Slot milling w/ .0312 endmill


Results 1 to 19 of 19

Thread: Slot milling w/ .0312 endmill

  1. #1
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default Slot milling w/ .0312 endmill

    I'm milling 6 .04 wide slots, equally spaced, on a 5/16 dia part. The slots are about .052 deep. Material is 17-4ph. Not hardened yet.
    Roughing with one end mill, finishing with another. Finisher still going, roughers lasting 1.5 parts. Both endmills are 4 flute stubs (tried 2 flute std but it broke right away).
    My attempts are 11,000 rpm, 1.5 ipm, .015 doc
    11,000, 1.0 ipm, .015 doc
    11,000 1.0 ipm .01 doc
    9,000, 1.0 ipm, .01 doc
    Can somebody help?

    edit: sorry. using carbide endmills

    Similar Threads:


  2. #2
    Registered beege's Avatar
    Join Date
    Feb 2008
    Location
    USA
    Posts
    586
    Downloads
    0
    Uploads
    0

    Default

    Might work better as hardened. 17-4 cuts better at H900, H950, etc. You aren't going to get that tool up to the proper speed, so the speed you are going isn't going to matter much. I'd rough slower, though, maybe .7ipm, two or three flute stub.



  3. #3
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Thanks, I'll try slower next part.



  4. #4
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    I don't think this stuff comes in "non-hardened" condition , not that I've yet had a project that called for it.

    http://www.aksteel.com/pdf/markets_p...Data_Sheet.pdf

    Even condition A is Rc35

    Anyways, this type of difficult slotting is something that I use OneCNC's high speed toolpath for. I checked to be sure, and yes, it will create a looping toolpath with a .031 diameter tool, down a slot .040 wide with .001 finishing allowance. The advantage is avoiding that full width tool engagment that is so hard on a tiny little tool.

    I mention this because many people are not familiar with the concept and think nothing else is possible but full width cutter engagements to open up a slot.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  5. #5
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Lol, ok, ok, I meant it gets even harder later.

    Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?



  6. #6
    Registered
    Join Date
    Sep 2005
    Location
    usa
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default 17-4PH

    I have machined this successfully with Destiny tools. I was using a 1/2 dia endmill going 1/2 deep with a full engagement at 1000 RPM and 30 IPM.
    Walked right thru it and made literally not a bit of noise.



  7. #7
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by extanker59 View Post
    Lol, ok, ok, I meant it gets even harder later.

    Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?
    Drill a plunge point or helix down into it, since you'd have to cope with the conical drill point at the bottom anyways.

    Perhaps you can draw your own looping toolpath. If you have cadcam software, you can draw a series of overlapping circles....just enough to make two complete tool circuits in the loops, trim the entities to save just what you need, then copy and paste enough copies end to end to make the length of the slot. Then use some simple cut chain type operation on them.

    IIRC, someone on these forums may have written some kind of a macro to do this type of machining on simple shapes.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  8. #8
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    1389
    Downloads
    0
    Uploads
    0

    Default

    I dont know what type of endmills your using but dont go more than a .025 pass with a endmill that small. I am guessing .015 tops.
    a stub endmill will help big time and you may be able to go deeper.

    No offence to huflungdung, but dont drill a spot hole you will break more endmills on small slots like that. the burrs get in the way and grab the tool into the part

    I dont know your situation as sometimes you have to use a endmill, but personally I would be using a slitting saw not an endmil. even if it requires a second op the slitting saw is the only way to go.

    also dont forget the smaller the endmill dia. the better the tool run out must be, you can get by but you have to cut your speeds in half if you have too much runout.



  9. #9
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Oops, no offence taken, but I could have specified to drill a plunge point with a spot drill A ramp into the cut would be better except that it is still a full width entry.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by extanker59 View Post
    Lol, ok, ok, I meant it gets even harder later.

    Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?
    Is it a straight slot?

    Do it the old fashioned way, something like 30 lines of code and about 30 minutes to write it.

    Have a look here: http://www.cnczone.com/forums/showth...t=73902&page=4

    Posts 67, 73 and 74, code is in Post 73 all you need to do is delete the multiple subroutine calls, change a few coordinates and feeds.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  11. #11
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    1389
    Downloads
    0
    Uploads
    0

    Default

    Understood, I guess I could have read it better too.

    I had the same part almost funny, cause it was the same dia ( had a thru-hole) same slot size. depth I think was like .060 -.001 +.000. .304ss 303ss and 17-4 ph
    I ran hundreds of them, most boring job in the world and the slowest by far.
    I had a cam system so I just programmed a non stop loop for the slots speed it up on the no cutting parts slowed it down on the cutting parts in the program.

    anyhow. I tried everything including drilling a ton of holes in the slots to take out the material and what I found was that the burr edge would suck into the cutter and snap me off.

    even put them on a 4th axis to rough the slots, then turn it up to finish didnt work either cause the rad. when the 4th was at a ninety causes burrs and snapped me off when the 4th was upright.

    the 303 wasnt that much easier like I thought it would be.



  12. #12
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    1389
    Downloads
    0
    Uploads
    0

    Default

    heres a pic of another one this one I believe was either 15-5 or 17-4 could be 303( dont have my glass's on) I ran it in 1999,
    just happened to be doing some cleaning over the weekend and saw about 60 scrapped ones in a box and tossed them.

    they are scrap cause they needed a .003 max rad on every side and the operator wasn't paying attention to the O.D. dia. it was easier to scrap them then debur them.

    Delw

    Attached Thumbnails Attached Thumbnails Slot milling w/ .0312 endmill-img_1725a-jpg  


  13. #13
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Hey, thanks guys.
    We used saws before but when I tried the end mill they liked the result better. It is really an EDM job if you ask me (thru slots with a lolipop shape at the end).
    I am able to plunge outside the part so no pilot drill needed. I have no problems with this material but the size of the tool is giving me fits.
    We're a small shop and the job is over half done so the tools on hand are what we are going to use.
    I might try that overlapping arc idea. Only need to make one arc in cam then step it in. Interesting.
    Thanks to all who responded.
    I'm currently trying 9000 rpm and .8 ipm. Man this is a long job.
    The tools are osg 4 flute carbide stub. We have 4 double ended ones left for 8 parts.



  14. #14
    Registered
    Join Date
    Mar 2009
    Location
    USA
    Posts
    133
    Downloads
    0
    Uploads
    0

    Default

    If you run a 4 flute endmill at 11K and 1 ipm that's a chip load of only .00002. That's more like grinding than cutting.

    11k Rpm
    .00013 chip load = 5.72 ipm

    I'd back off your depth of cut rather than slow your feed down so much. Try taking .003 DOC. The bottom line is that the endmill needs to cut, not rub itself to death. I'd much rather take a small DOC than a deep one at a super slow feed rate.

    You didn't say what kind of machine, tool holders or coolant you're running.

    We run .031 4 flute TiALN coated endmills in 17-4 h900 every day.



  15. #15
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Thanks John,
    It's a Haas VF-2ss with synthetic coolant holding a ER-11 (non-high precision collets). Total run out close to .001!
    In the last hour I've boosted the feed up to 1.4 ipm at 6000 rpm. When I went slower the end mill broke sooner- rubbing like you said.
    They only break on the slotting (roughing) operation.
    .003 doc? Ok, I'm game.
    Next part I'm going 5ipm, 11,000 rpm, and .003 doc.
    Or do you think that with the TIR being sloppy that I should go slower?
    High precision collets will be ordered but won't get here before the end of the job.
    Thanks for your insight.



  16. #16
    Registered
    Join Date
    Mar 2009
    Location
    USA
    Posts
    133
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by extanker59 View Post
    Thanks John,
    It's a Haas VF-2ss with synthetic coolant holding a ER-11 (non-high precision collets). Total run out close to .001!
    In the last hour I've boosted the feed up to 1.4 ipm at 6000 rpm. When I went slower the end mill broke sooner- rubbing like you said.
    They only break on the slotting (roughing) operation.
    .003 doc? Ok, I'm game.
    Next part I'm going 5ipm, 11,000 rpm, and .003 doc.
    Or do you think that with the TIR being sloppy that I should go slower?
    High precision collets will be ordered but won't get here before the end of the job.
    Thanks for your insight.
    .001 is a lot of run out. You may be able to monkey around and tap it in to run a little better. Get everything cleaned up as best you can. Inspect the holder and collet and endmill shank with a microscope or whatever you've got to magnify. Clean your spindle taper. A tiny bit here and a tiny bit there adds up to run out. Make sure your collet isn't damaged from a previous tool break. Take advantage of everything that is in your control.

    If your endmill is taking a proper chip it will work better. The next thing you can control is the DOC. A .031 EM can't take all that much side load so you're forced to take a small DOC. Maybe you can take .010 with your set up, maybe only .001. There are a lot of variables so you've got to play around and figure out what works. Remember the endmill must be cutting and not rubbing. Doesn't matter if your endmill is .005 or 5.00 inches.

    Try not to get frustrated and start making radical changes back and forth. Sometimes cutters break and people get pissed and then quickly load a new tool without getting things cleaned up and properly reset. (of course I've never done that ;-) )



  17. #17
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Makes sense. Trying it now. Will post results.
    Thanks again John



  18. #18
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    OK, well, I like the results better than before. Unfortunately the number of pieces that were left didn't let me experiment more so my results are not sure.
    I had 5 pcs left when I switched to 11000 rpm, 5.72 ipm, .003 doc, with my 1/32" 4 flute stub end mill.
    The end mill was already used on one part (6 slots) at the slower feed rate so it was most likely dull.
    Even so it lasted almost 3 parts. It broke on the last slot of the 3rd part.
    The next end mill went through the last 2 pcs but I don't know how long it would have lasted.
    If I get this job again I'm definately going the faster feed rate and lower doc.
    Thank you very much to all who helped.



  19. #19
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Sorry for bringing this one back but I thought a little update might help somebody else with this problem.
    We got the job back finally and I ran it with a 1/32" regular length 4 flute endmill (it's what we had) at 11000 RPM, 5 IPM, and a DOC of .004
    The part is a 3/16 diameter 64 ELI titanium tube- about .03 wall- 3 slots per part- held in a rotary on our Haas.

    It went through the 25 pieces we had to make- about 34 linear inches of slot total. Worked well. Tool still ok.
    Thanks again. Great help here.



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Slot milling w/ .0312 endmill

Slot milling w/ .0312 endmill