What are your favorite HSM cutters?

[danielm]

I'll start. Sandvik Coromill 210 High Feed mill. 1.0 diameter. #RA210-025O25-09M. 850sfm / .030" chip load in 4330M steel (annealed). 195ipm!

[Matthew Hajicek - Singularity]

I use Fraisa solid carbide 6mm, 4mm, and 3mm high feeds for roughing between closely spaced tapered ribs. I run the 3mm at 12000 RPM and 227 IPM, .0024 step down in hardened H13, leaving about .003" for finishing. They last several hours at that rate too.

[Mic]

Iscar 5 flute Chatter Free solid carbide

 

[Matthew Hajicek - Singularity]

Iscar 5 flute Chatter Free solid carbide

 

What material and hardness?

[Allan]

What material and hardness?

 

Machine: Mikron HPM 800U ( 20k Step-Tec spindle )

Material: Material: 1.1730 ( low alloyed carbon steel 200HB )

Tooling: Iscar Chatterfree

[Joe788]

Matt, who do you guys buy the Fraisa tools from?

[tooljockey]

Fraisa USA sells direct.

http://www.fraisausa.com/cms.php?id_cms=9

 

http://www.youtube.com/user/fraisausa

[djstedman]

I have used the iscar 5flt solid carbide.. They are pretty amazing..

3/4 solid carbide 5flt w/ 1.75 flute length

 

We are doing 1.36 depth of cut .05 width of cut 100 inches per minute

 

This is in 300M at 28-32Rc

 

Iscar also makes a great series of feed mills ..

 

Just used a 1.25 Iscar helido feedmill FF EWX D1.25-4-2.5-W1.00-05

 

1.25 Dia 4flute and the inserts have 6 sides each..

 

was using it in 17-4 stainless .03 depth of cut 70 - 100% engaged on the diameter 1070 rpm at 100 ipm..

at those speeds was getting over an hour of life pre edge on the inserts..

 

We also use a lot of solid carbide hannita and kennametal feedmills..

 

we use a 6MM Hanita 70N706002MT in 300M at 54-56Rc .01 depth of cut .236 width of cut .. 5000 rpm 300 ipm and we cut litterally all day with one cutter..

 

I am going to have to look into these Fraisa cutters since I havent been able to find any feedmills smaller than 6MM in the past..

 

Thanks for the tip..

[Thoob]

Iscar 1.5" Helido upfeed. 44W Mild Steel 1200SFM .03/tooth x 5 inserts with .03DOC

3056RPM - 458IPM

I also have other high feed mills from 5/8" up to 4" but this 1.5 one is my favorite.

[Matthew Hajicek - Singularity]

I am going to have to look into these Fraisa cutters since I havent been able to find any feedmills smaller than 6MM in the past..

 

The Fraisa HFMs are four flute and go down to 3mm. Seco has down to 2mm but they're only two flute, so we use them only for 2mm. Fraisa said they'd make us some 2mm but we'd have to order about 50 at a time.

[danielm]

Speaking of Solid Carbide...there is only one place that I've seen thru-coolant for solid carb end mills. The sales guy said that they have a patent pending for it. They have the hole drilled before grinding while the carbide is 'green'. http://www.swiftcarb.com/catalog/ENDMILL_XT5_1.html

 

 

Cool Video here: http://www.swiftcarb.com/index.php/videos/16-rampmill1

[Matthew Hajicek - Singularity]

Lots of companies have through coolant solid carbides.

 

http://www.mitsubishicarbide.com/EU/West/product/pdf/b171e.pdf

[Millertime]

The Fraisa HFMs are four flute and go down to 3mm. Seco has down to 2mm but they're only two flute, so we use them only for 2mm. Fraisa said they'd make us some 2mm but we'd have to order about 50 at a time.

 

Cut alot of hard tool steels for molds h-13 s-7 m-2 d-2 up to 60-62 rc. Seco IMHO have the best solid carbide out there for mold work.They have feed mills down to 1mm 2fl. Just the other day I ruffed a mold cavity from solid s-7 58rc with a 6mm ball at 560 sfm 9000rpm 80 ipm .023 doc .070 step over.This cutter ran for 3hrs and still looked good. I would like to try a fraisa feed mill in some high rc material.

[post-al]

+1 seco.

[Tyler Robertson]

+1 Sandvik Coromill 210 High Feed mill 1.0 DIA.

 

 

Used this with a robot set-up and the thing just tears it up. Helps the low rigidity robot bigtime, and with the 2-D dynamic paths we just laughed as we turned the feed up. The sound it makes is awesome.

[David Colin]

I tried a lot of high feed cutters (with inserts).

 

One of the best to me is Stellram 7792 and X500 carbide grade. I mainly use it with Inconel718, TA6V,15-5PH,Z6NCT1810.

 

Here is my ranking (best first)

ATI Stellram 7792

Mitsubishi AJX

Ceratizit HFC

Sumitomo MSX

Sandvik 210

 

With smaller diameter cutters i also had great tool life with seco feed2 machining TA6V

[MotorCityMinion]

The Indexable 1" AJX we have has a very narrow range that you use for helical entries, but other than that it's been a great tool with the old school tool paths. Inserts last a long time and the length to dia. cut ratio that this can achieve is impressive as well.

 

Quick hijack. I thought I'd ask here because of the experience with these tools. Are you guys using the feed mills with the 2D HST tool paths? How about 3D Opti tool paths? What's the typical step over with these tools in this scenario?

 

Axial vs Radial chip thinning: Can we expect a longer or shorter run times with the feed mills in the HST tool paths?

 

I'm thinking parts with shallow part geometry / slopes would appear to be the most beneficial scenarios for this type of tool.

 

I have a job coming up, A2, L shaped part that is going to lose about 75% of the material when finished. ( 9 x 5 x 4, 10 parts ). I was thinking about using 2D HST peelmill with the 1" AJX, 45% step over and cutting a 2" wide L shaped channel from both sides to get rid of a big chunk of this. The powers that be are making me mill this. (Should have made 2 parts from 1 blank)

Any thoughts about this milling strategy are welcomed.

[MotorCityMinion]

I did a quick test using the above scenario. In peelmill, the rounding radius must be larger than the step over so..... 1" tool, (AJX) Axial DOC at .03, .45 stepover, .46 RR. required a 2" wide L shaped slot. At 2" deep, time 55 min. to rough.

 

A .50 bull em at 1.0 Axial DOC., 10% Radial DOC., .15 rounding radius only required a 1" wide slot. 5 minutes to rough. at a conservative 117. IPM. Enough said there. I can't think of a single scenario where a feed mill would out run a bull em in the 2d HST. Answered my own question.

 

To be fair, If i had a 12mm 4flt Frasia HFM, the time would be under 15 minutes according to their suggested S&F. Fraisa users, I'm calculating this at about 720 SFM and 624 IPM. Is this correct? Seems a little fast for that tool. IDK

[Newbeeee™]

MCM

Not cut A2 by HSM, but for this sort of size job and only 10off in 304 stainless steel, we would just use a 12mm dia 4x flute variflute.

Use Optirough 3D toolpath with F10000. (metric) max backfeed.

Run at 5250rpm, DOC at 100 to 150%, stepover at 10%, feedrate at 3500mm/min and coolant on (8% mix).

Now whether this is good or bad in comparrison to others I don't know. I know it knocks a ton of time off our parts doing this compared to the old way of insertables that we used to do, and it also dramatically cut insert cost as well. Also it is way kinder to our machines, compared to the 'ol way of doing it.

HTH

[Matthew Hajicek - Singularity]

I use Surface High Speed (Rest Roughing) with a stock model and 80% step over. Then I update the stock model before going to the next smaller cutter. I've been running it dry, with air blast.

[tooljockey]

Cut alot of hard tool steels for molds h-13 s-7 m-2 d-2 up to 60-62 rc. Seco IMHO have the best solid carbide out there for mold work.They have feed mills down to 1mm 2fl. Just the other day I ruffed a mold cavity from solid s-7 58rc with a 6mm ball at 560 sfm 9000rpm 80 ipm .023 doc .070 step over.This cutter ran for 3hrs and still looked good. I would like to try a fraisa feed mill in some high rc material.

 

Try the NEW Sphero-XR and Sphero-XF series ball nose end mills from Fraisa. They are made especially for Roughing and Finishing in Die/Mold applications of hardened tools steels up to and including +60 HRC!

 

http://www.fraisausa.com/

[JeffreyS]

I have been struggling with a few issues regarding tooling, and this topic got me thinking, and I would appreciate any input. I am milling 316SS using a 3/16 solid carbide end mill and looking for a better performing with less tool pressure. I have used both Helical and Walter tools with the nod going to Helical on price and performance. Where my issue lays is in the burrs generated during the cut cycle, and as we all know, the larger the burr, the more stress being introduced into the material.

 

While machining a test piece from 304ss the part remained stable within 0.001 flatness, whereas my 316ss actual piece run with the same program was 0.009 out of flat, and both parts were flat w/i 0.0005.

 

I have 400-inches of linear/radial machining, I am machining the grooves .200 deep in 0.045 DOC to keep as stable as possible, and running at 200SFM.

 

Any tooling input would be greatly appreciated.

[jeff]

I I am milling 316SS using a 3/16 solid carbide end mill and looking for a better performing with less tool pressure.

Have you tried Hanita Varimill?

Or the similar and less expensive HTC Hotmill?

[Brando]

Have you tried Hanita Varimill?

Or the similar and less expensive HTC Hotmill?

both definitely good! ive had no problem with either of these on 304L

 

hanita try this p/n TF4V4505000

htc try this p/n 800-3870

sgs zcarb ap is also good p/n 36852

 

dont know what kind of coolant your using but i ran hocut 795 at that time @ 10% mix

and make sure the tool runout is less than .0003 to get maximum life

 

i havent found too many that beat a tf4 or a tm5 series hanita