Machining Heat-Treated 17-4

rokstarr999 · May 15, 2020

I have a rush job starting Monday. I have some thin 17-4 SST parts to do. The geometry isn't all that complicated, but the part is thin with a couple semi-tight tolerances.

The Jist..

1.5" dia x .062 w/ .002 flatness.
.o62 and .0645 hole with +/- .0002
.o65 x .625 slot w / 45 deg x .040 chamfer all the way around the slot.

This is what I'm thinking so far.

1.) .063 ground plate.
2.) rough Water jet blanks. finish OD and chamfer both sides.
3.) heat treat
4.) machine slot
5.) drill and ream holes

The diameter is small so I'm hoping it will maintain flatness after heat treat. I ordered cobalt reamers thinking carbide might be too brittle at this diameter.

Any tips on sfm and chip load on a .030 4FL EM and for the reamers would be helpful.
Thanks in a Advance.

SeymourDumore · May 15, 2020

17-4 is actually nicer in HT condition, so I'd put Heat treat first, then grind, then waterjet, them machine the whole thing in one seating.

Speeds and feeds I can't give you as I usually start low and go up until shit starts to break.

rokstarr999 · May 15, 2020

SeymourDumore said:
17-4 is actually nicer in HT condition, so I'd put Heat treat first, then grind, then waterjet, them machine the whole thing in one seating.

Speeds and feeds I can't give you as I usually start low and go up until shit starts to break.

Part of the problem is we don’t have the time to send out for grinding. So we’re hoping it stays flat during heat treat.

Street · May 15, 2020

a lot of things do warp during heat treat, hoping won't help you in any way.

eaglemike · May 16, 2020

I machine 17-4 H900 all the time. I would h/t prior to grinding/machining. If you are doing a another h/t than H900 it will be easier. In my experience, it's actually easier to machine after h/t rather than annealed and pickled, especially H1150. So what condition do the parts need to be?
You can use cobalt, but I use mostly carbide. I'd use a .045 em for the slot, rather than .03, but that's just me. You might even want to rough with a .045 carbide em down the middle if you can down the middle, then finish with a .03. Slow feeds - there's a guy on here (zero divide) that sells some cool software for calculating speeds and feeds. HSMadvisor.
IMHO it's hard enough to be stable through the machining process, but not so brittle to be awful to work..0002 is sorta close - you might need to burnish to final size. Or some other way - I don't think the material will be an issue if you are used to working that close.
Good luck!

Bobw · May 16, 2020

rokstarr999 said:
Part of the problem is we don’t have the time to send out for grinding. So we’re hoping it stays flat during heat treat.

Should. That's pretty much the whole point of PH grades (Precipitation Hardening, not pre-hard).

Compared to most heat treats, its incredibly mild. Its one shot and done. Relatively low temps.
No quenches or rapid temperature changes.

I've never seen 17-4 or 13-8 warp in heat treat, at least not that I've noticed. There is a small
size change. 13-8 being more predictable than 17-4, but its small. IF I remember correctly,
17-4 will shrink in 2 directions, but may either grow or shrink in the 3rd direction. Couple
tenths an inch. Never paid too much attention on 17-4, since 99% of the time, its machined
after heat treat.

And obviously. Make sure your discs are sitting flat in the oven, not just in a big random pile.

rokstarr999 · May 16, 2020

Street said:
a lot of things do warp during heat treat, hoping won't help you in any way.

We're ordering .08" plate as well just in case, but will avoid using it if possible. Thanks for the tip though.

rokstarr999 · May 19, 2020

eaglemike said:
I machine 17-4 H900 all the time. I would h/t prior to grinding/machining. If you are doing a another h/t than H900 it will be easier. In my experience, it's actually easier to machine after h/t rather than annealed and pickled, especially H1150. So what condition do the parts need to be?
You can use cobalt, but I use mostly carbide. I'd use a .045 em for the slot, rather than .03, but that's just me. You might even want to rough with a .045 carbide em down the middle if you can down the middle, then finish with a .03. Slow feeds - there's a guy on here (zero divide) that sells some cool software for calculating speeds and feeds. HSMadvisor.
IMHO it's hard enough to be stable through the machining process, but not so brittle to be awful to work..0002 is sorta close - you might need to burnish to final size. Or some other way - I don't think the material will be an issue if you are used to working that close.
Good luck!

Tried just about every toolpath fusion had to offer and I just couldn't get a good toolpath with a .045" EM. I'm sure it's something I'm doing, but I'll be going with an .030 tomorrow morning. I already had a machining app on my phone for speeds and feeds. 69SFM with a .00008 chipload. .035 DOC. Predrilled hole with a .007 stepover. Using an adaptive toolpath. We'll see how it goes.

gkoenig · May 19, 2020

rokstarr999 said:
Tried just about every toolpath fusion had to offer and I just couldn't get a good toolpath with a .045" EM. I'm sure it's something I'm doing, but I'll be going with an .030 tomorrow morning. I already had a machining app on my phone for speeds and feeds. 69SFM with a .00008 chipload. .035 DOC. Predrilled hole with a .007 stepover. Using an adaptive toolpath. We'll see how it goes.

Slot that fucker like a goon:

Wsurfer · May 20, 2020

gkoenig said:
Slot that fucker like a goon:

I do it just like that using InventorHSM slot tool path down the center line.1/16" end mill, and flood it with a firehose. Then finish the walls. I have access to fusion but don't use it. Does fusion not have a slot toolpath?

gkoenig · May 20, 2020

Wsurfer said:
I do it just like that using InventorHSM slot tool path down the center line.1/16" end mill, and flood it with a firehose. Then finish the walls. I have access to fusion but don't use it. Does fusion not have a slot toolpath?

That is Fusion.

eaglemike · May 21, 2020

rokstarr999 said:
Tried just about every toolpath fusion had to offer and I just couldn't get a good toolpath with a .045" EM. I'm sure it's something I'm doing, but I'll be going with an .030 tomorrow morning. I already had a machining app on my phone for speeds and feeds. 69SFM with a .00008 chipload. .035 DOC. Predrilled hole with a .007 stepover. Using an adaptive toolpath. We'll see how it goes.

The quality and coating of the end mill make a huge difference in tool life. I use coated tools from Mari.
Also, it looks like you are machining in annealed and pickled, right? Stuff is gummy, and worse to machine than after heat treat.
I've been making my parts in 17-4 for 20 years. The slot in mine is wider, but principles are the same. Adaptive might work - but I think h/t and using the right tool would make a difference. Be sure your tools are running true. Good luck!! Looking for a success story!

rokstarr999 · May 21, 2020

gkoenig said:
Slot that fucker like a goon:

Well there she is. I figured out how to use the .046 EM. I just needed to draw my own slot inside the feature and use that as the feature isn't a true slot. Thought I'd share some feeds and speeds.

.045 4FL Em

Slotting at a 2 Deg Ramp
56 Sfm
.0001 FPT

.046 4FL EM

Roughing
.035 max DOC
70 Sfm
.0001 FPT
.009 Step Over

.032 4FL EM

70Sfm
1.5 IPM
.006 Step over

.032 3FL Ball Mill

80Sfm or 10K RPM (My Max)
.0001 FPT
.008 DOC with a .006 Step Over

Run Time is a little steep at 20min a part, but I've done 8 so far and haven't snapped a tool yet. All I'm doing with the .032 is rouging out that tight corner and finishing the inside wall so it's not being used much. Anyway, thanks for all the help.

Wsurfer · May 21, 2020

gkoenig said:
That is Fusion.

Aaaa. That explains why I didn't recognize the image cam tree.

gkoenig · May 22, 2020

rokstarr999 said:
Well there she is. I figured out how to use the .046 EM. I just needed to draw my own slot inside the feature and use that as the feature isn't a true slot.

Ohh yea... that Chamfer would have nuked the wall that Fusion would use to identify the slot, wouldn't it?

I was wondering why you were having trouble, and when I modeled it, I cut the chamfer a bit to form an actual slot edge (though, very tiny). That would be enough for Fusion to make it work.

Nice part!

Search

Largest Manufacturing Technology Community on the Web

Search

Machining Heat-Treated 17-4

rokstarr999

Aluminum

SeymourDumore

Diamond

rokstarr999

Aluminum

Street

Hot Rolled

eaglemike

Stainless

Bobw

Diamond

rokstarr999

Aluminum

rokstarr999

Aluminum

gkoenig

Titanium

Wsurfer

Cast Iron

gkoenig

Titanium

eaglemike

Stainless

rokstarr999

Aluminum

Attachments

Wsurfer

Cast Iron

gkoenig

Titanium

Similar threads