What's new
What's new

Looking for some advise on turning 17-4 in Condition A

shdfx1

Plastic
Joined
Jun 4, 2019
Hey there guys. I usually turn 7075 aluminum ( stuff will make anyone feel like a rockstar) and 4140 PH for my job. I am running a Haas ST-15Y with collet chuck that provides me with a decently rigid setup. I am now working with some 17-4 in Condition A. I am looking for some advice from people who have turned it before. I use Sandvik OD and ID profiling tools a few, through tool coolant, I-dream Carbide drills and a Mitsubishi Indexable drill at .937 diameter. I make fairly small parts and I start with stock at a diameter of 1.75.
What kind of feeds and speeds do you guys run for this stuff? My insert recommends have been fairly useless so far. I have had some success running at an SFM of 800-900 and a feed anywhere from .008 to .011.
My self and a partner run a small start up business with just the two of us. We are trying to conserve money and with hat being said, I am here asking for some insight from fellow machinists. I am trying to achieve good tool life and decent finish. Mainly I am just trying to avoid the waste of inserts. I want to achieve good running numbers but do not have unlimited corporate funds to troubleshoot without some good research and advice. I am self taught in both programming and operating a cnc so you will have to forgive me if I am speaking with a lack of knowledge or nomenclature. Thanks guys
 
Do you have the option of heat treating it to H1150? It will machine better, by a fair bit. My experience with condition A (annealed) is that it's pretty gummy, and tough. I normally machine H900, which is harder, but actually finished better, and cleaner.
It does normally shrink a little in the h/t process, but not a lot. I can't remember how much off the top of my (old) bald head :) - but someone else will be along soon that will know.
Good luck!!!
ETA: agree on the beauty of 7075! Love that stuff.
 
Specifics with pictures is the best way to get help here. What are the actual inserts you're using now, what failure modes are you seeing (Chipping? Crater wear? BUE?), speeds and feeds you've tried that didn't work well enough, etc.

Your metals vendor may have machining parameters for the stuff they sell. Also, must you use Condition A, or can you use a hardened variety. Most of us prefer to machine 17-4 hard rather than soft.
 
I don't think we are going to get it heat treated this time around. I am willing to bet that nexct time it wilkl be ordered in H900 or H1150. Honestly i think he ordered in cond A as a mistake. Thanks for the advice
 
I run it in the 400-450sfm range usually, or whatever I have to do to make it happy. I don't really care what condition, all 17-4 machines like butter to me.
 
Turning it in the A condition I think is terrible.

I would use as strong of insert shape as possible I prefer on the sticky gooey stuff a positive type chip breaker like Kennametal MS in grade 5025.

What part of Idaho?
 
I would just stick with 7075....

Of course you need to use what you've got though. 17-4 isn't difficult in any condition. The only exception to that is building complex parts under 1" diameter. Tiny uncoated Tools are different, but doable.

It's sort of annoying when a noob asks how to Machine a material, and all the responses are "change material". Like geeewiz guys, thanks!!! :)

R
 
BTW the best start feeds and speeds for stainless's and harder gummy metals and Stainless are 350SFM and .008-.010 MAX and .050 to .1 on DOC maybe more if your machine can handle it.

I use CNMG432 or WNMG332 at 400SFM, .01 feed and .08 depth of cut for most stainless. That seems to be the sweet spot for me.

No wonder he is getting that weak VBMT insert destroyed at 800SFM and .011 feed.
 
Stainless specific inserts like you are using are really intended for austenitic stainlesses like 300 series.

17-4 in particular (and martensitic stainlesses generally) cut much more like alloy steels, and respond much better to steel specific grades and geometries than stainless ones.

That said, machining 17-4 in the A condition is horrible, and I have deliberately not done enough of that to make an informed statement on what works best.

I work with it very frequently in H900 and H1150 conditions. H1150 is best if you don't have a specific requirement for anything different. H900 still turns and mills really nicely, but is pretty difficult to tap etc.
 
Your inserts are strong enough to run that kinda feed. let alone the speed. I dont know what your DOC is but anything over .020 is going to beat the crap out of that style insert..

Sorry that was a huge Typo, your inserts ARE NOT strong enough for that type of cut. not "ARE" like I said "above"
Those inserts are basically useless for any rough turning over .020 doc if that.
 
Jeeze, you guys. 17-4 annealed is okay.

Since you are a Sandvik guy, op, I was happy with KNUX inserts on that. Dash -2 nose. More if you can get away with it. Slippery coolant (oil would be better but ...) And no 900 sfm, either. Eek. 400-ish is more like it. Mess with the feed to just break the chip. Cuts good, nice finish. Shrinks a reliable .001"/inch during heat treat. Turns a kind of golden-purpley color, pretty.
 
Last edited:
Max spindle speed is 4000 rpm. I usually take anywhere from .045 to .065. That seems to usually be where my machine is happy. It gives me quiet cuts and meets specs consistently that way so I tend to keep it there. I have been unsure of whats the best for 17-4. I currently have it at .048. 450 sfm and .008 feed per rev. It is not doing bad job but its noisy and i would think that must be chatter unless it just cuts noisy as my surface finish was not to bad. I have a lot of unknown with materials outside of 7075. I have been teaching myself for the past 9-10 months so If you have to hold my hand in getting the answer your looking for to help me out, Then I apologize.
 








 
Back
Top