D2 dimension post heat treat?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default D2 dimension post heat treat?

    I've called my local heat treat facility 3 times attempting to find someone who can help me out, unfortunatly there must be only 1 guy and he is never in his office, so I am turning here for some answers. I have a few parts that will be machined out of D2. The part is roughly 5.5" OD with a 3" bore. Its 0.625 thick. I plan on grinding it post heat treat in order to meet dimensional tolerances. I just need to know how much extra stock I should leave for a worse case scenario. I can't afford to scrap these parts.
    Do I leave .0005"? .005"? .05"? On all dimensions. I don't want to be grinding on these to long but I would be screwed if they came back from heat treat as scrap.
    I understand it "depends" on a lot of factors. I just need a ball park worse case scenario.
    Thanks!

  2. #2
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Hardened to 60 RC......I forgot to include that.

  3. #3
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,220
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2655

    Default

    Quote Originally Posted by Evlyn View Post
    I've called my local heat treat facility 3 times attempting to find someone who can help me out, unfortunatly there must be only 1 guy and he is never in his office, so I am turning here for some answers. I have a few parts that will be machined out of D2. The part is roughly 5.5" OD with a 3" bore. Its 0.625 thick. I plan on grinding it post heat treat in order to meet dimensional tolerances. I just need to know how much extra stock I should leave for a worse case scenario. I can't afford to scrap these parts.
    Do I leave .0005"? .005"? .05"? On all dimensions. I don't want to be grinding on these to long but I would be screwed if they came back from heat treat as scrap.
    I understand it "depends" on a lot of factors. I just need a ball park worse case scenario.
    Thanks!
    usually size change is certain amount per inch say .001" per inch so 5" maybe plan on .005" but it depends often bores get smaller its like part is a balloon being inflated. outside gets bigger and holes get smaller. i do no know exact amounts most would do a test part and measure. also sometimes stuff goes out of round or warps or distorts. distortion or warpage often can be a lot on bigger parts

  4. #4
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by DMF_TomB View Post
    usually size change is certain amount per inch say .001" per inch so 5" maybe plan on .005" but it depends often bores get smaller its like part is a balloon being inflated. outside gets bigger and holes get smaller. i do no know exact amounts most would do a test part and measure. also sometimes stuff goes out of round or warps or distorts. distortion or warpage often can be a lot on bigger parts
    Thank you for your reply. It would be nice to do a test piece and would be the smartest route to take. I have 30 days to get these parts delivered unfortunatly.
    From a few thread I read through I got the impression .005 - .01 would be a safe landing zone, but after doing some calculations, I saw in various heat treating websites, I was calculating some whacked out numbers.

  5. #5
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    139
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    91

    Default

    I would leave .010-.015 on the thickness.

    I would also turn the od and the id leaving about 1/16th on both surfaces, and then take them out of the lathe chuck and let them spring.

    Re-chuck with light pressure on the jaws, finish the i.d. and then repeat for the o.d.

    I would leave around .010 on each dim.

    You may want to consider hard turning them after H.T. with ceramic inserts (if it is an uninterrupted cut). That way you can leave plenty on all sides and the post h.t. machining would be much faster.

    Just a thought.

  6. Likes plastikdreams, PegroProX440 liked this post
  7. #6
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    139
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    91

    Default

    You may also want to double draw your parts back to around 54-56 r.c. this will keep them more stable during finishing.

    If this isn't an option, then I would ask your heat treat house if they offer a straightening service, if you're concerned about warping.

  8. #7
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I am making a few extra then the order requirea so I can scrap a few if I need to while finding the right setup.
    I can hard turn a few dimension but some surfaces are riddled with alignment pin holes, air blast holes and threaded holes.
    I have a +/- .005 on all but finished OD, ID and alignment pin bore. Those are on size to -.0005.

  9. #8
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I am loving all this advice! Thanks guys.

  10. #9
    Join Date
    Sep 2006
    Location
    SE PA, Philly
    Posts
    5,340
    Post Thanks / Like
    Likes (Given)
    997
    Likes (Received)
    1778

    Default

    Get yourself a copy of the vintage "Carpenter Matched Tool and Die Steels" booklet.

    This thread may be of interest: Holes and threads in tool steel vs. heat treatment

    From that booklet and from a post on PM by a German guy trying to harden D2 (and having problems with total fails) realize that you must avoid overheating D2 (this would be to 1900° F or above - stick to 1850° F or below for sure, less if mfr's instructions tell you too). If it shrinks and becomes nonmagnetic Carpenter's book says you can try to fix it by deep freezing and retempering, or retempering at 1000°F, but from your description you'd already be screwed at that point. Follow your mfrs recommendations, but the Carpenter book indicates that HT at 1800-1850°F, drawn for an hour, and air quenched should start you out at 62/62 RC. Tempering at 450F gives you 59/60 RC. Much higher (1000F) tempering gives you 59/60 RC as well, but the book indicates that 450 is a sweet spot.

    HT at 1850 and tempering at 450 was predicted to give you about 0.00025" per inch increase in dimensions. So a rough starting point would say that a part machined to nominal size will grow on the OD by 0.01625". The ID is trickier. Because of the "failure is not an option" aspect of this, perhaps you could leave a more that adequate margin (see recommendations above) in undersizing the bore by a bit more than 0.01625. This means more grinding, but you kind of have to play it safe, right? Too bad you're not doing HT piece by piece - you could do one piece with significant margins, measure it, take the hit in more post HT grinding, but then adjust tolerances to make the follow-on pieces closer to what you need.

  11. Likes sfriedberg, PegroProX440 liked this post
  12. #10
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    139
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    91

    Default

    Too bad you're not doing HT piece by piece - you could do one piece with significant margins, measure it, take the hit in more post HT grinding, but then adjust tolerances to make the follow-on pieces closer to what you need.
    Actually, that is a really good idea^^^^^^^^^^

    You may want to turn up a quick dummy without all the little shit and send it to the heat treat house and see what happens to it.

    Then adjust accordingly.

    If treated properly, D2 is pretty stable when it comes to stuff like this. The problems arise when you induce too much stress into a workpiece and don't address it before it goes to high heat.
    And +10 on the overheating that stuff.....it never ends well.

  13. #11
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,763
    Post Thanks / Like
    Likes (Given)
    1813
    Likes (Received)
    5461

    Default

    Will you be cutting the parts from plate, or slices off a round bar? If you have the choice go with bar cuts, should be more stable due to not having directional grain structure as a plate would have from when it was rolled.

    [OK, the bar has a grain direction too, but it's on axis and shouldn't matter when making disks]

  14. #12
    Join Date
    Mar 2014
    Location
    Michigan
    Posts
    760
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    271

    Default

    Quote Originally Posted by Evlyn View Post
    I am making a few extra then the order requirea so I can scrap a few if I need to while finding the right setup.
    I can hard turn a few dimension but some surfaces are riddled with alignment pin holes, air blast holes and threaded holes.
    I have a +/- .005 on all but finished OD, ID and alignment pin bore. Those are on size to -.0005.
    Make sure the customer knows you’ll be using a .005” oversized tap on all tapped holes. I couldn’t tell you how many D2 die sections I’ve seen that wouldn’t take screws after heat treat. Chasing hardened threads with carbide taps gets expensive really quick.

    Andy

  15. Likes AD Design, Rewt liked this post
  16. #13
    Join Date
    Oct 2011
    Location
    West-Central Illinois, USA
    Posts
    1,276
    Post Thanks / Like
    Likes (Given)
    2024
    Likes (Received)
    582

    Default

    All the chrome in D2 makes it grind pissy, so a detail sent to the heat treat folks is usually a good idea. As mentioned above quenching from a too high (Ac3) temp will shrink it, over 1900F° will burn it.

    That said, it’s usually considered THE most stable tool steel out there. Attached is D2 stuff from Cincinnati & Bethlehem

    Good luck,
    Matt
    Attached Thumbnails Attached Thumbnails d2_cinci_1.jpg   d2_cinci_2.jpg   d2_bethlehem_1.jpg   d2_bethlehem_2.jpg   d2_bethlehem_3.jpg  


  17. #14
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    139
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    91

    Default

    I couldn’t tell you how many D2 die sections I’ve seen that wouldn’t take screws after heat treat. Chasing hardened threads with carbide taps gets expensive really quick.
    You can request that your heat treat house brines the tapped holes.

    We always had this option chosen. We also never chased holes with a tap, we usually used a s.s. cap screw with a "flute" ground in longways going up the screw for as deep as the callout was.

    Works great, and if you use oil, they hardly ever break off. (and they clean out all the sand from the sandblaster.)

  18. Likes Hobby Shop liked this post
  19. #15
    Join Date
    Mar 2014
    Location
    Michigan
    Posts
    760
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    271

    Default

    Quote Originally Posted by Thunderjet View Post
    You can request that your heat treat house brines the tapped holes.

    We always had this option chosen. We also never chased holes with a tap, we usually used a s.s. cap screw with a "flute" ground in longways going up the screw for as deep as the callout was.

    Works great, and if you use oil, they hardly ever break off. (and they clean out all the sand from the sandblaster.)
    Thanks, I learned something new today and sounds simple enough.
    I’ve seen guys get lucky and a couple fired for not using a .005” oversized tap. I’m sure the issue at our end because I’ve never seen or heard of this option before. The 5 shops I’ve worked at for the last 25yrs have all sent their sections to the same heat treat company.

    Andy

  20. #16
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I would think that I could take my parts and prints down to the heat treater and let them apply their expertise, right? You guys have me second guessing my decision to take on this project lol.

  21. #17
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    [QUOTE=Milland;3448399]Will you be cutting the parts from plate, or slices off a round bar? If you have the choice go with bar cuts, should be more stable due to not having directional grain structure as a plate would have from when it was rolled.

    My supplier will cut these blanks from a bar.

  22. #18
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Matt_Maguire View Post
    All the chrome in D2 makes it grind pissy, so a detail sent to the heat treat folks is usually a good idea. As mentioned above quenching from a too high (Ac3) temp will shrink it, over 1900F° will burn it.

    That said, it’s usually considered THE most stable tool steel out there. Attached is D2 stuff from Cincinnati & Bethlehem

    Good luck,
    Matt
    Thank you! I didn't realize grinding was going to cause a bit of trouble as well.
    I have a sharp learning curve ahead of me.

  23. #19
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by bosleyjr View Post
    Get yourself a copy of the vintage "Carpenter Matched Tool and Die Steels" booklet.

    This thread may be of interest: [URL="https://www.practicalmachinist.com/vb/general/holes-threads-tool-steel-vs-heat-treatment-253636/"]Holes and threads in tool steel vs. heat

    Too bad you're not doing HT piece by piece - you could do one piece with significant margins, measure it, take the hit in more post HT grinding, but then adjust tolerances to make the follow-on pieces closer to what you need.
    I wish I had more time to play with this. Honestly, when took this job, I didn't realize the issues I might face. All good though. You all provided excellent advice. Hopefully I can return the favor in the future. I think the only real issue I might regret is not charging enough for the headaches I foresee in my near future lol

  24. #20
    Join Date
    Sep 2006
    Location
    SE PA, Philly
    Posts
    5,340
    Post Thanks / Like
    Likes (Given)
    997
    Likes (Received)
    1778

    Default

    Yeah, the whole point of D2 is wear resistance, and so (as you'll read on this forum) grinding is tough: you probably should be talking to your abrasives supplier to ensure that you have the right wheel for this.

    The SS screw in the holes is a cool idea.

    Another book-learnin' thing from that Carpenter Matched Tool and Die Steel* booklet, in addition to "Thou shalt not overheat D2" is their recommendation to HT in a neutral salt bath. If you use a furnace, recommended to pack the part to be HTed with cast iron borings, and (to avoid sticking) to wrap the part in Kraft paper first. So they suggest wrapping the part, packing it into a pipe with cast iron borings, and adjusting the heat-treat time to account for getting the pipe and borings hot (they say 25 minutes per inch of diameter to get to 1850).

    *I regard that little booklet as perhaps the finest example I've ever read of something that's useful, concise, to the point, and unambiguous. It was a bit of sales genius, too. Very clear directions for perhaps 99% of tool steel selection. Worth picking up a copy from eBay.


Tags for this Thread

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
  •