525,666 active members*
2,475 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 26
  1. #1
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    MRR 4140HT (PH)

    I've got quite a bit of 4140HT left over from a customer project making some press dies a few years ago. I've been using it periodically for various projects. Its decent, strong, modestly hard steel for hand tools. Some of you may have seen the ER collet wrenches I made for my TTS tool holders. Well, I've got another project I'd like to do with some of it, and I need to remove quite a bit of material. A lot more than any previous project using this material. Even the press dies.

    My Hurco currently has a major issue with one of the axis. It suddenly in the middle of a job went from about 0.001" backlash in one axis to 0.037". Something in the screw failed catastrophically. Of course its the hardest screw to get to. I'll fix it eventually, but in the mean time I want to get this job done.

    With the PCNC1100 a 1/4 4 flute endmill taking a modestly deep cut and relatively small width of cut I can get theoretically around 0.99 CI^3. I don't know that I have run it that hard, but that 1/4 mill sounds really good in the 4140HT. When I plug numbers (with generic mills) into HSM advisor with 5/16, 3/8, and 1/2 I still only get about 1.07 CI^3. I've never really gotten good sounding cuts with the larger mills in the 4140HT although they rip through other steels like it isn't even there. The 1/4 inch Altin coated 4 flute seems to be the magic mill. Even on the larger more powerful Hurco mill.

    I'm looking at 20-24 CI material to remove per part, and I want to make 9 of them. I also need to cut a precise undercut with a T-slot cutter of some kind, but that's a secondary problem. Right now I am looking to see if I can get any better MRR for the bulk stock removal without killing my machine.
    Bob La Londe
    http://www.YumaBassMan.com

  2. #2

    Join Date
    Mar 2020
    Posts
    41

    Re: MRR 4140HT (PH)

    If you figure it out please post back up. I've been having a helluva time getting any kind of good results with steel. Granted I have no idea what I'm doing and I've discovered that the material I was working with most recently was not what I thought it was (some unknown grade of stainless rather than the 4140 I was expecting) so that all has a huge role to play in this. Even so, it would be nice to run a 3/8 tool instead of the 1/4 for a bit of extra rigidity. I have some new tools from Lakeshore Carbide that I have not tried yet and a couple blocks of (for sure) 1018 so I'm hopeful I will have better results this time around but in general I like the properties of 4140 and would prefer to use that whenever possible for my steel needs.

  3. #3
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    I was just reviewing an old video (2 actually) on cutting 4140 on the 1100 by John Saunders (NYCCNC) on YouTube. He used a 1/4" endmill for the entire test and according to his spreadhseet he maxed out at 0.74 CI^3 MRR. He also didn't specifiy, whether it was annealed or HT/PH. Unlike John I don't get freebies to test though. LOL.
    Bob La Londe
    http://www.YumaBassMan.com

  4. #4

    Re: MRR 4140HT (PH)

    Any idea on DOC, WOC, FPT?

    I have quite a large steel project coming up with my G0704 and am frankly lost where to start. I have TTS and a 2hp 6k spindle. But again, I am clueless in steel! I'm sure I'll have to go conservative compared to a Tormach, but any numbers will help.

  5. #5

    Join Date
    Mar 2020
    Posts
    41

    Re: MRR 4140HT (PH)

    I have watched that video repeatedly as well as the related one (he did an early video with mixed success and a later one with more success where he also talked about G10 L20). That video is the reason I bought the lakeshore carbide tools instead of the other stuff I've been experimenting with but I have a very limited supply of 1/4" tool holders and plenty of 3/8 so I broke from the example and got the size I'm used to working with for aluminum. If I'm still not successful with these tools I will end up getting some 1/4" so I can exactly replicate his setup but I'm hoping to avoid that. My biggest issue seems to be that the second I hear the chatter, the tool is already damaged (though not visibly) so even if I back off from whatever the chatter causing parameters were, I can't get a good cut from that point on unless I change the tool.

  6. #6
    Registered
    Join Date
    Oct 2008
    Posts
    1986
    Quote Originally Posted by CL_MotoTech View Post
    Any idea on DOC, WOC, FPT?

    I have quite a large steel project coming up with my G0704 and am frankly lost where to start. I have TTS and a 2hp 6k spindle. But again, I am clueless in steel! I'm sure I'll have to go conservative compared to a Tormach, but any numbers will help.
    A G0704 is certainly a lightweight
    , but a 2 horsepower spindle overpowers the Tormach 1100. I honestly don't think you could use two horsepower on that machine effectively. The only benefit I would think there is to that size motor is having a little more torque at lower RPMs. That depends on pulley ratio of course too.
    Bob La Londe
    http://www.YumaBassMan.com

  7. #7

    Re: MRR 4140HT (PH)

    I use mostly 4140 in my 770 , but I do small parts and don't remove tons of excess materials .

    But I've found that looking for a bigger tool isn't always the best solution for getting things done quickly .
    I like 3/16 and 1/4 inch tools . And I like to run them fast .

    For roughing with a 1/4" 4 flute tool I run it @ .200 doc with a .015 woc 9000 rpm and 40 ipm
    I think I could push it quite a bit faster but it sounds really happy in the cut .

  8. #8
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    I have to admit that I've found a 1/4 inch end mill to be my happy place for a lot of nice work.

    I'm just looking at MRR in 4140 for one project. I ordered some 3/8 coated roughers to play with. Once I get the bulk of the materials out I'll probably finish with the 1/4" 4 flute altin coated mills. They do a really nice job.

    Have to remove around 20 ish cubic inches in the first major operation. Then a couple more inches in secondary operations before finishing.

    If I have good results that push significantly beyond what John did in those old videos I'll let you know. I should be able to get upto 1.77CI / 1.78CI in theory. If I can get a real 1.3 or better I'll be thrilled. I played with a lot of numbers and tried to keep the mill in the low to mid 3000 RPM range. I'm looking at surface speeds around 330-340 with as much load as I can put on the cutter without over coming its torque limits or maxing out the mill spindle.
    Bob La Londe
    http://www.YumaBassMan.com

  9. #9
    Registered
    Join Date
    Apr 2016
    Posts
    106

    Re: MRR 4140HT (PH)

    Quote Originally Posted by Bob La Londe View Post
    I have to admit that I've found a 1/4 inch end mill to be my happy place for a lot of nice work.

    I'm just looking at MRR in 4140 for one project. I ordered some 3/8 coated roughers to play with. Once I get the bulk of the materials out I'll probably finish with the 1/4" 4 flute altin coated mills. They do a really nice job.

    Have to remove around 20 ish cubic inches in the first major operation. Then a couple more inches in secondary operations before finishing.

    If I have good results that push significantly beyond what John did in those old videos I'll let you know. I should be able to get upto 1.77CI / 1.78CI in theory. If I can get a real 1.3 or better I'll be thrilled. I played with a lot of numbers and tried to keep the mill in the low to mid 3000 RPM range. I'm looking at surface speeds around 330-340 with as much load as I can put on the cutter without over coming its torque limits or maxing out the mill spindle.
    I use a lot of 5/16 and 3/16 for Titanium, 17-4, and 4140 on my 770.

    The 5/16 is already pushing where machine rigidity and power can take a deep enough cut and also not chatter. 4 flute 5/16 Tialn running between .3 and .5 DOC with a WOC somewhere between say .014 and .028 gives pretty smooth cutting results on adaptive clearing. How hard you can push without brutal chatter will depend on the machine. Your 1100 may be a bit better for that than the 770. If you go too little on DOC when side milling hard materials with the 4 flute the cut gets realllllly rough and noisy because the cutting edges aren't constantly engaged. At that point best to switch to a full WOC and shallow DOC instead.

    But oddly I've had better luck with the 4 flute end mills than 5 for hard materials. I suspect it has to do with amount of cutting edge engaged at once and machine rigidity.

  10. #10
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    Yeah, I bought into the 5/6 flute hype a while back, but I found that as long as my cuts are reasonable i get a lot better results with 4 flute. I think I posted some video about slotting with a 1/4 inch 4 flute AlTiN coated in 4140HT a while back. I think the slot depth was only .0905, but it was moving right along and sonded really good. The big helper for me was a simple air blast.
    Bob La Londe
    http://www.YumaBassMan.com

  11. #11

    Re: MRR 4140HT (PH)

    Quote Originally Posted by Bob La Londe View Post
    A G0704 is certainly a lightweight
    , but a 2 horsepower spindle overpowers the Tormach 1100. I honestly don't think you could use two horsepower on that machine effectively. The only benefit I would think there is to that size motor is having a little more torque at lower RPMs. That depends on pulley ratio of course too.

    I regularly run at or close to 5 cu. in.^3 in aluminum. I get nice operation with little issue. I'm not sure I am over powering much of anything. I run it 1:1. though I have run overdrive to achieve 8k at spindle.

    I'll probably give a three flue a try in steel because that's what I mainly have in the box.

  12. #12
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    Aluminum is pretty easy once you have found your way of eliminating chip welding. 5 Cu^3 is about 1.3 HP.

    Really your material removal rate in aluminum is limited by machine speed, horsepower, and rigidity. If you have flood coolant its otherwise nearly unlimited.

    I wouldn't use a 3 flute in steel because all of my 3 flutes are optimized for cutting aluminum with 40 to 47 degree helix angle and razor sharp cutting edges that just can't take the stress and the heat.

    I also found I got much better results cutting dry with coated endmills and air blast in steels. Some report good results flooding steel, but they have machines with a zillion nozzles and pumps with rates measured in gallons per minute. Not gallons per hour. They never experience thermal shock because there is a ton of coolant being blasted at the cutter. None of that is absolute though. I d work on the high speed spindles that just has to have flood coolant even in steel.


    But of course this thread is about what can be done with a Tormach 1100 with its 1.5 HP spindle.
    Bob La Londe
    http://www.YumaBassMan.com

  13. #13
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    Almost forget. My 3/8 4 flute AlTin coated roughers arrived yesterday. Hopefully I'll have some time to push one to failure and have some results to report back.
    Bob La Londe
    http://www.YumaBassMan.com

  14. #14

    Join Date
    Mar 2020
    Posts
    41

    Re: MRR 4140HT (PH)

    Well my tests with the 3/8 lakeshore carbide tools and 1018 steel finally happened yesterday and were a pretty miserable failure. I honestly don't know what my issue is. 250SFM on one tool 450 on the other. .25DOC, .05 WOC, .0016ipt. Worked fine for a couple passes than halfway through a cut starts screaming like a wounded pig. Cutting edge and corners appear to be fine but the as before, I can't get a cut without the tool screaming at me once it's happened the first time. 1/4" tools are on order now and I will be testing using the exact same recipe as saunders has posted as well as some of the postings here so hopefully i find something I can actually work with. This whole process has been truly discouraging so far. While I wait for the new tools to arrive I will be looking at my setup to see if I have something going on either in terms of loose fixturing, tool runout, or something because I just don't understand why I can't seem to make a chip in mild steel with this machine. I also have a microscope on it's way so i can better inspect the tools after they start chattering. Maybe that will give me some clue as to what is going on.

  15. #15
    Registered
    Join Date
    Jul 2011
    Posts
    248

    Re: MRR 4140HT (PH)

    Quote Originally Posted by soofle616 View Post
    Well my tests with the 3/8 lakeshore carbide tools and 1018 steel finally happened yesterday and were a pretty miserable failure. I honestly don't know what my issue is. 250SFM on one tool 450 on the other. .25DOC, .05 WOC, .0016ipt. Worked fine for a couple passes than halfway through a cut starts screaming like a wounded pig. Cutting edge and corners appear to be fine but the as before, I can't get a cut without the tool screaming at me once it's happened the first time. 1/4" tools are on order now and I will be testing using the exact same recipe as saunders has posted as well as some of the postings here so hopefully i find something I can actually work with. This whole process has been truly discouraging so far. While I wait for the new tools to arrive I will be looking at my setup to see if I have something going on either in terms of loose fixturing, tool runout, or something because I just don't understand why I can't seem to make a chip in mild steel with this machine. I also have a microscope on it's way so i can better inspect the tools after they start chattering. Maybe that will give me some clue as to what is going on.
    How much is your end mill sticking out past the chuck?

  16. #16
    Registered
    Join Date
    Oct 2008
    Posts
    1986
    Quote Originally Posted by upnorth View Post
    How much is your end mill sticking out past the chuck?
    that could be an issue, but if he's using something like fswizard or hsmadvisor tool stick out is one of the parameters that you enter.

    I would be curious to know what you use to clear chips and if you looked at the cutting edges before and after under any kind of magnification.

    I have started to favor a directed air-blast for steel cutting. You absolutely have to get the chips out of the cut. I have a 3X magnifying lamp that I use for inspecting cutters and if I'm not comfortable with that I have a small pocket microscope that I use.

    the other thing to look at is Cam. So often people use inefficient routines that excessively load the tool in the corner of cuts. I like to use a trachoidal path to remove the bulk of material when roughing and then use An almost tool wearingly slower feed for a cleanup pass. usually to clean up passes. One to clean up the nibs from the trochoid, and then the second to go to final dimension.

  17. #17

    Join Date
    Mar 2020
    Posts
    41

    Re: MRR 4140HT (PH)

    I had the 3/8 tool sticking out 1.2" which I know is pushing it but it was necessary to reach into where I needed to cut.

    I've been using a combination of GWizard and FWizard to figure my speeds and feeds but I've also been basing things on posted recipes that other people have used with success.

    For chip clearing I have flood coolant. I do notice that in deep, narrow pockets the flood isn't strong enough to clear things out and I will eventually be adding air blast or some other method to better deal with that but for now my issues have been happening even on open pockets and exterior profiles where I can clearly see good chip evacuation.

    I don't yet have anything to magnify the cutting edge for inspection but that changes tomorrow. Ordered a digital microscope that is supposed to be capable of 1200x magnification (doubtful but whatever it does will be better than naked eye for sure). Once that arrives and I get it set up I'll be going back to my old tools to see if I can identify any points of failure.

    CAM wise, I use fusion exclusively at the moment. I had access to solidworks cam for a while but that access has gone away and sw didn't have any kind of adaptive tool path anyway. Most of my pocket roughing is done with 2d adaptive followed by a 2d pocket and/or 2d contour for a cleanup pass, always with a second pass as the first finish pass never seems to get me quite to size but the second one will take that last 1-2 thou.

    On the better side of the news, I did get a 1/4 tool in yesterday and played with that for a bit. Same 1.2" stickout, 378 SFM per FSWizard game me 5778rpm. .0015ipt gave me 34.4ipm and lo and behold, it worked! Beautiful cut, sounded great, no chatter at all. I truly don't understand why a smaller, theoretically less rigid tool would result in better results AND a higher MRR. Someday I do hope to understand the mechanics and physics of this but for now I'm just happy to have finally had some positive results. We'll see what the next couple days bring as I have a 1.5x3x12" block of 1018 that needs about 70% of it's mass hogged out so that will be a good test of tool life. Fingers crossed.

  18. #18
    Neuer Benutzer
    Join Date
    Jan 2013
    Posts
    588

    Re: MRR 4140HT (PH)

    There's less tool pressure with the 1/4 inch tool and you are running it at a higher RPM so the frequency of cutting edge entering and leaving the material has changed. Could simply be the 3/8 tool hits the resonant frequency of your machine.

  19. #19
    Registered
    Join Date
    Oct 2008
    Posts
    1986

    Re: MRR 4140HT (PH)

    The Tormach flood coolant system may not be enough for carbide milling in steel. Its a split camp at all. If you read the guys over at Practical Machinist some say, "Oh we run flood on carbide in steel all the time, and others say "THERMAL SHOCK! THERMAL SHOCK! THERMAL SHOCK!" They are both right. The guys running flood aren't running fractional horsepower pumps with just two nozzles rated in gallons per hour. They are running big VMCs with giant pumps and giant coolant reservoirs half dozen nozzles and delivering coolant at a staggering rate that keeps the cutting edges completely buried in coolant in spite of incredible cutting and chip flinging forces trying to blow the coolant away. For serious cutting they are also running through cutter coolant which has to carry away chips as it exits the cut.

    If the cuts are well planned and I get everything just right I can cut steel dry on my Hurco Mill (currently has a major problem in one lead screw), but I got better tool life and tool evacuation by setting up an air blast. Air does act as a coolant, but it doesn't cool enough fast enough to cause thermal shock generally. The air also helps clear chips. I don't see (within its horsepower limitations) why the Tormach would be any different. Both machines have similar size coolant pumps (I also have a 3 phase pump on the shelf out of the base of the Hurco) The coolant tank I am using on the Hurco is slightly smaller, but the useable volume is about the same.

    Now, an interesting aside. On my little Speedmasters (don't buy one unless you like fixing new machines) which also have similar capacity coolant systems I did run coolant for 4140HT with small cutters (1/16 -1/32) when making embossing press dies. Very smaller cutters even at 24,000 rpm were not able to fling the coolant away. Tools lasted for hours. Larger tools just aren't really up to steel cutting on those machines.

    I'm sorry I have not yet had time to work on this project and report back. Unfortunately customers want me to actually work on their parts. They won't just give me money and let me do whatever I want. With the Hurco down (sorta, I used it some yesterday) The Tormach is taking up the slack which is primarily why I bought it.
    Bob La Londe
    http://www.YumaBassMan.com

  20. #20
    Neuer Benutzer
    Join Date
    Jan 2013
    Posts
    588

    Re: MRR 4140HT (PH)

    I found the same when running 4140 on the X7. An air blast was key to cutter life as that chips coming off are hardened once cut. Keeping them out of the way of the advancing cutter edge was important to keeping a cutter alive.

Page 1 of 2 12

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
  •