[MDLang]

I was at the WMTS here in Edmonton last week and three of the machine tool suppliers were running feedmills. Hass, Mori and Hurco. Of the three only the Mori was running at what I considered to be the correct feeds and speeds. The other two were way to slow and seemed a bit surprised at my suggestion that they could easily double the feed and increase the SFPM by 30%.

I came away realizing that feedmills are not well understood by many people and obviously allot of people are missing out on an excellent roughing tool.

We use feedmills almost every day where I work and have been fortunate enough to get free trail tools from Sandvik, Ingersoll, Tungaloy , Hitachi and Iscar. It seems we are the most willing to run at the suggested feeds and speeds so the suppliers are always bringing us the latest tools to break. We also find unconventional uses for their tools so we can give them good feedback to take to other customers.

A couple days ago the Hitachi guys gave us the latest Hitachi high feed endmill to try out and we happened top have the perfect job to try it on. The last time Hitachi came by we decided to try their 1 inch feedmill to shave some time off a slow roughing job and managed to cut the cycle time from 15 minutes to 7. Today I tried the new hitachi feedmill out on the same job and cut another minute and a half.

For those of you who don't use feedmills or don't know what they are here is a clip of the job I setup today using the new tool.

http://www.youtube.com/watch?v=RVttPttIQZ0

Any one else use feedmills?

[ctate2000]

Haas and Hurco are not capable of pushing a tool like a Mori. However, the Mori costs twice as much. Probably the reason for the difference.

[laka]

I'm actually going to run my first job with a feedmill tomorrow. We got an Iscar 1.25" 3 flute feedmill. the material is 3.5" thick A516 Grade 70 carbon steel, and i'm going to use it to open up many pre drilled holes from 1.5" to about 3.5" finished size.

I did some test cuts today, and was having good success with approx 600 SFM and I forget the chipload, but somewhere around 165 IPM was sounding nice.

As far as I know, the proper way to use these tools is to take light DOC's but very high feed. I was planning on using helical interpolation to open up these holes 0.3" on diameter per pass, at about 0.045" DOC. After watching your video, would it be beneficial to simply bury most of the tool in the cut and instead of taking multiple passes at 0.3" larger dia, just take possibly one pass to make the hole to finished size?

It is a little nerveracking watching this thing rip around so fast, especially when I dont have much experience with this tool, and how much it can take. I'll be running it on a Matsuura VG800.

I'd be interested on your thoughts with my setup. Can I really push this tool to it's limits?

Thanks

[Joseph Souza]

Dear MD,

Could you possibly send me some sort of link to these "Feedmills" either Iscar or Sandvik I would appriciate seeing what sort of mill cutter you are refering to?

[email protected]

-Joe

[MDLang]

Joseph,

http://www2.coromant.sandvik.com/cor...C-1129-044.pdf

Sandvik R210. Nice feedmill with a good insert for stainless.

http://www.iscar.com/Ecat/familyHDR....type/1/lang/EN

Iscar with the WOMT inserts. Great feedmill for helical milling bores because of the large insert. These ones give you the smallest hole vs. endmill diameter with no predrilled hole.

http://www.hitachitool-eu.com/downlo...w/ASR-Pico.pdf

Hitachi ASR or IASR. Very inpressed with the performance of the 1" 4 flute cutter. Double or more the feed of their 2 flute and much more resistant to insert failure.

Laka,

We have a 1 1/4" Iscar. It's the last Iscar we have and the only one we still replace when we need to. We keep it for exactly what you are doing. You can helical mill a 1.5" diameter hole with that cutter with no predrilled hole. It's the only 1 1/4" we know of that will do that small a hole.

Here's where I would start.

650 SFPM, .120 inches per revolution (.04 chip per tooth), .045 pitch per rotation around the hole spiraling down, full 3.5 inch diameter in one pass (that's a 1.0" radial width of cut) with a 1.5 inch predrilled hole, no coolant, lots of air to keep the hole clear of chips to avoid double cutting.

I would be looking for a medium blue chip, loose 6 shape. Some sparking is acceptable. flame is obviously bad and indicates too high rpm or too slow a feed combined with too high rpm or worn inserts.

With the Iscar you need to be careful about catastrophic insert failure due to excessive wear. Watch the bottom of the insert for flat spots. I would say a .015 flat spot is maximum. There isn't much clearance between the cutting edge and the bottom of the pocket on the Iscar's so insert failure usually results in pocket damage. This is why we've moved away from the Iscar's. Rolled down sleeves, a gloved hand and an air hose to keep the chips clear is a good idea. If you check the inserts after every hole until you get an idea on insert life, insert failure shouldn't be a problem.

I would expect 25-30 minute in cut time before indexing, if youu need to index sooner lower your surface footage

I would think you may end up anywhere between 600-750 SFPM. I rarely have to run below 600.

Watch the entry on the first hole. There is usually some sparking on entry but it goes away once it's fully in cut. If it doesn't, stop and drop the surface footage 25 SFPM at a time. If it sparks more than occasionally stop again check your inserts reduce the speed again and restart or you may not make it through 3.5 inches.

The sound is your best friend. Get used to the tone of the cutter and listen for changes in the tone. It should remain fairly consistent and if you hear a second tone come in you've probably chipped an insert. It will be a low under tone that sounds like a misfiring engine and it's easy to miss at first. The operator should never leave the machine as insert failure will lead to cutter destruction fairly quick if you don't catch it immediately.

Reducing the surface footage is the best way to make yourself more at ease as reducing feed has little effect except to rub rather than cut leading to premature insert wear. Reduced DOC. has the same effect as you really have a fairly thin chip to begin with due to the chip thinning effect of the lead angle.

Definitely try the full diameter in one pass. If you watch the video again listen to the difference in the sound between the pocket with full engagement Vs. the half diameter radial cut when it's roughing the OD.

Again resist the temptation to use coolant as thermal shock will break down the cutting edge leading to premature insert wear. Air is best.

When it's cutting right it will sound right so play with the overrides till you get the right sound and compare it to insert life.

Have fun and don't forget Iscar specs up to a .060 DOC and a .060 feed per tooth so the .040 and .045 are middle of the road and what I find to be average. SFPM is what is hardest to predict.

Mike

[laka]

I'm anticipating my program to be in the range of 5 hours of using this feedmill so I'd love to use coolant rather than hold the air gun. Our machine has 300 PSI coolant thru the spindle, should this be sufficient?

Thanks for all the other info, i'll let you know how she runs. I'm excited!

[MDLang]

You can use thru coolant with that cutter but I find it reduces insert life.

I had a job that ran 30 minutes solid feedmilling and I had to use coolant because of spindle and tool growth. I was gaining .01 in length after about 10 minutes in cut. Coolant solved the growth problem but I had to reduce the surface footage to get the insert life back up to where I could finish the cycle without stopping to index the inserts.

I would set it up without coolant then add coolant, reduce the SFPM a bit and watch insert life. Make sure the coolant is on before the cut starts and stays on till its done.

Mike

[laka]

This tool is great!

I ran this tool today for about 2 hours straight and it easily cut our previous machining time in half. I was running it pretty conservatively until I get the feel for it, but the chips sure were flying.

Any experience using these on 316ss? From what the insert box says, the SFM is about 50% faster. But will the insert life be there?

Thanks for all your information. It was pretty fun running this thing today, just watching the chip bin fill up!

[MDLang]

Iscar has a stainless grade ,IC 908, insert with a positive rake, WOCT I think, that we've used in 17-4 but not in 316.

We use a sandvik feedmill with their stainless insert for 316.

Mike

[blowmebigtime]

I use high feed mills daily, Hitachi runs the best for me, although I use Iscar's multimaster screw on feed mill head with great results. I also use Fette's and Jabro's solid carbide feed mills as well - they go all the way down to 1.5mm dia. there is no quicker way to rough out a small rib than with a Jabro feed mill. Also I have the advantage of having to be able to program a form tool and run 3D programs . I have measured all the tools shapes and program right to size without having to lie about what the cutter shape really is, that way I can semifinish and even finish molding areas with high feed mills. I would also stay away from the thru coolant.. I have tried this with 1000psi thru the spindle coolant and found the insert life suffered, also you can't see what is going on and don't know when to change the inserts, it's nice to be able to see that slight red glow and know the inserts are getting dull and it's time to change. If an insert lets go at the huge feed rates these are capeable of, forget trying to salvage the tool body it's all over, I usually change inserts slightly premature for this reason.

[dertsap]

http://coroguide.coromant.sandvik.co...asp?LangID=ENG
you guys may be interested in sandvics cutter module (calculator) which should apply to any similar grades from other companies

the calculations are bullet proof

[kalmah]

Any one else use feedmills?

Prototyp give correct parameter for high feed mill.

http://www.cutting-data.com/

[Razor-Tool]

So, I took some time to develop my own tool. It’s called Razor-HF and can be used to cut hard metals at high metal removal rates. It’s great for confined spaces, tight corner radii in molds and long reach applications.

The first trials seemed to work out ‘OK’. We made up a 1/2” tool and were able to cut .020” deep in D-2 Tool Steel at 80 IPM and 2700 RPM(only because that was the max speed and feed on our ProtoTrak). After a few adjustments to the tool geometry, we were able to cut smoother and harder. We just scratched the surface of what this tool is capable of. A 1/2” Razor-HF should really run at 4000RPM and 150 IPM. Tool life was reasonable considering the nature of cutting hard steel with uncoated carbide.

Come and check it out at www.Razor-Mill.com

This tool is for sale at less than 1/3 of the cost of the Big-Name manufacturers and is available in both coated and uncoated versions. I can offer different lengths as well depending on your requirements.

Feel free to reach out to me at [email protected]

[Razor-Tool]

You really have to look at the metal removal rates. It's cool to go really fast but in some cases, like where you don't have a lot of stock or if you need a good finish, you may be better off with a conventional cutter.
Also, if you're in really soft metals or plastics, high feed tools will probably just smear the material.
That said, I still really LOVE high feed cutters for STEEL, STAINLESS and TITANIUM. The indexable cutters make a lot of sense but the not much has been available in small diameters. The replaceable heads cost a fortune and so do most solid carbide shank tools.
These guys are half the price of the replaceable heads and can resharpen them on the cheap RAZOR-HF
I ran the 1/2" at 100 IPM yesterday at 3000RPM with a DOC of .020" and it purred like a kitten