How to avoid work hardening 304 while machining
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Jan 2008
    Location
    Goleta, California
    Posts
    12
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default How to avoid work hardening 304 while machining

    A coworker of mine is machining a part for our drive system out of 304, but we've heard it can be tough to work with. The primary problem seems to be that you can very easily work harden the 304 as you machine it. That being said, does anyone have some tips on how we could machine the part the quickest without hardening it?

  2. #2
    Join Date
    Jun 2006
    Location
    Beaverton, OR
    Posts
    5,459
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    51

    Default

    Keep your cutter moving. Dont let it sit on one spot or its hard time. I have never had to much of an issue with it though.

  3. #3
    Join Date
    Dec 2007
    Location
    Iowa
    Posts
    230
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default 303?

    Switch to 303 if you can. You'll never go back to 304.

  4. #4
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,232
    Post Thanks / Like
    Likes (Given)
    1068
    Likes (Received)
    3025

    Default

    It doesn't get that hard, if you keep your tools sharp.

    Where the trouble starts is most often in drilling with HSS: the drill overheats, the cutting edge fails, the pressure and rotation begins to stir weld some of the drill to the bottom of the hole. That creates the hard skin (of HSS), but its a very thin hard skin.

    For regular turning, and milling, keep the tools sharp, and you won't have much grief. Finish with sharp carbides. The honed edge of a roughing insert promotes cold working of the surface skin. On flimsy pieces, this can increase deflection of the part on subsequent passes, as the tool rides the surface. I've bored and bored and bored the last thousandth out of a 5" long hole in stainless Finally ended by sharpening a razor sharp high rake edge to really make the tool take out what was intended. I still wouldn't say the hole was 'hard' but it was cut resistant. It'll still pick-up and score like nobody's business if you try to slide something close fitting into that 'hard' surface, so its not very hard.

  5. #5
    Join Date
    Oct 2003
    Location
    Philadelphia, PA
    Posts
    880
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    83

    Default

    Gave me a problem cutting off in the lathe. Cut great until I got close in to the end of the cut at the core of the rod. All of a sudden what cut great throughout the entire cut just stopped cutting. And I mean stopped.

    I wasn't using power cross feed for the cut-off and I bet that when I got in close to the middle of the rod the remaining diameter got small enough to heat up and spot harden. Everything was fine until I had to stop cutting for an instant to readjust my hand on the cross feed knob and then after that, it just laughed at my cut-off tool.

  6. #6
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    10,603
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    3955

    Default

    That's right. Don't let the tool dwell. Keep feeding. Back the cutting edge away slightly if you have to stop feeding for any reason. Leave sufficient finishing stock to ensure the cutting edge gets below the work hardened film left by the semi-finish cut. Change out/sharpen dull tools. Good tips for any material.

    Work hardening is usually a different deal than heat treatment. Work hardening has to do with generating a cold worked film on the material that has different properties than the undisturbed material. These properties in some materials can be significantly harder than the base metal, and in those materials capable of heat treatment elevated temperatures from friction can range ip to hardening heat.

    304 is an austinetic material. It will not harden appreciably from heat it and quench it technique. However it will readily work harden and for that reason it has to be cut with a definite feed and depth of cut so the passage of the cutting edge goes under the hardened film left by the previous cut.

  7. #7
    Join Date
    Mar 2007
    Location
    Long Beach,CA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Make sure you have a lot of lubrication in your coolant.8-10%.Go easy on the speeds.
    Last edited by Stewen; 02-23-2008 at 10:58 PM. Reason: Misprint

  8. #8
    Join Date
    Feb 2006
    Location
    Oakland, California, USA
    Posts
    1,780
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    13

    Default

    I've done a lot with SS, mostly 304. Not like some guys here, tho.

    Unless you can sharpen drills, you will want to have several new bits on hand. When you feel the drill just begin to dull, and it's pretty quick when it happens, yank it right out instantly and put a new, sharp drill in. I've found that slow RPM with pretty heavy feeds seem to work well, along with dark sulfured cutting oil.

  9. #9
    Join Date
    Jan 2007
    Location
    Pinckney Mi.
    Posts
    3,004
    Post Thanks / Like
    Likes (Given)
    4266
    Likes (Received)
    778

    Default Coolant

    my issues (so far) with S.S. have been solved since I started using flood coolant,like stated above,minimum 10%.I am presently useing water soluble oil type coolant,it is white after mixing,the seller said 8%,I went 10%,it has eased my burden quite a bit.
    It drills almost nice now,almost.
    the gol darnit of S.S seems to be the in freak went sea we machine it,if we cut it every day perhaps we would become friends. but for some folks ,only seeing S.S. once in awhile,perhaps we forget the proper procedures,as stated above.
    GW

  10. #10
    Join Date
    Nov 2005
    Location
    Ohio
    Posts
    305
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    28

    Default

    I'm so glad this thread came up.

    I just recieved a delivery of some 304. 3/8" x 4" x12 foot randoms. My job is to make Auto exhaust flanges (header flanges). The part will be just under 4" square with a 4 bolt pattern and a thru pocket in the center. I've never worked with 304 before and use high performance carbide drills and endmills (z carb).

    I was planning to saw the material into blanks which will get predrilled. Then bolt the blanks to a sacrificial tool plate to machine the inner pocket and outer perimeter with a 3/8" dia Z-carb end mill. With the 3/8 endmill in 3/8" material, I'm planning to do a full slot, full depth in one pass for the pocket and perimeter leaving about .015" for a finishing pass. SGS suggests about 3000rpm and 23 ipm feed.



    Whattaya think? is .015" enough for a finishing pass...or should I go deeper..say .060" to get under the work hardened "skin".

    Any thoughts and tips for this part are appreciated. This is a goverment job for a buddy...with no payment/profit...so it would be nice to do this as painless as possible. He bought the material.

    Rob

  11. #11
    Join Date
    Mar 2007
    Location
    Long Beach,CA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    0.03 is enough to get "under the skin".

  12. #12
    Join Date
    Feb 2006
    Location
    Oakland, California, USA
    Posts
    1,780
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    13

    Default

    When you say "saw", do you mean bandsaw? While I'll freely admit that I have a POS 4x6, I do use good blades. Stainless is pretty hard on bandsaw blades. You might want to ask your bud to pony up for "expendables" as well -- such as several extra blades to have on hand.

  13. #13
    Join Date
    Nov 2005
    Location
    Ohio
    Posts
    305
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    28

    Default

    Thanks Al,

    Yep, I'm planning to bandsaw the 12 footers into 8" blanks. I use lenox bi-metal blades...and normally run about 180 sfpm in CRS. I'll drop the speed for the 304.

    I think the blades run me about $45ea....about $35 for a 3/8" z-carb...and about $55 for a 3/8" carbide drill. Hmmm...so it looks like I'm already in over $100 on perishables...It will be a very nice bottle of single malt.

    -Rob

  14. #14
    Join Date
    Feb 2008
    Location
    Salem, Oregon
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default 304 "secrets"

    I am in the food industry. We have used 304 exclusively for the last 4+ decades. Two main points of advice is to flatten the angle on your drill bits by half. The same with your cutting tools. Reduce your speed by half. Band saw blades will last a long time cutting the stuff if you slow them down and brush the chips off the blade. The best coolant for 304 is water with a small amount of soap to help it spread. Water is hard on equipment. We rely on working it slow and if you need coolant, use higher concentrations of water not less. 304 is like putty. That is until you heat it up. Take large wide cuts and go for shallow and slow.

  15. #15
    Join Date
    Dec 2004
    Location
    Mariposa, California
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Stainless is painless

    Half your speed? flaten your cutter angle? Use water and soap?

    Jeez.


    Learn how to calculate sfpm(speed) and ipm(feed). That would be Surface Feet Per Minute and Inches Per Minute.

    4 divide Diameter (whatever your spinning) times desired sfpm= RPM

    RPM times # of cutting flutes times chip thickness = IPM

    Know your tooling material, M42 cobalt for drills(you can't use hss) Reams and cheap end mills.,

    Carbide for turning and good end mills.

    Coated carbide for you rich guys.

    M42 cobalt is 35 to 50 sfpm with FLOOD!!
    Carbide is 250 sfpm
    Coated carbide for turning 450 to 650 sfpm


    So, a good tian (titanium aluminum nitride) coated DataFlute 3 flute carbide endmill in a stainless geometry (about $80.00)

    4 divide .500 is 8
    8 times 350 sfpm (dataflute has free tech support for feeds and speeds) is 2800 rpm!!

    2800 rpm times 3 flutes is 8400
    8400 times .0015 (chip thickness) is 12.6 IPM

    Now your cookin with Crisco!

    Now a M42 ruffing mill (about $30.00)
    4 divide .500 is 8
    8 times 40 is 320 rpm (yawn)
    320 times 3 is 960
    960 times .0015 is 1.44 ipm


    So which is the cheap endmill?


    And, yes you have to flood, make some splash gaurds, it's not that Bad.


    Quick Vic

  16. #16
    Join Date
    Jun 2007
    Location
    New Zealand
    Posts
    2,661
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    28

    Default

    <<Everything was fine until I had to stop cutting for an instant to readjust my hand on the cross feed knob and then after that, it just laughed at my cut-off tool.>>
    Ain't that the truth !

    When cutting off (parting-off) in SS, if for any reason you have to stop the feed, reverse it instantly to prevent rub (as Mr Addy implies). This is one good reason to hand feed- because even 'tool-room' lathes with a single-tooth clutch sometimes have an appreciable 'dwell' when you reverse the feed on the fly.

    You have to develop the reflex to always be winding either in or out, until the tool is no longer rubbing.


    Perhaps the only other reason to hand feed when parting off is you get slightly more warning - rising feed force - if something goes wrong.

    But you do need good hand-feeding technique, which not everyone gets when even "newbie lathes" have power cross feed.

    In the more general turning case: if turning between shoulders, when you're winding in to start each cut, pretend you're a machine feed: anticipate when the contact will happen and have the other hand ready to supplement the feed force so there's no dwell at the moment of contact. Think inexorable !

    And on no account wind on a plunge cut with the cross feed unless your hand is on the feed lever to engage the longitudinal feed as soon as the DoC is established, if not before.

    This all assumes you can't switch to 303SS

    Even then it doesn't hurt to follow the advice given by most posters - but if contemplating this switch you need to take into account that the corrosion performance (especially in respect of pitting, which is the achilles heel of 300-series stainless steels in chlorides, such as seawater) is seriously degraded by the addition of sulphur to promote free cutting.

  17. #17
    Join Date
    Jan 2004
    Location
    Claremont, NH
    Posts
    1,639
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    49

    Default

    Everything Vic said, but adding to the drill bit message, use a 135 degree split point drill, not a 118 jobber drill. No dwell on any tools.

    Often I may add .0005 to .001 to the feed rate on 304 on the roughing cuts if the machine is sturdy enough. The trick I was taught by my old german apprentice master was "beat the material to its harden ing point - meaning cut faster than it can harden or cut it before it can harden.

    You may also want to be sure you check on inserts that are graded to cut 304 stainless, a quick call (or visit to the site) to your carbide rep or a carbide tooling company like Kennametal ect. would help. beats spending several bucks on tooling that would never quite work out quite right anyway.

  18. #18
    Join Date
    Feb 2008
    Location
    Netherlands, Papendrecht
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    We do machine a lot of Stainless steel 304 and 316(L).

    The feedrate i use is what i also use on C45 and St52 (0.25 to 0.30 mm/rev)
    The only thing i lower down is the RPM at roughing the maximum m per minute is 80 (cant tell what it is in fpm).
    For finishing i use 120m per minute, and have never had troubles with hardening of material, only if the carbide tip broke i got a little firework, but i turned that away without trouble.

    I must say that we use carbide tips (CNMG) from Iscar can't say what quality or coating.

  19. #19
    Join Date
    Feb 2008
    Location
    medford oregon
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    lots and lots and lots and lots and lots of coolant. never had an issue. I use indexable tooling and cut about 500 rpm. flood with coolant. drilling can be tricky but doable. drill small and bore to size.

  20. #20
    Join Date
    Nov 2005
    Location
    Ohio
    Posts
    305
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    28

    Default

    I started making my parts yesterday...and I can tell you that machining 304 sucks big time!!

    Speed/feed charts seemed to be all over the board depending on hardness, austienic? 304L..? Heck I really don't know what I have other than "304"... So I pick some numbers, wrote my program and let it fly. No problems on the band saw. I was able to quickly saw up the blanks for my VMC.

    In the VMC, I started with a 3/8" z-carb running thier suggested feed and speed (3400 rpm at 23 ipm). My parts are 3/8" think so I figured could do a full slot at full width to make my internal pockets...wrong! The endmill immediately broke. Hmmm...this stuff is not like CRS. So I adjusted the feed and tried again...I made it through the first pass, but the chips were packing up in the slot and welding together...and it sounded horrible. So I decided to reduced the DOC to 1/2 of the material thickness...or .187 for the 3/8 endmill. This works better...but again, the endmill breaks. Long-story short...I finally settled for running at 100 sfpm (1000rpm) with a .0015" chip load on a 2 flute carbide end mill. The feed turned out to be about 3 IPM!! A far cry from 23 IPM. I've never ran anything at 3 IPM..OMGOSH..Is this thing actually moving..? What I thought would take about 1-1/2 minutes a cycle has turned out to be just over 17 minutes. This seems to be as fast as I can run and still keep the tools together. Any faster and the corners start breaking down ...then the endmill self-destructs before the cycle is completed.

    So, my 2 hour job for a friend is turning out to be 2 days and costing a couple hundred bucks in perishables. Erhg!! You live and learn. I learned that I hate 304 and will never, ever, NEVER make anything from this stuff again.

    Yes, I'm using coolant. My VMC has a 1/2 dozen jets on the bottom of the spindle housing blasting coolant into the cutting zone.

    Just for the record.." I hate 304!! "

    -Rob


Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •