Final machining flame cut hole
Close
Login to Your Account
Results 1 to 18 of 18
  1. #1
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    10
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Final machining flame cut hole

    Hey I've got a potential job lined up for 1-1/4 thick A36 flame cut plate, it's got a 2.5" hole that's been flame cut through it and I need to machine it to final size. I've got about 300 of these to do, and I didn't want to chew through carbide endmills on the flame cut. I only need to take around an 1/8 off to get to final diameter, does anyone know a good way to do this? right now I'm thinking about using a boring tool holder or maybe anneal the plates before I machine?

    I've got a Hurco VM1 that I'm planning to use. any help would be appreciated.

  2. #2
    Join Date
    Apr 2007
    Location
    Pillager, MN
    Posts
    5,666
    Post Thanks / Like
    Likes (Given)
    1852
    Likes (Received)
    5122

    Default

    Are the parts already cut? Leave out the hole.................drill and plow through the material with some high speed tool paths..............................

  3. #3
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,655
    Post Thanks / Like
    Likes (Given)
    1214
    Likes (Received)
    3475

    Default

    You won't have any trouble milling through the flame cut on A36. I'd use a Garr coated 1/2 5 fl and let it rip.

  4. Likes Mtndew liked this post
  5. #4
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,599
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    614

    Default

    I would bore (circle interpolate helix down) the hole with an inserted endmill. Depending on the tolerance and finish required, you could potentially finish it with your last boring cycle.

    Flame cut sucks. Regardless.

  6. Likes neilho liked this post
  7. #5
    Join Date
    Sep 2011
    Location
    Langley, B.C.
    Posts
    1,606
    Post Thanks / Like
    Likes (Given)
    324
    Likes (Received)
    942

    Default

    First question is: Are the holes already cut? If you have a choice water-jet will cut the holes without leaving
    a HAZ (Heat Affected Zone). Annealing probably won't help much. Mild steel doesn't harden up that much; it's
    the carbon/slag build-up at the cut line that is tough on tools.

    When dealing with situations like this you're usually better off to have a bit more material to remove rather than
    less. If you have minimal material to remove the cutter is always working in the HAZ--not good. With a little extra
    material once you start the cut the cutter is working in unaffected material and breaking through the HAZ from the
    back side. The cutting edge still has to pass through the HAZ but it always seems to cut easier this way. You
    definitely don't want to climb cut...

  8. Likes Jashley73, doug925 liked this post
  9. #6
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,249
    Post Thanks / Like
    Likes (Given)
    407
    Likes (Received)
    1634

    Default

    Quote Originally Posted by Fal Grunt View Post
    I would bore (circle interpolate helix down) the hole with an inserted endmill. Depending on the tolerance and finish required, you could potentially finish it with your last boring cycle.

    Flame cut sucks. Regardless.
    ^^^ That's how I would do it.

    If the OP uses an endmill, I'd conventional the first pass around- it'll get under the crap and be easier on the cutter.

    edit:
    Quote Originally Posted by LKeithR View Post
    ...You definitely don't want to climb cut...
    Lol. beat me to it. Agree, climbing will eat up cutters.

  10. Likes Jashley73 liked this post
  11. #7
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,996
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    Quote Originally Posted by tyleradambrown1 View Post
    Hey I've got a potential job lined up for 1-1/4 thick A36 flame cut plate, it's got a 2.5" hole that's been flame cut through it and I need to machine it to final size. I've got about 300 of these to do, and I didn't want to chew through carbide endmills on the flame cut. I only need to take around an 1/8 off to get to final diameter, does anyone know a good way to do this? right now I'm thinking about using a boring tool holder or maybe anneal the plates before I machine?

    I've got a Hurco VM1 that I'm planning to use. any help would be appreciated.
    .
    sure take a minute to remove any big pieces of slag and carbide end mills normally can handle the rest.
    .
    i wouldnt waste a hour or much money when a few minutes with a grinder removing slag is alot faster and cheaper

  12. #8
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,249
    Post Thanks / Like
    Likes (Given)
    407
    Likes (Received)
    1634

    Default

    Quote Originally Posted by DMF_TomB View Post
    ....i wouldnt waste a hour or much money when a few minutes with a grinder removing slag is alot faster and cheaper
    OP has 300 pieces to do. The right strategy is to approach it in a way that minimizes hand work and still allows a decent tool life.

    Hand grinding 300 parts is not the way...

  13. #9
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    10
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    What do you guys think about doing a first pass with HSS and then running carbide to finish? just basically sacrifice the HSS to take out that slag?

  14. #10
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    10
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Unfortunately they are already cut, that's what I was thinking also.

  15. #11
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,249
    Post Thanks / Like
    Likes (Given)
    407
    Likes (Received)
    1634

    Default

    Quote Originally Posted by tyleradambrown1 View Post
    What do you guys think about doing a first pass with HSS and then running carbide to finish? just basically sacrifice the HSS to take out that slag?
    You can do it, but it will be slow.

    I have a 3/4" Kennametal 2-flute indexable that would make short work of that hole. With 300 pcs, the tool pays for itself in time saved...

  16. #12
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,599
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    614

    Default

    Quote Originally Posted by tyleradambrown1 View Post
    What do you guys think about doing a first pass with HSS and then running carbide to finish? just basically sacrifice the HSS to take out that slag?
    If you have a bunch of HSS laying around with no purpose other than to burn up... I guess?

    To me it wouldn't be worth the time changing tools.

    Without knowing more specifics as to the economics of the job, it would be hard to make that judgment call.

    If it were my job, I would be looking at buying a high feed inserted endmill, most brands have them, you can get a body and a pack of inserts for less than $300. Thats $1 per plate.

  17. #13
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    325
    Post Thanks / Like
    Likes (Given)
    61
    Likes (Received)
    92

    Default

    Quote Originally Posted by Fal Grunt View Post
    If you have a bunch of HSS laying around with no purpose other than to burn up... I guess?

    To me it wouldn't be worth the time changing tools.

    Without knowing more specifics as to the economics of the job, it would be hard to make that judgment call.

    If it were my job, I would be looking at buying a high feed inserted endmill, most brands have them, you can get a body and a pack of inserts for less than $300. Thats $1 per plate.
    I agree with this. If Mitsubishi is still running their promo, buy a couple packs of inserts for an AJX, get the body for "free", and have at it. You'll make really quick work of the roughing and the inserts for running hardened material last forever and a day.

  18. #14
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    591
    Post Thanks / Like
    Likes (Given)
    123
    Likes (Received)
    656

    Default

    This is embarrassing to admit, but I had a similar problem years ago. I had them leave about .100" to cleanup. Then I took a cheap ass Chinese Fly Cutter and ground cemented carbide cutters by hand and eyeballed them until the were about right for diameter. Then I bored straight down to take out the HAZ, then finished the bore with a carbide endmill. Every once in a while, I would bump out the bar and re-grind the carbide. It was old school and crude, but it got the job done. It was kind of fun, since I could alter my eyeball grind and see the change in spindle load and surface finish. Total tooling cost on the job was a couple of bucks.

  19. Likes kenton, sfriedberg liked this post
  20. #15
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,468
    Post Thanks / Like
    Likes (Given)
    4064
    Likes (Received)
    2648

    Default

    I've never had an issue cutting A36 flame cut burnouts.
    Stuff cuts like butter.

  21. Likes Larry Dickman liked this post
  22. #16
    Join Date
    Jan 2003
    Location
    Posts
    284
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    65

    Default

    Quote Originally Posted by Fal Grunt View Post
    I would bore (circle interpolate helix down) the hole with an inserted endmill. Depending on the tolerance and finish required, you could potentially finish it with your last boring cycle.

    Flame cut sucks. Regardless.
    Id do it the exact same way, ramp down with insert endmill. I like using Sandvik R390s for this, it will have no problem with flame cut mild steel. You can use the same tool at 2-3 different depths to finish depending on size of insert or use a long endmill in one pass if you dont want to see the steps.

    Use a carbide insert double angle cutter to chamfer the top and bottom all in the same setup. Wont have to touch a thing in terms of removing slag before hand or burrs after.

  23. #17
    Join Date
    Apr 2006
    Location
    Austin, TX
    Posts
    1,730
    Post Thanks / Like
    Likes (Given)
    182
    Likes (Received)
    442

    Default

    We ran some parts that were flame cut "A36". Some cut like butter and other pieces cut like crap. Ended up running a high speed roughing pass using a Mitsubishi "feed mill" that used the little button style cutters. Ran them as fast as they would go with something like a .030" DOC and they did great. Finished the parts out with .5" 5 flute mill running a high speed path. Parts were eventually switched to A514 and AR500 that was jetted and they still cut well using this strategy.

  24. #18
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,945
    Post Thanks / Like
    Likes (Given)
    6848
    Likes (Received)
    2472

    Default

    Conventional mill. Find some decent carbide endmills meant for semi-roughing, or use the inserted/indexable endmills, and helix down. But always conventional milling.

    Once you cut away the flame cut, then sure - climb-mill away...


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
  •