degrees if the machine can handle it. Endmills are much better at making holes this way than drilling.

tome9999 · Sep 4, 2021

Nagol said:
Why not try some helical interpolation using the C axis? Make a bigger hole or use a smaller tool to make the hole. You should be able to ramp at 10-15 degrees if the machine can handle it. Endmills are much better at making holes this way than drilling.

That is plan B. But the endmill is supposed to be able to do this. Perhaps the machine cannot, but I’d like to get it to work if possible….

Nagol · Sep 4, 2021

Even if you get it to do it tool life would most likely be better interpolating. At the least a lot of pecking may be in order.

Nerdlinger · Sep 5, 2021

How does the first 1/8” look? Is it all chattery? Maybe do another one only going .100” into it so you can examine the part to see what the surface finish looks like. If it’s all chattery and ugly you know rigidity is a problem. How big is the part and how far is it sticking out? What are you holding the 1/2” em in? ER20?

Good luck!

tome9999 · Sep 5, 2021

Nerdlinger said:
How does the first 1/8” look? Is it all chattery? Maybe do another one only going .100” into it so you can examine the part to see what the surface finish looks like. If it’s all chattery and ugly you know rigidity is a problem. How big is the part and how far is it sticking out? What are you holding the 1/2” em in? ER20?

Good luck!

I’ll look at it more closely today but it looked pretty good while I was picking out the carbide chips. The part is a 3” dia, 3” lg round and is sticking out only about an inch. The live holder uses a ER25 collet.
-Tom

tome9999 · Sep 5, 2021

Attached are some images of the hole and setup. Surface finish isn't great but I don't see signs of horrible chatter...

tome9999 · Sep 5, 2021

After talking with pcasanova (who has the same machine) and looking at the machine specs I am pretty sure the problem I encountered is the torque limit on the VDI-30 live tool holders in my machine. The spindle on the live tools is 9HP but it is torque limited so as to not break the gearing/spindles that drive the tool holders. The specs say the Torque is only 12 lb-ft. For the main spindle it is 141 lb-ft! If you crash a live tool a clutch disengages (done that a couple times). I think I was able to hit reset when I saw the endmill stall just before the clutch let go.

I suspect I will need to slow my feed and/or ramp/spiral the hole to keep the torque down.

-Tom

Fancuku · Sep 5, 2021

Any reason why you are not using an insert drill for that hole?

MaxPrairie · Sep 5, 2021

Why not drill and bore with an indexable drill? Those videos are always done on a 50 taper and probably switch the endmill out after every cut.

tome9999 · Sep 5, 2021

Fancuku said:
Any reason why you are not using an insert drill for that hole?

Two reasons. I don’t have one :-) , and I only have so many tool positions and live toolholders. I was hoping to have an endmill do double duty…..
-Tom

Fancuku · Sep 5, 2021

MaxPrairie said:
Those videos are always done on a 50 taper and probably switch the endmill out after every cut.

Too many people have watched the Titans of CNC videos on youtube and think that his bullshit is real.

D Nelson · Sep 5, 2021

Put a tool block on the turret that holds 2 drill bits and go to town
Don

Sent from my iPhone using Tapatalk Pro

D Nelson · Sep 5, 2021

here you go like this
Don

Sent from my iPhone using Tapatalk Pro

Breaking 1/2" Kennametal HARVI I TE ENDMILL while plunging

Aluminum

Diamond

Aluminum

Diamond

Stainless

Cast Iron

Aluminum

Aluminum

Aluminum

Aluminum

Stainless

Aluminum

Aluminum

Aluminum

Cast Iron

Hot Rolled

Aluminum

Cast Iron

Stainless

Stainless

Similar threads