Some assistance please with 1045
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 31
  1. #1
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    568
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    193

    Default Some assistance please with 1045

    I have a 1510 ford tractor and the valve rocker arm is busted. The part does not exist because it was a low production machine and OEM parts are no more. Can't locate the part at several very large ford tractor junk yards across the country.

    So, I want to make the rail myself. I searched google and a nice topic from practical machinist came up saying use 1045 since its already designed for the job.

    I ordered a piece and started playing with it last night. Now I normally machine 303,304,316 stainless in my manual machine. 17" south bend tornado. I see this stuff almost burns as it cuts.

    So I'm not trying to blow a ton of money on Tooling to figure out 1 small project that I may never do again. Problem is I want the tractor back so I can clean up my yard for a party in a month and machine shops aren't going to get it done for me. Which I understand, hence why I'm going to do it.

    I ordered the tube from Mcmaster with a close enough id and I need to turn the OD from 0.75 to 0.668.

    Any help on tooling and speed/feeds would be very helpful.


    Sent from my 2PS64 using Tapatalk

  2. #2
    Join Date
    Dec 2009
    Location
    Louisiana
    Posts
    425
    Post Thanks / Like
    Likes (Given)
    141
    Likes (Received)
    240

    Default

    these low carbon steels need a decent depth of cut to get a shear going other wise they just tear and leave an awful surface finish. If light cuts are all you can do I'd recommend grinding your HSS bit very sharp at a positive angle and cut in oil.

  3. Likes Gobo liked this post
  4. #3
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    385
    Post Thanks / Like
    Likes (Given)
    125
    Likes (Received)
    215

    Default

    I would use sharp tooling with lots of relief, such as an insert intended for aluminum. I would also try to keep the sfm down to keep from tearing up the cutting edge.

  5. #4
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,632
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    760

    Default

    1045 "burns"? Induction hardened by any change?
    Can you be more specific? It should be really easy to machine and not overly picky of anything.

  6. Likes Mtndew liked this post
  7. #5
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2609

    Default

    4140 steel is a popular steel

  8. #6
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,632
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    760

    Default

    Quote Originally Posted by DMF_TomB View Post
    4140 steel is a popular steel
    You won't solve anything by switching from 1045 to 4140 machinability vise. Better just sort out the original problem.

  9. #7
    Join Date
    Jan 2005
    Location
    Houston
    Posts
    5,513
    Post Thanks / Like
    Likes (Given)
    475
    Likes (Received)
    2345

    Default

    1) A photo sure would be nice.

    2) Are you making a rocker arm or a rocker arm shaft? It sounds like a shaft you are making but clearly you refer to it as a rocker arm. The rocker arm is the thing that...rocks...and pushes on the valve tip. The shaft is the cylindrical tube that the rocker might or might not pivot on.

    3) 1045 is pretty easy to machine as far as steels go. If it's 'burning' that gets a WTF.

  10. #8
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,632
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    760

    Default

    Any change that your "tube" is this?
    Hollow Linear Motion Shaft
    Last edited by MattiJ; 05-09-2018 at 01:08 PM. Reason: Goddammit, linking to MCM can be "#%"#¤

  11. #9
    Join Date
    Mar 2017
    Country
    LATVIA
    Posts
    300
    Post Thanks / Like
    Likes (Given)
    76
    Likes (Received)
    163

    Default

    MattiJ is probably right

    by "burns" OP probably means glowing chips, which in turn will mean that the 1045 in question is hardened, and razor sharp HSS will be of no use there, carbide will do the job, but might need a follower rest if that shaft has some legth to it

  12. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2609

    Default

    Quote Originally Posted by MattiJ View Post
    You won't solve anything by switching from 1045 to 4140 machinability vise. Better just sort out the original problem.
    .
    i machined plenty of prehardened 4140, not super hard and usually fairly high strength. i have known engineers who often asked for it
    .
    machines ok with carbide. might have some tapping problems other wise it machines ok

  13. Likes Gobo liked this post
  14. #11
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    568
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    193

    Default

    Wow, overworked and unappreciated by my customers and 2 kids, take your pick at what connects to what.

    Yes it's the 52100 from Mcmaster. I'm working in a 1045 part for another machine of mine and switched info.

    Thanks for correcting me.

    Sent from my 2PS64 using Tapatalk

  15. #12
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,632
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    760

    Default

    Quote Originally Posted by Bondo View Post
    Wow, overworked and unappreciated by my customers and 2 kids, take your pick at what connects to what.

    Yes it's the 52100 from Mcmaster. I'm working in a 1045 part for another machine of mine and switched info.

    Thanks for correcting me.

    Sent from my 2PS64 using Tapatalk
    No wonder you have problems. It's a rock hard high carbon bearing steel.

    If you want to try carbide try reeally slow speed, like 100 sfm. Seco TH1000 grade has been recommended more than once over here.

    Or go to Ceramic or CBN and let the fiery orange hot chip fly! time to read up on "hard turning".

  16. #13
    Join Date
    Jan 2005
    Location
    Houston
    Posts
    5,513
    Post Thanks / Like
    Likes (Given)
    475
    Likes (Received)
    2345

    Default

    If you are making a shaft, I think the guys who do it start with unhardened material then harden it after...maybe a final grind is all they do after hardening.

  17. Likes 72bwhite liked this post
  18. #14
    Join Date
    Sep 2012
    Location
    California, Ventura county
    Posts
    1,407
    Post Thanks / Like
    Likes (Given)
    256
    Likes (Received)
    602

    Default

    that's a tough one trying to turn woodpecker lips hard material
    what you need is a grinder

  19. #15
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    953
    Post Thanks / Like
    Likes (Given)
    1093
    Likes (Received)
    612

    Default

    MattJ is in the ballpark on 100sfm. Low depth of cut like .02" starting at .003"-.004"/rev.

    This is where I would start anyways. A decent steel grade WNMG TiAlN coated insert should be able to get the job done for ya.
    Last edited by AARONT; 05-09-2018 at 05:20 PM. Reason: Added insert style

  20. #16
    Join Date
    Mar 2005
    Location
    Northwest Indiana
    Posts
    3,920
    Post Thanks / Like
    Likes (Given)
    631
    Likes (Received)
    720

    Default

    Might not be the way to go if that linked tubing is what you've got. The link says it's case hardened. By the time you cut it down to the diameter you need you will probably lose a lot of that hardness. Depends on the depth of the case. Might be better off roughing it down close and getting it heat treated again - leaving just a bit for finish grinding or turning - I'd advise grinding seeing the length and wall thickness. Unless the rockers pivot on a bearing, in which case you don't need that hard of a shaft. If they pivot directly on the shaft then you'll probably want it pretty hard.

  21. #17
    Join Date
    Jun 2008
    Location
    TN
    Posts
    1,545
    Post Thanks / Like
    Likes (Given)
    323
    Likes (Received)
    250

    Default

    A picture of the old part would be very helpful!

  22. #18
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    568
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    193

    Default

    Quote Originally Posted by henrya View Post
    A picture of the old part would be very helpful!
    Wow, now I feel stupid... Yeah that would help. When I get back to the shop I will take a picture

    Sent from my 2PS64 using Tapatalk

  23. #19
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2609

    Default

    again 4140 preharden is often used to make parts and no other heat treatment needed. its moderately hard so carbide works better. it can be moderately difficult to drill and tap with hss but it normally can be done

  24. Likes DJ2 liked this post
  25. #20
    Join Date
    Apr 2004
    Location
    Shandaken, NY, USA
    Posts
    4,263
    Post Thanks / Like
    Likes (Given)
    1131
    Likes (Received)
    6715

    Default

    This may be "locking the barn door after the horse has run out", but: have you checked the hardness of the original/broken part ? Without going into a formalized hardness test, checking the undamaged portions with a file and center punch should give an idea if the rocker shaft is hardened. If you have a fractured surface, try your center punch across it, working from the outer circumference in towards the center bore (rocker shafts usually being made hollow). This will tell you if the shaft was through-hardened or surface (aka "case") hardened.

    A spark test done on a bench grinder can also give a rough determination of carbon content and alloying elements. If you take some specimen pieces of steels of known compositions and spark them first, then compare the rocker shaft's sparks, you can often get a pretty good idea of what basic elements and approximate carbon content in the shaft is.

    A rocker shaft usually has some holes drilled into it for locating it or for getting oil up to the rockers, so whatever you make the replacement shaft from has to be something you can drill and possibly ream or tap, depending on the design of the shaft. A soft steel which can later be hardened or surface hardened is what I'd use. Something like an 8620 which can be machined easily in its soft condition, and can be surface hardened with minimal distortion would be my choice. I'd send the shaft out to a commerical heat treaters after you machined it and have it surface hardened perhaps 0.020-0.030" deep. It is your call as to whether you want to leave a grinding allowance and finish grind the shaft to final outer diameter/straightness.

    For a rocker shaft in a tractor engine, I'd be OK with surface hardening at final diameter. I'd check the actual clearance of the rocker arms on the undamaged sections of the shaft, and if there is a couple of thousandths of clearance, I'd go with the shaft at final diameter before heat treating. I know from experience that some steels tend to "swell" or "grow" a bit when hardened or surface hardened. Usually, final grinding is called for, and this brings the hardened part to final dimensions, so this is not an issue. In your case, you may want to make the shaft maybe minus a half thousandth to allow for "swell" which sometimes occurs with surface hardening. I'd then polish the shaft with emery cloth and crocus cloth in the lathe and run with it.

    No disrespect to you or the tractor, but you are not making parts for a high speed high performance engine like a Ferrari or Maserati. Try to match the hardness and dimensions and you will be good to go without splitting the ten thousandths of an inch.

  26. Likes DJ2 liked this post

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
  •