What's new
What's new

Thread Turning 304 Stainless HELP

Italiano83

Aluminum
Joined
Mar 4, 2013
Location
Miami, FL
This is a CNC turning application. I'm getting really frustrated with this material. 304 Stainless is probably the worst material I've ever had to machine. I mean even Titanium machines MUCH better. All I want to do is Single Point ID thread a 1/2"-18 thread into a part, but man I've tried 900rpm, 1300rpm, 1700rpm, 2000rpm, 2500rpm and not only do none of them sound particularly nice, I'm getting chipped inserts every 15 to 20 pieces or so and the thread is never consistent. I'm flooding coolant and using carbide 60 degree inserts. Clamp pressure is fine and all other ops on the part cut like butter now. Please, somebody give me a recommendation before I throw this bar stock thru a wall.


-Jon
 
Feeding straight in or at an angle? If its a Fanuc control, what value are you using for the infeed angle? Sometimes people think they should use 29* as you might for manual threading, but 29* in the Fanuc control is for Acme threading. Should use 60* since the control is set up for using the included angle rather than infeed angle.

IMO, a standard 60* on-edge single point insert always makes it sorta difficult to get good threads in tough materials. Much easier to get good results with lay down partial or full profile inserts. The same single point insert that works fine on free machining materials can give finishes that look about like a pine cone on either tough alloys or SS.

Also, there seems to be a lot of 304 out there today that has about the same machinability characteristics as poor quality rebar.
 
Ha!Ha!... Doubt that will solve anything but could make you feel a bit better.

Is 1/2"-18 a typo? Interested in what you're using as a threading bar/insert? You've tried tapping it with no luck?

Sorry I'm not awfully familiar with 304SS other then to say folks considered it a major PITA. Obviously you've tried tool manufacturer suggested speeds in 304SS. Do they have a insert designed specifically to 304 you could try?

Is the turret sitting off kilter?

Brent
 
Ha!Ha!... Doubt that will solve anything but could make you feel a bit better.

Is 1/2"-18 a typo? Interested in what you're using as a threading bar/insert? You've tried tapping it with no luck?

Sorry I'm not awfully familiar with 304SS other then to say folks considered it a major PITA. Obviously you've tried tool manufacturer suggested speeds in 304SS. Do they have a insert designed specifically to 304 you could try?

Is the turret sitting off kilter?

Brent

The thread is technically a PG-9 thread. I'm using a 60 degree insert and just making the thread a bit oversized, rather than the required 80 degree on the PG-9 thread, but the customer is ok with this. I just used 1/2-18 for those who are not familiar with PG threads. Major: .600" dia, Minor: .560" dia, and 18 threads per inch. I'm using a lay down style insert which is giving me much worse results that the solid carbide 60 degree bar. I'd like to avoid thread milling this, so any other recommendations would be helpful and much appreciated.
 
For a .600 dia, I'd say anything less than 3k rpm's would be too slow and you'd just be tearing the material instead of cutting it. Are you able to run it faster than 2,500?
What type of infeed are you using?
Depth of cut?
Good coolant concentration?
 
I think you should write your own threading cycle. Plunge straight in for a little thread like that, in however many passes, probably about 5 passes should get it done. You don't want the tool tip taking light spring cuts at the end, you want it to take a chip with every cut. This means aggressive cutting right to the last pass, in the sense that you position the tool a little deeper so that last pass spring is eliminated. Use a thread cutting oil, run at moderate speed, same as you would tap it at with HSS and it should be ok.

If you still don't have success, then write your thread cycle so that there is a forward and then a backward shift to the tool position to make the insert cut on one side only, no dragging the insert along on the material. I usually do this for heavier threads than that would be. Spring passes are a carbide killer particularly on stainless because of the tendency for the chips to weld to the cutting edge, and then break off taking some insert with it.
 
For a .600 dia, I'd say anything less than 3k rpm's would be too slow and you'd just be tearing the material instead of cutting it. Are you able to run it faster than 2,500?
What type of infeed are you using?
Depth of cut?
Good coolant concentration?

I believe I can run up to 4000/4500 rpm on that spindle. straight infeed. DOC .002 and also tried 20-30% of total thread depth for first cut, but that didn't fix anything. Good coolant flow and concentration. I'm just using a G71 threading cycle (okuma control). Based on this any recommendations?
 
I believe I can run up to 4000/4500 rpm on that spindle. straight infeed. DOC .002 and also tried 20-30% of total thread depth for first cut, but that didn't fix anything. Good coolant flow and concentration. I'm just using a G71 threading cycle (okuma control). Based on this any recommendations?

yes I have a suggestion but no one likes it or tries it or they complain aboot it....but it works fine....try it as see if it fixes problem.....100RPMs and take off small amounts like maybe .001 per side or .002 per side....takes a tad longer but threads will always be toot sweet....if you need to make money then speed up from there....slowly....until your making crap again....then back it down a notch and that should be the ticket....basically run it same as titanium or slower yet....but I run almost all threads at 100RPMs...I need them to be perfect instead of hundreds and hour...I have only one shot and no extra stock.....sometimes its the only stock that exists....try 100 and see what happens....if you have to go larger diameter like 3 inches and maybe 4 threads per....then I speed it up to aboot 300....never more....good luck.....oh one other thing....set the code to run at 55 degrees infeed on compound...again...only thrying it will you see results and be able to make your own determination then...post up a pic then.....bet there perfect,,,,later
 
I believe I can run up to 4000/4500 rpm on that spindle. straight infeed. DOC .002 and also tried 20-30% of total thread depth for first cut, but that didn't fix anything. Good coolant flow and concentration. I'm just using a G71 threading cycle (okuma control). Based on this any recommendations?

I can't recall offhand the format of it, but Okuma allows different types of infeed for threading.
Straight in, alternate, and you can even set the angle for coming down 1 wall of the thread (which I've had the most success with).
It's either a Gcode format, or a parameter setting. It's been a long time since I've been on an Okuma lathe.
 
Technically, a decent thread carbide grade for mixed materials (including stainless) should be able to run up to about 2500 rpm (about 350 sfm) for external threads. On internal threads I have not been able to run the same parameters as OD threads. Take into account length/diameter ratios of threading bars and chip control and life goes down even more.

I'd recommend the solid bar rather than laydown...that's quite a small hole even when considering a mini laydown style insert.

Okuma 1/2"-18 UN ID thread...

G0 X50 Z50 G97 S1500 M3 M8 M42 T202
X.37 Z.3
G71 X.50 Z-.??? D.01 U.002 H.062 B50 F1 J18 M33 M73

The B50 gets you a 5° modified flank infeed off a 60° thread. The M33 turns that modified flank to an alternating flank infeed (also called zig-zag infeed). The M73 is just one of Okuma's options for how it divides up the passes between your D and U values.
 
just got done threading 600 pcs. 304 stainless 5/8"-11 by 1.250" long o.d. thread using sandvik lay-down profile insert. no modified infeed angle, just straight in. thread looks like it was chromed. perfect finish. great tool. one insert (three edges) for 600 pieces and not one chipped insert edge. profile inserts are the way to go, if possible.
 
yes I have a suggestion but no one likes it or tries it or they complain aboot it....but it works fine....try it as see if it fixes problem.....100RPMs and take off small amounts like maybe .001 per side or .002 per side....takes a tad longer but threads will always be toot sweet....if you need to make money then speed up from there....slowly....until your making crap again....then back it down a notch and that should be the ticket....basically run it same as titanium or slower yet....but I run almost all threads at 100RPMs...I need them to be perfect instead of hundreds and hour...I have only one shot and no extra stock.....sometimes its the only stock that exists....try 100 and see what happens....if you have to go larger diameter like 3 inches and maybe 4 threads per....then I speed it up to aboot 300....never more....good luck.....oh one other thing....set the code to run at 55 degrees infeed on compound...again...only thrying it will you see results and be able to make your own determination then...post up a pic then.....bet there perfect,,,,later


I'm pretty new to machining, been doing it for about 3 years now when I started my own manufacturing company, and to this date, I've never been given a more accurate, mind-blowing piece of advice. I cannot post a pic due to our customer confidentiality agreements, but I can tell you that looking at the thread in that 304ss is akin to the birth of my first child. WOW! Sir...you are my hero.

For future reference in this forum, I ended up at about 200RPM and .002" DOC for the time being. It produces a beautiful thread. I need to get some parts out the door so I'll try to play around and speed it up a bit later, but with only a .040" thread depth, it doesn't completely sandbag my cycle time currently.

Thanks again, I'm still in awe

-Jon
 
just got done threading 600 pcs. 304 stainless 5/8"-11 by 1.250" long o.d. thread using sandvik lay-down profile insert. no modified infeed angle, just straight in. thread looks like it was chromed. perfect finish. great tool. one insert (three edges) for 600 pieces and not one chipped insert edge. profile inserts are the way to go, if possible.


Could you please post or PM me some part numbers? I'd like to play around with that to speed up my cycle time. What RPM were you running? Thank You. -Jon
 
Technically, a decent thread carbide grade for mixed materials (including stainless) should be able to run up to about 2500 rpm (about 350 sfm) for external threads. On internal threads I have not been able to run the same parameters as OD threads. Take into account length/diameter ratios of threading bars and chip control and life goes down even more.

I'd recommend the solid bar rather than laydown...that's quite a small hole even when considering a mini laydown style insert.

Okuma 1/2"-18 UN ID thread...

G0 X50 Z50 G97 S1500 M3 M8 M42 T202
X.37 Z.3
G71 X.50 Z-.??? D.01 U.002 H.062 B50 F1 J18 M33 M73

The B50 gets you a 5° modified flank infeed off a 60° thread. The M33 turns that modified flank to an alternating flank infeed (also called zig-zag infeed). The M73 is just one of Okuma's options for how it divides up the passes between your D and U values.

Thank You, when I get in to the office tomorrow morning, I will play around with this. thanks for the advice.
 
I'm pretty new to machining, been doing it for about 3 years now when I started my own manufacturing company, and to this date, I've never been given a more accurate, mind-blowing piece of advice. I cannot post a pic due to our customer confidentiality agreements, but I can tell you that looking at the thread in that 304ss is akin to the birth of my first child. WOW! Sir...you are my hero.

For future reference in this forum, I ended up at about 200RPM and .002" DOC for the time being. It produces a beautiful thread. I need to get some parts out the door so I'll try to play around and speed it up a bit later, but with only a .040" thread depth, it doesn't completely sandbag my cycle time currently.

Thanks again, I'm still in awe

-Jon

glad it worked for ya....you can thread or tap most (almost all) materials at 100RPMs....even plastic and cloth and wood sometimes....and then you speed up if need be for desired results....what degree did you use or did you just go straight in and did you run a free pass at the end also...sometimes another free pass or 2 it will burnish the hard materials and look like ya ground the things and could produce an unexpected....."ATTA BOY".....LOL....that 55 degrees on CNC lathe will produce sweet threads 97% of the time on all threads except acme or buttress....NPS and NPT included so that there is minimal need to ever change a basic G71 threading program....now you can leave the RPMs and just plug and play X and Z and feeds for all threads and reduce scrap and save money on tips and save the machine on wear and tear....remember.....the tortoise won the race....and speed kills....enjoy
 
just got done threading 600 pcs. 304 stainless 5/8"-11 by 1.250" long o.d. thread using sandvik lay-down profile insert. no modified infeed angle, just straight in. thread looks like it was chromed. perfect finish. great tool. one insert (three edges) for 600 pieces and not one chipped insert edge. profile inserts are the way to go, if possible.

What insert grade?
 
Well... rule of thumb, lower speeds. 900 seems like dying of old age... but the last threads I did in 304 were on a 2" diameter, like a 6 pitch... 150 or so RPM, diesel for cutting fluid... and HSS!!! aloris cutter, compound in as above at 29..
Most beautiful threads.
Speed kills, coolant is a serious consideration.
But look at your insert coating selection. Altin seems to do good..
 
When I have been like the OP and to the point of throwing the steel through a brick wall.

When you've tried everything you can think of then sometimes you have to go to extremes.

When nothing has worked and changing something defies all logic try it anyway.

Nothing is off the table when things turn to shit. When your out of ideas test the extreme change anyway. Testing is how you prove, testing is how to eliminate ideas on how to fix the problem.

Speed, feed, doc, tool, holders, steel, if your limiting what your willing to change to figure out problems chances are you'll limit your ability to find solutions.

Brent
 
When I have been like the OP and to the point of throwing the steel through a brick wall.

When you've tried everything you can think of then sometimes you have to go to extremes.

When nothing has worked and changing something defies all logic try it anyway.

Nothing is off the table when things turn to shit. When your out of ideas test the extreme change anyway. Testing is how you prove, testing is how to eliminate ideas on how to fix the problem.

Speed, feed, doc, tool, holders, steel, if your limiting what your willing to change to figure out problems chances are you'll limit your ability to find solutions.

Brent

little tip...you wont have to do ANY OF THAT if you run at 100RPMs for all threading and tapping in lathes or VMC or whatever....its the math and physics....its why hand tapping you can tap KRYPTONITE rather easily all day long with one tap...cuase your going 10 RPMs...you wont have to limit a thing or try to figure anything out....there will be shinny perfect threads all day long....it is what it is...and a lot don't like to hear this on this site
 
little tip...you wont have to do ANY OF THAT if you run at 100RPMs for all threading and tapping in lathes or VMC or whatever....its the math and physics....its why hand tapping you can tap KRYPTONITE rather easily all day long with one tap...cuase your going 10 RPMs...you wont have to limit a thing or try to figure anything out....there will be shinny perfect threads all day long....it is what it is...and a lot don't like to hear this on this site

Hi John,

Thanks for the tip!

I don't know the math and physics, maybe you could expand on that a bit? I'm mostly self taught by trial and error along with guessing. When I said "defies all logic" I was hoping you wouldn't take it as I was referring to you.

I was trying to get the point across that when having problems nothing is off the table when looking for solutions including a really slow rpm. Good call! You nailed!

I actually think in such a small thread if I was doing it myself would have been not far from what you recommended to the OP except at a smidgen higher rpm. I would definitely thread at 100rpm if that solved my problem I was having? Hell I would piss on a spark plug if I'm to the point of throwing the stock though the wall. The point being to eliminate possibilities by testing them rather then dismissing them even if you think it's a waste of time.

I'm in Kokomo, where at in Indiana are you?

Brent
 
Last edited:








 
Back
Top