Roughing end mill help - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 56
  1. #21
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    138
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    81

    Default

    Quote Originally Posted by SamS View Post
    So I was able to run the program once I decreased by axial depth of cut. So it's cutting (albeit slowly) until the carbide cutter comes in from Maritool. We went with the 3/4 coated carbide from them. If you don't mind helping me again what would be some safe numbers to start off with side milling with carbide cutter? We are climb milling, still force to go into a .7 radius corner. Material is 4140A. Thanks again guys!
    There is a link to a speeds and feeds chart on the web site.
    3/4 TIALN rougher MariTool

    per chart
    med carbon steel

    200-280 sfm
    .0035 feed/tooth
    .25x dia stepover for profiling
    2x dia for axial depth

    probably be a good place to start

  2. Likes SamS liked this post
  3. #22
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,537
    Post Thanks / Like
    Likes (Given)
    12048
    Likes (Received)
    9674

    Default

    Quote Originally Posted by kenton View Post
    There is a link to a speeds and feeds chart on the web site.
    3/4 TIALN rougher MariTool

    per chart
    med carbon steel

    200-280 sfm
    .0035 feed/tooth
    .25x dia stepover for profiling
    2x dia for axial depth

    probably be a good place to start
    NO ITS NOT.. Not for an annealed 4140.. Annealed 4xx0 isn't very far off of
    1018... You can get stupid with it.. Maybe back her down 15-20%.

    Hardened, different story..

  4. Likes triumph406, litlerob1 liked this post
  5. #23
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,280
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    1374

    Default

    Quote Originally Posted by SamS View Post
    I should have mentioned we are using conversational programming for this part so HSM toolpaths are out of the equation.
    It's 2018. You need to make HSM toolpaths part of your equation.

  6. #24
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Quote Originally Posted by gkoenig View Post
    It's 2018. You need to make HSM toolpaths part of your equation.
    What useful insight, thanks I'll just go purchase a machine with HSM capabilities now.

  7. #25
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    138
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    81

    Default

    Quote Originally Posted by Bobw View Post
    NO ITS NOT.. Not for an annealed 4140.. Annealed 4xx0 isn't very far off of
    1018... You can get stupid with it.. Maybe back her down 15-20%.

    Hardened, different story..
    Going off the chart, 15%-20% down from 1018 (low carbon) would put you slower than the speeds for 4140 (med carbon). Do you have a more specific speeds and feeds recommendation for someone looking for advice.
    Not trying to be an ass, just trying to help and I'm curious myself.

  8. #26
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Quote Originally Posted by Bobw View Post
    NO ITS NOT.. Not for an annealed 4140.. Annealed 4xx0 isn't very far off of
    1018... You can get stupid with it.. Maybe back her down 15-20%.

    Hardened, different story..
    Yeah I really enjoy working with 4140. Some of the charts I've used seem to be way off, so I just wanted to see if I could get some opinions, but I'll start with what they've provided!

  9. #27
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    8,543
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2275

    Default

    Quote Originally Posted by SamS View Post
    I haven't had much experience using a roughing end mill in a cnc machine previous to this part so I am a bit in the dark on how to run it. We have a lot of material to remove so it's important I get it right so we don't burn through tools! The material is 4140A, the set-up is not an issue, plenty to grab by in the vice. I am using a HSS 3/4 diameter x 1-5/8 length roughing endmill, machine has 20HP. I am side milling, the required depth is 1.5 inches. My initial numbers are 1.5 axial depth of cut, .116 radial depth of cut, speed 500 RPM and feed of 6.6 ipm. After the first piece the endmill seems to be cutting fine but already looks a bit worn, should I not be taking the full 1.5 inch depth at once?

    Thanks for your help!
    1.75 or 2.0" dia roughing HSS endmill can often take 10 or more hp

  10. Likes SamS liked this post
  11. #28
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,280
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    1374

    Default

    Quote Originally Posted by SamS View Post
    What useful insight, thanks I'll just go purchase a machine with HSM capabilities now.
    What makes you think your machine isn't capable of HSM paths?

    1- With a wide smoothing tolerance, most older machines aren't going to have an problem feeding steel HSM feed rates of 30-50IPM. Sure, if you want to do maximum PsychoMill aluminum killing speeds of 400ipm, older machines can't keep up, but that isn't the application here. If you've got a conversational control, I'm betting you can probably do HSM just fine. For reference, my 2006 Robodrill with the low-end 0i-MC Fanuc control can do 200ipm aluminum roughing HSM paths just fine.

    2- CAM to spit out high quality HSM toolpath is now free with Fusion 360. You can download it, run through some YouTube tutorials, and probably have HSM paths running on your machine in a day or two. And those techniques are going to improve basically everything you ever do with it, so it's a worthwhile investment.

  12. #29
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Quote Originally Posted by gkoenig View Post
    What makes you think your machine isn't capable of HSM paths?

    1- With a wide smoothing tolerance, most older machines aren't going to have an problem feeding steel HSM feed rates of 30-50IPM. Sure, if you want to do maximum PsychoMill aluminum killing speeds of 400ipm, older machines can't keep up, but that isn't the application here. If you've got a conversational control, I'm betting you can probably do HSM just fine. For reference, my 2006 Robodrill with the low-end 0i-MC Fanuc control can do 200ipm aluminum roughing HSM paths just fine.

    2- CAM to spit out high quality HSM toolpath is now free with Fusion 360. You can download it, run through some YouTube tutorials, and probably have HSM paths running on your machine in a day or two. And those techniques are going to improve basically everything you ever do with it, so it's a worthwhile investment.
    HSM is generally defined as RPMs over 12,000, our machine only gets to 10,000. I believe you are referring to just better toolpaths (adaptive clearing). We have Fusion and we are working towards getting it function with our machine, but we are also working on a million other things at the same time! I do have plenty of questions on Fusion if you're willing to answer them though

  13. #30
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    171
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    108

    Default

    Quote Originally Posted by SamS View Post
    HSM is generally defined as RPMs over 12,000, our machine only gets to 10,000. I believe you are referring to just better toolpaths (adaptive clearing). We have Fusion and we are working towards getting it function with our machine, but we are also working on a million other things at the same time! I do have plenty of questions on Fusion if you're willing to answer them though
    My hitachis max at 10,000 and I run HSM at 7500 because our machines are old but that didn't stop me from trying. Start out with light cuts at full depth and make adjustments in the machine. I started out slow and light cuts and when I finished a job I nearly tripled the feed and doubled the step over before the parts starting moving out of the fixture.

  14. #31
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,563
    Post Thanks / Like
    Likes (Given)
    708
    Likes (Received)
    1366

    Default

    Quote Originally Posted by kenton View Post
    Going off the chart, 15%-20% down from 1018 (low carbon) would put you slower than the speeds for 4140 (med carbon). Do you have a more specific speeds and feeds recommendation for someone looking for advice.
    Not trying to be an ass, just trying to help and I'm curious myself.
    I looked at the S&F chart for that Tool, pretty conservative, which is just good business for a Tool Manufacturer. It lists 500 SFM for 1018, that is pretty dang slow.

    I'm pretty sure Bob was under the impression that it would be much higher on the chart, hence the "drop it down 15-20%". I will run 1000 SFM in 1018 easy really. SO dropping it to 800 SFM is pretty reasonable (maybe a little high for my taste, but doable). Still that is double what the OP is doing. It takes a good effort to F-up 4140, so I would start with a .004" chipload with SFM below 800 and no HSM toopaths, and make adjustments from there.

    As far as JUST DO IT-HSM toolpaths go, it took me a little while to adapt to them, I didn't just wake up one day and everything was HSM. Granted once I got involved, that was a spiritual experience, but it took time to prove out.

    My ±2 R

  15. Likes Bobw liked this post
  16. #32
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    331
    Post Thanks / Like
    Likes (Given)
    243
    Likes (Received)
    172

    Default

    I HFM 17-4 and titanium every day on a Haas. I also HFM 4140 prehard for vise jaws. I started learning about it almost 20 years ago, and there are very few situations I've seen where it isn't both applicable and preferable. You can probably get the basics of it even with conversational programming; just cut to full depth with 8%-10% stepover with appropriately adjusted feeds and speeds.

  17. #33
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,280
    Post Thanks / Like
    Likes (Given)
    575
    Likes (Received)
    1374

    Default

    Quote Originally Posted by SamS View Post
    HSM is generally defined as RPMs over 12,000, our machine only gets to 10,000. I believe you are referring to just better toolpaths (adaptive clearing). We have Fusion and we are working towards getting it function with our machine, but we are also working on a million other things at the same time! I do have plenty of questions on Fusion if you're willing to answer them though
    Fair!

    I think the term HSM often becomes a catch-all for a whole series of techniques and tools that I tend to think of as part of (to ape the gun world) the "Modern Technique" - algorithm generated constant cutter engagement toolpath, chip thinning speeds/feeds, trochoidal motion, maximum axial engagement, advanced tooling materials/coatings, etc. Depending on the application, material we're working with, and our equipment capabilities, we can pick and choose from this bag of tricks as necessary.

    In this case though? I think you'll get massive bang for your buck by getting this job off the conversational and into Fusion so you can apply their Adaptive Clearing (i.e. algorithm generated, constant cutter engagement, material aware lead-in tool path).

  18. Likes Bobw, micro liked this post
  19. #34
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,537
    Post Thanks / Like
    Likes (Given)
    12048
    Likes (Received)
    9674

    Default

    Quote Originally Posted by kenton View Post
    Going off the chart, 15%-20% down from 1018 (low carbon) would put you slower than the speeds for 4140 (med carbon). Do you have a more specific speeds and feeds recommendation for someone looking for advice.
    Not trying to be an ass, just trying to help and I'm curious myself.
    What he said up there. Slotting, take it easy, you are building heat for 180 degrees. 350-450...
    You start getting narrow and deep, you can get WAY up there. 700 sfm at a 10-12% stepover, I would say is
    comfortable. I've played a bit up to around 1200 with a 1/2" endmill, and I don't have much more spindle
    than that.. And feed the hell out of it. Messing around with a facemill, trying to make time(nothing
    fancy, just an SExx blah blah 45 degree lead, $7 or $8 inserts, and I'll run 800-900 surface feet, and
    I've not had anything bad happen finishing up to 1400..

    That's trying to make time and move metal.. One offs and small stuff where the time doesn't really
    much matter, my goto numbers are around 350-450sfm. Even at that speed and being conservative on feeds,
    you have to TRY and get below 4 cubic inches a minute..

    4xx0 ANNEALED, is really really close to dealing with a mild steel. It even likes to tear when
    you are turning it.

  20. #35
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Quote Originally Posted by gkoenig View Post
    Fair!

    I think the term HSM often becomes a catch-all for a whole series of techniques and tools that I tend to think of as part of (to ape the gun world) the "Modern Technique" - algorithm generated constant cutter engagement toolpath, chip thinning speeds/feeds, trochoidal motion, maximum axial engagement, advanced tooling materials/coatings, etc. Depending on the application, material we're working with, and our equipment capabilities, we can pick and choose from this bag of tricks as necessary.

    In this case though? I think you'll get massive bang for your buck by getting this job off the conversational and into Fusion so you can apply their Adaptive Clearing (i.e. algorithm generated, constant cutter engagement, material aware lead-in tool path).
    I thought you were being a dick, suggesting we don't have a modern machine. My fault! It was just misunderstanding. HSM is indeed a catch all phrase now. I've always thought of it as meaning high spindle speeds and accurate enough machine to hit points accurately at speed.

    Regardless....I've taken everyone's advice and I brought in an old friend who has taken programs from cam to the machine and he cleared up a lot of questions. Our cutters don't come in until Monday so I am hoping to have a program proofed out and ready from fusion by then. My cad skills are good so I'm only worried about that scary moment of hitting the start cycle button

    Again thanks for the help everyone!

  21. #36
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    99% of the stuff we do is expensive 1 - 10 qty jobs. Most of the industry that I am in, at least the shops I've worked at and visited, are still running on mostly 2.5 axis Bridgeports. So when they go over to full cnc the toolpaths, feeds and speeds don't seem to change much (machinists are faaaairly hardheaded). I was trained by someone just like that, so I am admittedly a bit ignorant on applying modern toolpaths and really getting the mrr up

  22. Likes Bobw liked this post
  23. #37
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    408
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    141

    Default

    Just for reference sake. Im running a group of 316L parts right now. Using a 3/4" kodiak carbide rougher 2.5" down at 1400 rpm .03" step over and 30 ipm (in an er32 holder none the less). Yeah, yeah.... its what I had on hand, and it works....
    Yes, small step over and higher rpm than I would usually like from a roughing mill, but when youre dangling out you have to find the happy harmonic place. I've removed 1/4" from 4 faces 6" long on 250 parts, and the end mill looks nearly new.
    Pretty sure it wants to go party with its buddies! love that one Bob

  24. #38
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Hey guys the cutter came in and we are cutting! Not used to that noise from a rougher, but it sounds good to me! Higher pitched and no recutting of chips. I started it at the recommended settings with a smaller step over due to going into a corner. Sounded better once I sped the feed up a little. Thanks for the help. Now it's time to cut some 410 ss

  25. #39
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    One more question...I see a lot of people saying a cutter with this coating should be run without coolant...is that true. I am running it with coolant now, unfortunately we don't have forced air.

  26. #40
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,563
    Post Thanks / Like
    Likes (Given)
    708
    Likes (Received)
    1366

    Default

    Quote Originally Posted by SamS View Post
    One more question...I see a lot of people saying a cutter with this coating should be run without coolant...is that true. I am running it with coolant now, unfortunately we don't have forced air.
    I was going to say something, but I figured someone else would. If you are cutting the periphery of the part, NO coolant. If you are doing a pocket, you need to get the chips out. Basically, the idea is that the hot chips are coming off the part, and the coating can deal with the heat generated in the Tool.

    But the last thing you want is to re-cut hot chips from 4140.

    R


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
  •