D2 dimension post heat treat? - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 26 of 26
  1. #21
    Join Date
    Aug 2006
    Location
    greensboro,northcarolina
    Posts
    2,393
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    587

    Default

    We get a lot of D-2 vacuum heat treated. I would leave .005 per side if I were doing them. Rough machine (leave .04 per side) and stress relieve , finish machine (leave .005 per side) , heat treat ,grind will be the safest route. If the part has very even cross sections, eliminate the stress relieving. Use sharp tools to cut it so as not to introduce stress while machining. CBN wheels for grinding is the way to go. Especially for ID grinding.

  2. #22
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2073

    Default

    How much grind stock to leave???
    Here's where you're at in a nutshell:
    D-2 as others have remarked, is shitty to grind...leave as little as possible.
    D-2 is a very stable air hardening steel that doesn't move much...leave as little as possible.

    On the other hand:
    Your project is intolerant to scrap...leave as much as possible.
    If your parts warp significantly, you may go out of tolerance from bending, not from swelling or shrinking...leave as much as possible.

    So, depending mostly on the form factor, you will need to make judgments about how to approach this.
    If your parts are long and skinny, leave more and stress relieve before finish machining and hardening.
    If they're not, you don't need to worry so much.

    Your parts are not particularly prone to warpage, they're only 5" diameter and they are 0.625" thick, so I predict all will be pretty good after heat treat.
    A standard allowance that most toolmakers I've worked with use, is 0.005" per side because it's convenient to add mentally without having to re-calculate dimensions with a calculator.
    I can't think of an occasion where I've had to toss a block because it had warped beyond beyond my ability to clean it up, and I've been toolbreaking for over 40 years. (but injection molds mostly, so not much D-2)
    Grinding 0.005" per side from D-2 with the wrong grinding wheel on 30 pieces will break your heart, so be sure to heed bosleyjr's advice on talking to your abrasive supplier and getting the best wheel possible for the grinding operations

    With regard to swelling and tapped holes too small after HT; be very very careful about just grabbing the oversize tap and going to town on it.
    The vast majority of D-2 is probably still made into punch tools, and in that instance it's perfectly OK to have the mounting bolts a bit loose, but if this is not going to be part of a punch tool, make SURE it's OK to tap oversize before you commit, by contacting your customer first, as hobbyshop recommends.
    If you need the threaded bores to be close tolerance, for some weird reason or other, you must plan to threadmill after HT, in which case you can threadmill before HT leaving stock and then go in again after HT.
    If you must threadmill do not try to pre-tap...it's gonna be a major battle to pick up the thread to re-work it after HT, so be clear on that part of your strategy before you start work on the parts.

    It's also possible to post HT tap with a carbide tap...I've seen it done successfully, but I've also seen it fail spectacularly, and carbide taps cost a bloody fortune.

    All in all, I wouldn't be too afraid of this part...it'll probably be just fine...leave 0.005" per side on all critical dimensions and just take a chance on it...it'll be a pretty safe bet.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

    Oh yeah:
    I concur with those who've recommended making a few extra just in case.
    However, I've recently started contacting my customer first, making the recommendation and telling them the reason for this, and offering the extra parts as part of the contract if they all work out before I make the extra parts.
    If they say OK, it's a bonus for me and often for them too.
    If they say NO, then I know whether I'm going to eat the extra cost beforehand and can decide whether to take the chance or not.
    I find customers respond way better when I offer the option BEFORE the parts are made...it shows I care about their contract and want to do a good job for them.
    About 50% of the time, my customers go for it and everyone wins

  3. Likes AD Design liked this post
  4. #23
    Join Date
    Oct 2011
    Location
    West-Central Illinois, USA
    Posts
    1,276
    Post Thanks / Like
    Likes (Given)
    2024
    Likes (Received)
    582

    Default

    Quote Originally Posted by bosleyjr View Post
    Get yourself a copy of the vintage "Carpenter Matched Tool and Die Steels" booklet.
    HT at 1850 and tempering at 450 was predicted to give you about 0.00025" per inch increase in dimensions.
    Quote Originally Posted by bosleyjr View Post
    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.

    *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. Worth picking up a copy from eBay.
    Yup!^

    Ohhhh! I forgot about Carpenter they smoothed that bump a bit at 450F° temper by 1986 (still looks like .00025" though). Carpenter (D2) temper slope & bumps attached from 1967,77 & 86 then 86 continues adding wear numbers and other slight changes from prior catalogs.

    I usually like Crucible docs (complete isothermal charts) but they don’t discuss THIS particular characteristic with D2 or how to deal with it.

    Good luck,
    Matt
    Attached Thumbnails Attached Thumbnails carpenter_0610_1967.jpg   carpenter_0610_1977.jpg   carpenter_0610_1986.jpg   carpenter_0610_1988_pg2-3.jpg   carpenter_0610_1988_pg4-5.jpg  


  5. #24
    Join Date
    Jun 2012
    Location
    Tennessee USA
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    353
    Likes (Received)
    417

    Default

    I agree with what others have posted. I've always used .005 per side, total of .010 for OD/ID in this case, as a convenient and safe number when the cross section is fairly uniform. You didn't mention whether the bore is blind or though. If the cross section changes a lot, blind bore meets flange for example, then the advice of rough machining/stress relieving/finish machining (leaving material for grinding) is good advice in light of "Failure not an option". Double or even triple tempering of D-2 is considered a better practice. Use a reliable heat treat company with a good name, it's worth the extra money for a reliable service in this instance. Somebody mentioned using a CBN wheel. They work well for jig grinding D-2 but may be cost prohibitive for OD/ID grinding. I've only used ceramic wheels in a surface grinder with a speed control (VFD) and coolant with good results at lower cost. I have limited experience with OD/ID grinding pieces larger than I could set up in a spin fixture on the SG. Controlling heat in the work piece per wheel condition merits your attention. A glazed wheel will thermal expand and/or burn the work surface in short order. You'll feel more confident on the second or third piece when you know what to expect and what you can do about it. If you are doing 30 or so pieces you may want to employ a rough grind/finish grind strategy, dressing the wheel (if not CBN) in between sets so the wheel condition is more predictable. Hardened D-2 does NOT stick to a mag-chuck well enough to trust it. Either hold in a grinding vise or block it in real solid. It may seem to hold but it will not. Good luck.

  6. #25
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    535
    Post Thanks / Like
    Likes (Given)
    257
    Likes (Received)
    421

    Default

    Quote Originally Posted by Matt_Maguire View Post
    Yup!^

    Ohhhh! I forgot about Carpenter they smoothed that bump a bit at 450F° temper by 1986 (still looks like .00025" though). Carpenter (D2) temper slope & bumps attached from 1967,77 & 86 then 86 continues adding wear numbers and other slight changes from prior catalogs.

    I usually like Crucible docs (complete isothermal charts) but they don’t discuss THIS particular characteristic with D2 or how to deal with it.

    Good luck,
    Matt
    The old Crucible book is sitting right behind me for when I forget what I've memorized.

    Anywho, to the original OP. 0.005 over for that size and you'll be ok. Also, unless your print requires you to have hrc 60 (which is harder than any D2 detail needs to be), I'd draw it twice back to 58.

    And yes, D2 eats rocks, hell it eats most anything.

  7. #26
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Update*
    Thank you all for your advice. What a great community! I read through each of your posts and have developed a game plan I feel confident in.
    I finally got a response from the man "in charge" at my local HT facility. His remarks as follows:
    "The D-2 when hardened, quenched, double tempered to 58/60 HRC will grow about 0.0003” per inch of dimension. The process we perform is in a vacuum furnace for hardening followed by a gas fan cool in the chamber. No scale or discoloration. Distortion will be very little due to the part symmetry and processing. We will double temper in air for maximum stability in function. This will produce discoloration and with come clean with a glass bead or scotch bright clean."
    I sent him my prints so he was able to review them.

    This is my first attempt at the tool and die world. Crunching the numbers I will break even on this job, but man I have a lot of cool new tools! This job got me in at a large nation wide manufacturer so fingers crossed this job goes well and leads to many more.
    Thanks all! Happy Thanksgiving!!


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
  •