Iscar H490 vs T490 vs apkt1505

Anyone have any experience with Iscar's line of H490 and T490 facemills?

I'm looking to try to get work to buy one for me, either the -09 (.335 tall) or -12 (.538 tall) inserts.

Most of the sqare corner facemills we have are either apkt 1505 or 1003 inserts, and they seem to not do as well as I'd like, performance wise. (Comparing it to Iscars OFCR octogon inserts, tool life is poor).

Anyway, currently I'm running a job out of 304 stainless, and am attacking it with a feedmill like this, 808 grade inserts.

This feedmill works very well for us cutting flame cut 4140. Great tool life, etc. But this 304 is chewing it up. Have tried 350-500sfm, .023 per tooth, .065 deep. Sounds great, until it doesn't. Glad this machine has a spindle load monitor lol.

I'll slow it down even further after I write this, but this experience has me wanting to use a regular facemill, and skip the high feed. 2 inch facemill taking a wide pass at a decent depth of cut is now what I think would be better for this application. (I'm milling a boss that sticks up 2.7" tall, about 1.5" diameter near one end of a 2x4" stainless block)


So, does anyone have experience with either T490 or H490 tools? Even better if you have experience with both. I'd like to know which one seems to perform better in materials like this. And I don't wish to try 1505s on this job.


H490 Facemill

T490 Facemill

The H490 will give you the option of using a high feed insert or the standard inserts. I Have both and use both in 304 / 316 / 17-4 and in carbon steels as well as aluminum for the T490 with the aluminum inserts.

Ive nver try the iscar line bit we use the seco square 6 and with the f40m insert they perform well in ss 304. They also have 6 corner intead of 4 might worth to take a look.

Can you also share the result if you happen to buy one of those.

Use them a lot. They are awesome cutters if you have the balls to push them.
2" Iscar H490 hogging - YouTube
3" Iscar H490 Hogging. - YouTube
51 rc milling - YouTube
Iscar 6" facemill - YouTube

These videos are all the H490 line of cutters.

Hertz said:

Use them a lot. They are awesome cutters if you have the balls to push them.

Click to expand...

This machine certainly has the balls to push them (and I'd gladly grow a larger pair myself once I get the cutters), Makino A88. I think it has a 40HP spindle and is stout as hell.

I've seen your videos many times, great stuff. Its what inspired me to want the H490s in the first place. Then I saw the T490s and was wondering which is better....



I saw that the H490s have feedmill-type inserts, so possibly a plus for that. But the T490s seem to have "rougher" style inserts, and they look to be ground like a standard solid roughing endmill would be. I don't see that option for the H490s?

Can you get me the exact item description on the H600 feedmill insert that you are using? I saw that you are using IC808 but is it "T" or "HP" edge prep?

For 304 stainless, you want to use the "HP" edge prep. I suspect that is the reason why you are wasting inserts on that material.

If you decide to go the route of the T490 in that material, make sure you use the LNHT edge prep (as opposed to LNMT). One sharp/ground and the other is molded. You need sharp.

If you decide to go the route of the H490 in that material, make sure you use the ANCX edge prep (as opposed to ANKT). Same reason as above.

T490 does great in high chipload applications. It will do poorly if you ever decide to enter a full slot/width of cut because of chip clearance. H490 is a great tool for full width cuts.

What's the failure mode you're experiencing with the H600 inserts? Chipping?

350-500sfm is pretty fast for 304 stainless. Perhaps too fast. I don't regularly machine 304 but I'm thinking somewhere in the 200-250 SFM range would be more appropriate.

Edge prep is a factor as TerribleJuan already stated. A T-land is a blunt edge better suited for steels. This is probably what you have since you said you were using the cutter for 4140.

My guess is that the high speeds and blunt geometry are work hardening the material and thus hammering the inserts. You could get inserts for the H600 that are better suited for the material, but I think you're on the right path by going to a normal face mill. A 50-taper horizontal like your Makino A88 can easily push a 2" facemill at high axial DOCs so you'll gain a lot of efficiency to make up for the slower SFMs. In contrast, a high feed mill can only be pushed so far if you cap the speeds (as you need to in 304 stainless).

The H490 is more free cutting than any tangential insert facemill like the T490, so that's the one I'd choose between the two. You could go a step further (I would) and try the HM390 which is even more free cutting, and close to the same cost per edge as the H490.

We use T490's (12mm) now in an application cutting pre-hardened 4140. They perform well, but the fatal flaw with the T490 design (as well as any tangential milling cutter I suppose...) is the cutter body's pocket design.

Any hiccups at all that damage the pocket, even the slightest, and the body is ruined. The inserts will still clamp up, but they will not hold their correct orientation, and you will end up with one insert sitting proud of the others. Unless you're O.K. with a single-flute face mill, you pretty much have to junk it and start with a new body. For that reason alone, I'd recommend going with the H490 instead.

If you have balls, look at their H690 line. I tested one of these, and it was awesome. Unfortunately, our fixturing was the weak point, and I couldn't push the cutter as hard as I wanted without the fixturing vibrating. If you have a solid setup, I would really suggest you give this one a try... The only downfall might be grade/breaker availability, as it's a newer design.

My choice would be the F90SD. Four cutting edges and excellent geometries. They are also about $5 on ebay.

Terrible Juan said:

Can you get me the exact item description on the H600 feedmill insert that you are using? I saw that you are using IC808 but is it "T" or "HP" edge prep?

Click to expand...

The inserts I was using as of this morning were H600 WXCU 080612T, meaning they have a honed edge. The reason I decided to give those a try was that when using H600 WXCU 080612HP IC830 in a 316 stainless job (milling 1.25 part down to 1"), the inserts did not hold up at all. Making the same parts out of titanium, HP is a must and works well.

Since I remember HP being poor on 316, I figured a little hone on the front of the tool (along with the tougher IC808 grade) would be fine. I was wrong

Failure mode is more like a smear. The inserts are chipped and smeared backwards. I agree that I was going too fast, so I slowed it down from 850rpm to 600, but kept the chipload and depth of cut the same. Still got the same results with that, 1 part per insert (not enough! they aren't huge parts).

I went into the can that holds all of the used inserts, and picked out some USED IC830 inserts (that had the HP edge prep) and was able to get 2 parts out of those used edges. Am currently running parts with new IC830 HP inserts; we'll see how it goes.

Of course, while writing this, my .500 variable flute endmill broke. Awesome...

FWIW you CAN run a .500 variable flute endmill that has 1.25" flute lengh out 1.950" from the nose of the toolholder to cut 1.9 deep in stainless going 150IPM with a .04" stepover in 304. I'm happy with the 12 parts it gave me....

IC808 is a hard, wear resistant grade. IC830 is a tougher, shock resistant grade.

A "backwards smear" sounds like flank wear, often caused by running too fast (too hot). The IC808 should actually be better for this since it's wear resistant.

How many "minutes in the cut" are the edges lasting?

Orange Vise said:

How many "minutes in the cut" are the edges lasting?

Click to expand...

With the 808 inserts with the honed edge, BARELY 15 minutes (smearing at the end)

With the 830 inserts and sharp (HP) edge, 30+ minutes (I'm seeing them as being possibly able to do 3 parts @ 45 minutes, but don't want to waste my only 2" feedmill body in case it fails suddenly)

The 830 inserts don't have any smear at 600rpm (315sfm) and maybe only some tiny chips after 2 parts. Not all the edges are chipped, and they aren't fatal chips either.

I like how this thread has escalated into saving my current tool. I'd like this job to pay for the newer facemills (and I'll most likely go to the H490 or 390 style, thanks for the input), but the office would like this job to not lose money in the short term. I quoted tooling costs for this op, and I'm still under what I quoted, even at one insert per part. I was worried about this very thing. There isn't a material that I hate more than 304

Newer tools aren't always the answer, although they do have their place.

Sounds like your on the right track with a different insert choice. I would still back off the rpm slightly and keep the feed the same or bump it up a bit to keep the cutting edge in clean materiel that hasn't had a chance to work harden.

If you are set on purchasing new cutters you may be better off using the H490 in the "C" periphery grind in IC330.

The other solution for your feedmill might be to use an "MF" body instead of "FF". It will take a .120" DOC, still run a high chipload, and be better suited for nasty stainless and titanium jobs.

So I finally got someone to purchase me an H490 facemill. This one: ISCAR Cutting Tools - Metal Working Tools - H490 F90AX-12 : 3104777 - H490 F90AX D2.50-4-1.0-12

2.5" diameter, 4 flute. Even got the coolant thru 50 taper holder to go with it.

Purchased 1 pack of H490 ANKX 120508PNTR and one pack of H490 ANKX 1205PNTR-CS (chip shredder). Gonna test them both to see what works well.

I guess I should have looked back at this thread to see the advice about the C grind, but oh well.

I purchased the 830 grade, as currently I've gotten that grade to play well with the current feedmill. I can get 2-3 parts out of already used IC830 HP inserts regularly. The new IC808 HP edge ones I purchased do not last any longer than the IC808 T edge, although they fail by chipping and not smearing like the T. Again, thankfully the Makino has spindle load monitoring, else that feedmill would be toast.



Any suggestions on how deep I should push the new facemill when it arrives in a few days? It has a max cutting depth of .472, so I was thinking in the .300" deep range. 250-300SFM, .008 ipt. Sound close?

I dont have any experience on H490 type yet, but i can confirm the few problems that have been raised regarding T490 / Tangential inserts.

I've wasted around five 40mm cutters T490/similar from Tungaloy, due to full slotting and chips not getting cleared, one or two insert breakages ruining the pocket, even when tool monitoring stops the machine, its already too late. And latest one was using face mill holder weakening the body too much/and or taking too big cut, so it would apparently "bend" abit, and inserts would break/fracture while running/tightening screws (I was offered weldon bodies next, but i think i'll skip due to other possible problems).

Tungaloys Dorec seems to be identical vs H490 i think?, been thinking about those, or maybe just try H490, have to compare prices abit, having more cutting edges doesnt always mean cheaper insert, think triangular insert lost vs regular shoulder mill, nor did we have good experiences from those either.

So, this job ended months ago, and I forgot all about updating here.

As I said, I purchased the 2.5" H490 facemill with TSC holder to go with it. I decided that I needed to be kind of aggressive on the depth and feed, so I programmed it to be about .300" deep and .008"/tooth on the feed (I think; it was months ago and I don't have the program at hand)

Anyway, put it in there, and went to town.

The Makino didn't mind the load the tool was drawing, and the setup was very rigid. No chatter, very nice. For the first 1.5" or so, anyway. Good thing I was standing there. On one of the steps, The inserts let go on the break thru.



Here is the part:




So, I threw the facemill back on the shelf, and put the feedmill back in the machine.

I ended up running 180 of these parts with used feedmill inserts. They were loud, cycle time wasn't great, and I had to flip them every part, but I got the job done, and inserts were essentially free!

This is what the feedmill looked like after running one part:



This is the used insert before running a part:



And here is the part:











BTW, I don't want to make it sound like the H490 facemills are bad, because they aren't!

I've since run a bunch of 1045 with this facemill, and .300 deep at .008" chipload 2" wide dry (thru spindle air blast) is completely doable. It works great!