Thread: 17-4 H900 machining

Having a hard time getting any kind of tool life roughing blanks in 17-4 (H900).

I'm using all AlTin coated carbide with coolant (Hocut795)
Tried speeds ranging from 200-350SFM
Tried heavy and light stepover (.200-.02 with a 1/2 inch 7Fl).
Tried running slow (12 IPM)
Tried running faster (up to 40 IPM).

Seems like I'm not getting any tool life no matter what I do.
Anybody with lots of experience running H900 17-4 have any advice?

I have never had much luck machining stainless at the stated SFM. Try 100-150.

Originally Posted by JCaswell

Having a hard time getting any kind of tool life roughing blanks in 17-4 (H900).

I'm using all AlTin coated carbide with coolant (Hocut795)
Tried speeds ranging from 200-350SFM
Tried heavy and light stepover (.200-.02 with a 1/2 inch 7Fl).
Tried running slow (12 IPM)
Tried running faster (up to 40 IPM).

Seems like I'm not getting any tool life no matter what I do.
Anybody with lots of experience running H900 17-4 have any advice?

Try this FSWizard Calculation

Basically try 0.05 stepover 1.0 depth.
390 SFM, 2750 rpm,
0.0030 ipt, 57 IPM

7 FLUTE?

Originally Posted by zero_divide

Try this FSWizard Calculation

Basically try 0.05 stepover 1.0 depth.
390 SFM, 2750 rpm,
0.0030 ipt, 57 IPM

7 FLUTE?

Yes, I had some nice 7 flute corner-radius end mills left over from a titanium job. Pretty much chunked them all messing with this and will probably go with 5 Fl next.
Those S&Fs are pretty much in line with what I started with, but I ended up backing off to .03 stepover, .4 depth, 200 SFM and .0012 IPM and it still wipes them out in a couple parts.

Very perplexing.

Originally Posted by JCaswell

Yes, I had some nice 7 flute corner-radius end mills left over from a titanium job. Pretty much chunked them all messing with this and will probably go with 5 Fl next.
Those S&Fs are pretty much in line with what I started with, but I ended up backing off to .03 stepover, .4 depth, 200 SFM and .0012 IPM and it still wipes them out in a couple parts.

Very perplexing.

Imho is SS you should feed as hard as possible without chipping the cutting edge. It does not like light feedrates.
Did you try running it dry? Just to see what happens. Might be coolant causing thermal cracking.

Sorry to threadjack but:

Your knives are beautiful! Absolutely love the raw power in the designs, they strike me as far more interesting than anything I've seen in a long time! (The CK-2 in particular)

I'm planning to get back into knifemaking once I get my CNC mill setup. So it's inspiring to see work like this!

[end of threadjack]

Originally Posted by JCaswell

Having a hard time getting any kind of tool life roughing blanks in 17-4 (H900).

I'm using all AlTin coated carbide with coolant (Hocut795)
Tried speeds ranging from 200-350SFM
Tried heavy and light stepover (.200-.02 with a 1/2 inch 7Fl).
Tried running slow (12 IPM)
Tried running faster (up to 40 IPM).

Seems like I'm not getting any tool life no matter what I do.
Anybody with lots of experience running H900 17-4 have any advice?

Have you thought about annealing the 17-4, roughing it within say .02, and then re-heat treating to H900?

I machine 15-5/17-4 H900 with solid carbide, depending on how much material your removing, your not getting to get great tool life, I always underestimate the amount of carbide I'm going to go thru. If you anneal the 17-4, you can machine with HSS, at a slower rate, so it can be a trade off.

I would be inclined to slow down to 750-1000 rpm and see what happens.

If you make a blade (I assume it's a blade) from 17-4 you could machine it net, annealed, then HT to H900 and not expect much if any distortion. That's one of the nice properties of 17-4/15-5. plus you can do the ht yourself, as long as the oven can got to 900f

Originally Posted by triumph406

If you make a blade (I assume it's a blade) from 17-4 you could machine it net, annealed, then HT to H900 and not expect much if any distortion. That's one of the nice properties of 17-4/15-5. plus you can do the ht yourself, as long as the oven can got to 900f

Thanks, everyone, for your comments and help.

The blades are NOT 17-4 --- too soft.

When they're stainless, it's going to be something like S30V, CPM154, etc. I go 59RC on S30V and 61RC in CPM154, etc. After Heat Treat, it's all grinding and honing pre-machined holes to final, etc.
I like 17-4 for pivots, screws and, in this case, certain lock components.

Anyway, I'm trying a different approach, which is similar to where I started--5 Fl, about 150 SFM, .05 radial and .220 axial engagement and about 12 IPM.

Doubtless that will change, --maybe lighter radial and faster on the feed,
but the ONLY cutter life I've gotten was maybe 20 parts doing 250 SFM .03 radial//.220axial engagement, and 24 IPM with a 7 flute.

Every variation I've tried with greater radial engagement (like .200 or .125) has resulted in chipped cutter flutes from the first part.

I do not think you said, conventional or climb milling? Might want to change directions.

Originally Posted by txcncman

I do not think you said, conventional or climb milling? Might want to change directions.

Climb

Originally Posted by JCaswell

Thanks, everyone, for your comments and help.

The blades are NOT 17-4 --- too soft.

When they're stainless, it's going to be something like S30V, CPM154, etc. I go 59RC on S30V and 61RC in CPM154, etc. After Heat Treat, it's all grinding and honing pre-machined holes to final, etc.
I like 17-4 for pivots, screws and, in this case, certain lock components.

Anyway, I'm trying a different approach, which is similar to where I started--5 Fl, about 150 SFM, .05 radial and .220 axial engagement and about 12 IPM.

Doubtless that will change, --maybe lighter radial and faster on the feed,
but the ONLY cutter life I've gotten was maybe 20 parts doing 250 SFM .03 radial//.220axial engagement, and 24 IPM with a 7 flute.

Every variation I've tried with greater radial engagement (like .200 or .125) has resulted in chipped cutter flutes from the first part.

Yes, stainless really hates high radial engagement.

Did you try running it dry with light radial engagement? Like 50 thou or less. I hope tou are compensating for chip thinning.

You may actually have more luck running dry because SS does not transfer much heat into the chip, but into the tool and the cuttion edge.
And coolant causes premature tool failure in those situations.
By the way TiAlN cutters are also known as "dry cutters" they beform better without coolant. High temperature causes the coating to become harder. And coolant will lead to termal shock and micro-cracking of the cutting edge.

Originally Posted by JCaswell

I like 17-4 for pivots, screws and, in this case, certain lock components.

(

If strength isn't an issue, 17-4 H1150 is a lot more civilised to work with.

When turning 17-4 I get great life from TiCN coated inserts, either dry or flooded.

Well, I think I may have a baseline to start from.
Cycle time is long, but the tools are holding up and the finishes are great. I'll do a few and maybe start juicing it up a little to see where I can make up some time.
Here's where it's out now:

.5 Duramill WhisperKut .025 corner radius. stub
160 SFM
.05 radial
.220 axial
10 IPM (about .002 IPT)

I know I can get 180 SFM and 14 IPM with minimal degradation, but I get slightly more warping of the part (flat 3/8 x 1.25 x 4), and am only saving about 10 minutes in a nearly 2 hour combined cycle time (2 operations about 50 minutes each right now--some subsequent 3D machining soaking up the time).

I'm thinking of going with .03 or less on radial engagement and moving faster, but I'm not sure I'll be making up much, but it might be quieter/easier on the machine ...

You still have not shown the part. What are the possibilities of using alternative machining methods, such as plunge milling?

Originally Posted by JCaswell

Well, I think I may have a baseline to start from.
Cycle time is long, but the tools are holding up and the finishes are great. I'll do a few and maybe start juicing it up a little to see where I can make up some time.
Here's where it's out now:

.5 Duramill WhisperKut .025 corner radius. stub
160 SFM
.05 radial
.220 axial
10 IPM (about .002 IPT)

I know I can get 180 SFM and 14 IPM with minimal degradation, but I get slightly more warping of the part (flat 3/8 x 1.25 x 4), and am only saving about 10 minutes in a nearly 2 hour combined cycle time (2 operations about 50 minutes each right now--some subsequent 3D machining soaking up the time).

I'm thinking of going with .03 or less on radial engagement and moving faster, but I'm not sure I'll be making up much, but it might be quieter/easier on the machine ...

Hah! thats within 10% in feed and 20% in speed from what FSWiz is suggesting with HSM turned off.
I am glad my program got it so close to the actual working parameters you are using.

Can you please update us on what final S/F you will be using after/if you decide to juice it up?

Originally Posted by txcncman

You still have not shown the part. What are the possibilities of using alternative machining methods, such as plunge milling?

I'm not sure plunge milling would be appropriate here.
Right now I'm doing more of a peel milling approach.

There's a lot of stock removed from around the part.
In retrospect, it probably should have been waterjet from sheet, but that would have created unique fixturing problems in this case. Might have been worth it, though.

Originally Posted by zero_divide

Hah! thats within 10% in feed and 20% in speed from what FSWiz is suggesting with HSM turned off.
I am glad my program got it so close to the actual working parameters you are using.

Can you please update us on what final S/F you will be using after/if you decide to juice it up?

I noticed that too. There are others that suggested wildly different things.
I started with similar perimeters when someone I trust recommended treating hard 17-4 like titanium (which is weird because it's so different in actual properties). When cutter life didn't seem too good, I looked around for other advice and received an astounding diversity of conflicting advice. I tried several of them, including those from cutter manufacturers I got on the phone. All of them suggested close to 50% engagement, but none of that worked long.

The parameters I'm using now (peel milling) were suggested from the fine folks at MilTec/Ultratool.

I have used the parameters from the SF Wizard you included (which are slightly more aggressive), and they seem to work fine. I plan to adopt those for a while, and (since I have more than 200 of these parts left to do, might try going faster and lighter too (apparently the rule of thumb for titanium on these lighter Haas machines), to see how that goes.

I really like the S&F calculator you posted. Thanks for doing so!:cheers:

Again, still no clue as to the actual part. That leaves you on your own to figure it out. But, another suggestion might be an inserted mill to remove the bulk of the material. Good luck.

I'm not sure how it'll help with the bigger question of S&F for hardened 17-4, but I don't mind showing the part, and if it's useful to someone, I'm game.

Here's what's left of the pile of stock (about 200 pcs.)
Results of the 1st op is on the left.
The 2nd op is on the right.

As you can see, I'm simply holding the stock in one vise for the first op, and go to softjaw in the second vise for Op 2.

EDIT:
Sorry, it's not uploading my pix. Not sure why ...
They're the right format, not too big ...
I'll try later, maybe a server thing (?)