HSM In 17-4

[kunfuzed]

So sometimes I think i've finally gotten this whole HSM thing figured out, but then on the next part the situation is never the same.

 

So what I've got is some long reach (~4x dia) roughing to do.  I ordered some 1/2" Garr V5's with 1.88 reach, and .88 loc to get down in there, but they didn't come in time, so had to use some Niagra "Stablizer's" instead with a longer 2.25 reach, shorter flute at 5/8 loc.  Anyways, I come up with some numbers, used an OptiRough path with 10% step over and 100% step down, 250sfm, and .0015 actual chip load (1910ss @ 24ipm).  This sounded horrible untill I doubled the speed and feed.  But after roughing that entire part, the flutes were just trashed.  Maybe had about one left cutting, lol.

 

Material - 17-4ss 35-40rc

 

Cutter - Niagra STRN430-0.500-E1-R030.3-Z4 (1/2" 4flt R.03 2.25 reach .625 loc)

 

Toolpath - Dynamic OptiRough 250sfm, .0015 chip load, 10% radial (.05"), 100% axial (.500")

 

Holder - Albrecht APC milling chuck

 

Any ideas, or critiques to fix the tool life issue, and still peel off the metal are greatly appreciated.

 

Sorry the video isn't that impressive... thought of it too late.

 

<iframe width="560" height="315" src="https://www.youtube.com/embed/vLSUedHpKLw" frameborder="0" allowfullscreen></iframe>

[jlw™]

Why not use a shorter endmill and go as deep as you can before using the chatter maker?

 

Also, I've had fantastic luck with high feedmills. I have a few 1in iscars that I use in tight spots or smaller parts and you just can't beat them. I don't have a machine that will push as fast as the little feedmills want to go.

[jeff]

Just a thought looking at your part,assuming that slot goes through.. .couldn't you rotate that 90deg and use an indexable slitter?

[kunfuzed]

Why not use a shorter endmill and go as deep as you can before using the chatter maker?

Also, I've had fantastic luck with high feedmills. I have a few 1in iscars that I use in tight spots or smaller parts and you just can't beat them. I don't have a machine that will push as fast as the little feedmills want to go.

Ya know, I can't really remember why I don't have a shorter one in there. It may be because of the technigrip I just needed the reach. Like I said, I did order a shorter one, but it didn't come in yet, and everything else was two short. Also, I suppose I was using the lodgic that this cutter is "supposed" to perform at some given parameters, so I'll just save a tool change. Hopefully the 1.88 reach V5 will be in today though.

 

And yes, I've just noticed some solid carb feed mills that look killer for something like this.... made by Niagara I think. Haven't thought to order some yet.

[kunfuzed]

Just a thought looking at your part,assuming that slot goes through.. .couldn't you rotate that 90deg and use an indexable slitter?

Right there at the tip of the triangle, inside the ears are some pads. The part was originally a casting, with no designed alternate method, so we have to make it verbatim. Like I said before, it seems that this endmill "should" perform given the right parameters, and it needs to be used at some point, so I just decided to use it to rough everything. That and we don't have any insert slot mills that would have fit the bill.

[Colin Gilchrist]

10% stepover is killing your tool.

 

10-15% stepover is great for softer steels, but not for 17-4.

 

Try between 5-7% stepover for 17-4. Maybe even go down to 4%.

 

480 SFM.

0.0044 per tooth.

[Colin Gilchrist]

Also, I strongly recommend that if you are going to be doing a lot of HSM and HEM milling, that you get cutters optimized for the process.

 

• Variable Pitch Flutes - non-equal cutting edge spacing prevents harmonic vibrations from building.
• Variable Helix - Also helps keep harmonics from happening.

I'd recommend the VariMill II line from Widia, or the HARVI (II or III) from Kennametal.

 

http://www.widia.com/en/products/29388747/29665015/29665021/38346376/100006723.html

 

http://www.kennametal.com/en/products/20478624/57493250/1522849/44814260/44814782/100004038.html

[?Mark]

What condition is this 17-4 PH at? It makes a world of difference, I

[Colin Gilchrist]

BTW, just for reference, I thought I'd just throw this here:

 

HSM starting values:

 

• 20-40% for Aluminum. Depends mainly on Depth to Diameter ratio. 1:1 = 40%. 2:1 = 30%, 3:1 = 20-25%, 4:1 <= 20%
• 10-15% for soft steels. Again, adjust for D2D ratio, going lower as your endmill gains length.
• 4-8% for Stainless, the harder and tougher the grade, the less stepover you can take.
• 3-5% for Ti and HRSA material

[kunfuzed]

Also, I strongly recommend that if you are going to be doing a lot of HSM and HEM milling, that you get cutters optimized for the process.

 

• Variable Pitch Flutes - non-equal cutting edge spacing prevents harmonic vibrations from building.
• Variable Helix - Also helps keep harmonics from happening.

I'd recommend the VariMill II line from Widia, or the HARVI (II or III) from Kennametal.

 

http://www.widia.com/en/products/29388747/29665015/29665021/38346376/100006723.html

 

http://www.kennametal.com/en/products/20478624/57493250/1522849/44814260/44814782/100004038.html

 Hmmm... the "Stabilizer" from Niagra says it has "Asymmetrical Flute Geometry"... but I'm not even sure if I should be using it in this application, was just the best tool I had on hand.

 

I have some Garr V5 em's coming in though, our local supplier pushes a lot of Garr.  Do you have thoughts on them (Garr V5's / VRX's)?  I would like to try the Varimills, or the Harvi's though too.

 

 

BTW, just for reference, I thought I'd just throw this here:

 

HSM starting values:

 

• 20-40% for Aluminum. Depends mainly on Depth to Diameter ratio. 1:1 = 40%. 2:1 = 30%, 3:1 = 20-25%, 4:1 <= 20%
• 10-15% for soft steels. Again, adjust for D2D ratio, going lower as your endmill gains length.
• 4-8% for Stainless, the harder and tougher the grade, the less stepover you can take.
• 3-5% for Ti and HRSA material

 

That's awesome info!  Where did you find that?  Also, where can I read up on a formula for determining the increase in SFM as a result of lighter step overs?  Ratio for Dia to Lenght of EM would be great to figure out too(for feed, and DOC too in reference to long reach em's, i just realized those numbers above do recommend for DOC).  And thanks for the advice on reducing the stepover to 5 to 7%ish, will probably try 5%.

[kunfuzed]

What condition is this 17-4 PH at? It makes a world of difference, I

I honestly can't remember, and honestly didn't look it up either... lol.  I just remember having the 35-40 Rc in mind.  Will look that up when I get back into the shop though!

[jeff]

 Do you have thoughts on them (Garr V5's / VRX's)?  I would like to try the Varimills, or the Harvi's though too.

 

I use Garr often for hardmilling keyways in 8620 after carb & harden, haven't used the ones you mention though. They do make quality stuff.

Varimill makes a great product.

 

I recently tested a 7 flute Force endmill from Fullerton Tool.  I removed a ton of material in Dynamic Mill and it is one of the best endmills I've ever used.

I'll definitely be buying more of those.

http://www.fullertontool.com/carbide/tools/3600?utm_campaign=Force+ReLaunch&utm_source=hs_automation&utm_medium=email&utm_content=27564546&_hsenc=p2ANqtz--irH63EwJIcWKVeN7sEOMnFXPPobmLSwrZhXYk-CbolD61ebWIpSOh-sPLsijeOUzY4duPGyY7fGJ-Tr9VnoxUBvEbcw&_hsmi=27564546

[kunfuzed]

I use Garr often for hardmilling keyways in 8620 after carb & harden, haven't used the ones you mention though. They do make quality stuff.

Varimill makes a great product.

 

I recently tested a 7 flute Force endmill from Fullerton Tool.  I removed a ton of material in Dynamic Mill and it is one of the best endmills I've ever used.

I'll definitely be buying more of those.

http://www.fullertontool.com/carbide/tools/3600?utm_campaign=Force+ReLaunch&utm_source=hs_automation&utm_medium=email&utm_content=27564546&_hsenc=p2ANqtz--irH63EwJIcWKVeN7sEOMnFXPPobmLSwrZhXYk-CbolD61ebWIpSOh-sPLsijeOUzY4duPGyY7fGJ-Tr9VnoxUBvEbcw&_hsmi=27564546

I can see where having the higher flute count can help pull off the metal in the tougher stuff, where you need lighter step overs.

[Matthew Hajicek - Singularity]

I'm using a Helical 3/8" 7 flute for HFM in 17-4 H900.  They have a program much like HSMAdvisor that recommends depth, step, speed and feed.  I've been using those numbers with pretty good results.

[kunfuzed]

I guess that's one tool I need to start using... HSM Advisor... or similar.

[gms1]

 

I have some Garr V5 em's coming in though, our local supplier pushes a lot of Garr.  Do you have thoughts on them (Garr V5's / VRX's)?  I would like to try the Varimills, or the Harvi's though too.

 

Im currently running 1/2" and 3/4" V5's in 316L stainless, waterjet cut. They are 110" long 3/4" thick and about 1in wide (it looks like a really looong picture frame with fancy angles).

 

1/2 with .03 rad (EDP 50107) V5 102ipm(.0089ipt), 2292 rpm(300sfm), 7%(.035") stepover, 1/2 doc with dynamic contour. Cut is roughly 1h 1min a part and we are getting 11 parts per end mill. I honestly believe I could double that feed and still be in that 40$ tools wheelhouse and still make a killing but the powers that be are happy as it is right now.

 

We had the niagra/seco folks in today and they want us to do an apples to apples change with their tool to test. Their tool has 7 flutes instead of 5 and I am betting it costs more $$$ but we will see.

[kunfuzed]

Im currently running 1/2" and 3/4" V5's in 316L stainless, waterjet cut. They are 110" long 3/4" thick and about 1in wide (it looks like a really looong picture frame with fancy angles).

 

1/2 with .03 rad (EDP 50107) V5 102ipm(.0089ipt), 2292 rpm(300sfm), 7%(.035") stepover, 1/2 doc with dynamic contour. Cut is roughly 1h 1min a part and we are getting 11 parts per end mill. I honestly believe I could double that feed and still be in that 40$ tools wheelhouse and still make a killing but the powers that be are happy as it is right now.

 

We had the niagra/seco folks in today and they want us to do an apples to apples change with their tool to test. Their tool has 7 flutes instead of 5 and I am betting it costs more $$$ but we will see.

Awesome! I have also had success with these cutters, though they were shorter, and in more ridgid setups at the time. Did you get those numbers out of the catalog? I usually try to use all of the flute, and I think I need to step down the radial value, cuz sometimes I blow through them.(seems the catalog only recommends 1xdia)

[jeff]

I guess that's one tool I need to start using... HSM Advisor... or similar.

HSM Advisor is the best out there, I use it daily.

[kunfuzed]

HSM Advisor is the best out there, I use it daily.

 

Hmmm.... was going to like that, but "You have reached your quota of positive votes for the day"....

 

... guess I need to be more negative?

 

Lol.

 

Seriously though, thanks for all the input guys!  This site is such a great resource, it's odd that I only pop up every few months or so.  Lol

[gms1]

Awesome! I have also had success with these cutters, though they were shorter, and in more ridgid setups at the time. Did you get those numbers out of the catalog? I usually try to use all of the flute, and I think I need to step down the radial value, cuz sometimes I blow through them.(seems the catalog only recommends 1xdia)

Yeah we are way above and beyond the book recommended feed and speed for that tool . I think the book is 1xD and like 40ipm. We plugged in these numbers to the sgs calculator (really good calc btw) divided the feed in half and started there. Now I just need to get the folks here to let me go faster till I break it.

 

http://www.sgstool.com/content.aspx?contentId=FractionalSquareCornerRadiusEndMillCalculators

 

 

Jeff have you tried their Fantom mills? I was really trying to get some in from them and they were a bit more expensive than the garr.

[jeff]

 

Jeff have you tried their Fantom mills? I was really trying to get some in from them and they were a bit more expensive than the garr.

I haven't tried those yet.

The Force had a free trial earlier this year and I just recently got to try it out on a job that had a ton of material removal.

[kunfuzed]

I think the book is 1xD and like 40ipm.

I know! Mind boggling ! The only thing I've tried is modifying a tool from the Iscar library and using the Iscar HEM factor slider. Sometimes works, sometimes doesnt.

[Matthew Hajicek - Singularity]

HSM Advisor is the best out there, I use it daily.

 

HSMAdvisor is the best for general purpose; I use it for my non-Helical brand cutters.  I like the Helical Milling Advisor for the Helical cutters because it has a complete and frequently updated library of all their cutters, and who should know their cutters best but them?  Sometimes I use both at once to get a second opinion sanity check.

[AMCNitro]

Get some kennametal harvii II and be happy.  Amazing tool.

[Tim Johnson]

Kennametal Harvii II are Widia Hanita varimill II. When they came out I wasn't impressed with them and went back to varimill I. The varimill ER series was a great improvement and the current ER victory grade is better yet. I'm pushing my five flute 1/2" .030 radius end mill in 316/316L stainless @ 5% woc and feeding at 347? ipm (I'm home and can't look) in a stubby er32 collet chuck.

 

Garr uses Mitsubishi carbide for its small diameter end mills which in my opinion is the best carbide manufactured at this time.