What's new
What's new

Looking for wisdom regarding 316ss

tjd10684

Cast Iron
Joined
Jan 26, 2011
Location
PA
I have an idea and I wanted to bounce it off some of wiser minds than mine.

Ok I got a problem job going right now with some 316L SS. The issue is I am going through tooling at a prodigious rate. The material is 1/4" x 3/4" sheer cut 316L and I am going through tools at the rate of about 2 per day. I am running a 3/8" 5 flute endmill made for SS .125 doc .015 woc 5500 rpm 90 ipm. Those are the same parameters that I run on all my other (extruded) 316 SS jobs and that endmill typically lasts 3 weeks or 150-250 parts. I think the difference between my current job where I'm getting 30-40 parts and other 316 SS jobs is the material. Specifically the fact that its sheered from a plate. I think the sheering process is work hardening the stock and killing my tools.

Does this sound right to anyone or am I just crazy?
 
cold rolled and work hardened 304/316 SS typically has a machinability rating of
0.2 cubic inches per min per hp as compared to
annealed thats about
0.4 cubic inches per minute per hp
.
so usually feeds and speeds and depth and width of cut is adjusted or you loose the corners or get fast wear or even sudden tool failures. it also warps a lot more when released from vise / fixture clamps
.
this assumes no large hard spots of slag. rice size ones can give sudden tool failure of many new tools one after another. small ones can give 10x or faster abrasive wear
 
Are you burning it or chipping it?

I usually burn tools in SS and have to slow the spindle speed.

Chipping and or complete failure. I am using a tool with a slight radius (0.015-.020) to help with corner chipping but even thats not helping on this one.
 
Chipping and or complete failure. I am using a tool with a slight radius (0.015-.020) to help with corner chipping but even thats not helping on this one.

.
loosing corners usually too much ipt feed, too much depth and width of cut, too much sfpm. and if hitting slag or hard spots that obviously hard on cutter
.
if metal is 200% harder to machine then cutting parameters need to be adjusted. also tool deflection (vibration) increases with harder material cause cutting forces are 200% higher
 
tool life normally 20 to 60 minutes with SS, number of parts dont mean much its how much cubic inches of metal you are turning into chips.
.
some SS you lucky to get 1 or 2 parts per end mill
 
Could you send the work pieces out to be annealed? I do prototype machining but if I have challenging parts to make out of stainless I will anneal the blanks in our little heat treat oven before I start just to make my life easier.
 
tool life normally 20 to 60 minutes with SS, number of parts dont mean much its how much cubic inches of metal you are turning into chips.
.
some SS you lucky to get 1 or 2 parts per end mill

If 20-60 is true then I may be getting greedy. I would say I'm getting at least 100 min of cut time from each tool on this job before I start to see signs of chipping then its quickly down hill.
 
Could you send the work pieces out to be annealed? I do prototype machining but if I have challenging parts to make out of stainless I will anneal the blanks in our little heat treat oven before I start just to make my life easier.

Maybe I would have to get a quote. My gut tells me though that I might be better off using up what I got then buying different stock for the next round. I think my material supplier has something called trubar thats extruded thing is its more expensive. The customer will not like that, I guess though they are either going to have to eat a price increase either from tooling or from different material. I guess I got some spreadsheets to make up do later.
 
Trubar is fantastic. It's square, parallel, and relatively flat on parts with a +/-0.005 tolerance we will index the part by flipping on the raw material surfaces and have no issues keeping tolerances.

Are you using hsm for these parts?
 
If 20-60 is true then I may be getting greedy. I would say I'm getting at least 100 min of cut time from each tool on this job before I start to see signs of chipping then its quickly down hill.

.
your doing good with SS, usually better to change end mill after 60 minutes rather than risk sudden tool failure
 
Trubar is fantastic. It's square, parallel, and relatively flat on parts with a +/-0.005 tolerance we will index the part by flipping on the raw material surfaces and have no issues keeping tolerances.

Are you using hsm for these parts?

Yes we are.

.
your doing good with SS, usually better to change end mill after 60 minutes rather than risk sudden tool failure

Your probably right, so far we have been lucky in that we have not scrapped any parts with a tool failure. At least nothing that can't be buffed out.
 
Yes we are.



Your probably right, so far we have been lucky in that we have not scrapped any parts with a tool failure. At least nothing that can't be buffed out.

.
3/8 carb end mill is extremely cheap compared to 1" dia end mills. SS often varies and if you hit a hard spot or slag thats big enough it will damage any end mill.
.
very hard to predict tool life with 100% certainty usually better to use conservative tool life times and change tool when expired
.
hard spots of slag shown damaged 42 carbide inserts, multiple times changed inserts on mill and still had problems getting past.
 

Attachments

  • HardSpots2.JPG
    HardSpots2.JPG
    85.8 KB · Views: 133
Why the low doc?



Sent from my Pixel 3 using Tapatalk

Stock is only .250 thick. I'm using soft step jaws with a .1 step so .125 doc is about all I can do before running into the jaws. On most other parts I'll limit it to .450 doc because I only have .5 flute length.
 
Stock is only .250 thick. I'm using soft step jaws with a .1 step so .125 doc is about all I can do before running into the jaws. On most other parts I'll limit it to .450 doc because I only have .5 flute length.
Gotcha.

3/8" 5 flute
.120 doc
10% woc .0375" 36.9 degree
3669 rpm
109.6ipm


Sent from my Pixel 3 using Tapatalk
 
Gotcha.

3/8" 5 flute
.120 doc
10% woc .0375" 36.9 degree
3669 rpm
109.6ipm


Sent from my Pixel 3 using Tapatalk

.
at those relatively high feed rates you have more sensitivity to
1) hard spots
2) cnc movement not smooth or oscillation or jerky movement as moving
3) corners and arcs sometimes very hard on end mills at high feeds
.
cycle time must not be very high ? minutes ? often its more the inconvenience of scrapping part or damaging it more than cost of end mill.
.
many will adjust cutting parameters up or down based on tool wear. that is go faster or slower til tool needs replacement at around 60-70 minutes. if tool lasts 20 minutes back off cutting parameters til it last 60 minutes and if tool lasting 200 minutes increase cutting parameters til tool lasts 60 minutes.
.
BUT metal can vary. quite often you can get a 98% success rate with certain cutting parameters and 2% of time have problems. often the 2% problems becomes a very large expensive costing 10x than some minor cycle time savings. this random problems often is cause there is random hard spots of slag in the metal
.
if your record problems with name date often at the end of the year you will see multiple problems recorded per hundreds of parts that might not seem a problem but if you track actual time wasted often its more a problem than many realize.
 
.
at those relatively high feed rates you have more sensitivity to
1) hard spots
2) cnc movement not smooth or oscillation or jerky movement as moving
3) corners and arcs sometimes very hard on end mills at high feeds
.
cycle time must not be very high ? minutes ? often its more the inconvenience of scrapping part or damaging it more than cost of end mill.
.
many will adjust cutting parameters up or down based on tool wear. that is go faster or slower til tool needs replacement at around 60-70 minutes. if tool lasts 20 minutes back off cutting parameters til it last 60 minutes and if tool lasting 200 minutes increase cutting parameters til tool lasts 60 minutes.
.
BUT metal can vary. quite often you can get a 98% success rate with certain cutting parameters and 2% of time have problems. often the 2% problems becomes a very large expensive costing 10x than some minor cycle time savings. this random problems often is cause there is random hard spots of slag in the metal
.
If your record problems with name date often at the end of the year you will see multiple problems recorded per hundreds of parts that might not seem a problem but if you track actual time wasted often its more a problem than many realize.
...if your using proper hsm, those issues go out the window. We are here to make money.

Sent from my Pixel 3 using Tapatalk
 
One hour tool-life and 20-40 parts sounds like heaven. Now and then I get a threading job in 316L stainless. One insert edge lasts one part. That is with Iscar inserts. I ran Sandvik too but then the tool-life was very unpredictable: between 1 and 5 parts. Cutting speed was about 1/3 that of the Iscar and it was string-city. Not sure what is most economical really.
 
316 ss truebar, 3/8" 6 flute imco endmill for roughing, 200 parts per endmill using Haas and ham...

That's considerably more roughing than the ops parts. Don't forget to run DRY as a bone while roughing.

e488491c24a76df32468c21e31f962af.jpg


Sent from my Pixel 3 using Tapatalk
 








 
Back
Top