Finish issues with tiny boring bar in 4140HT
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 38
  1. #1
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    557
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    304

    Default Finish issues with tiny boring bar in 4140HT

    Long story, sorry in advance...

    I'm a 99% aluminum one-person shop, mostly making my own products. I've got a buddy who has a much larger shop and is swamped. He asked me if I'd be interested in making some overflow parts for him. They are a family of bushings, with very tight tolerances on the bore (+/- .0001"). Originally it was going to be a one-time 1800 piece order for him. I've already made over 3000, and am booked solid for then next few months. The part is very profitable for me, but frustrating as you'll see below.

    Material is 4140HT. My machine is a Doosan Lynx 220 LYA. The part is .5" OD and the ID varies from .221" up to .375", with about 130 sku's total. Because of the number of sku's the bores are made by boring. I'm using a 5mm SCLCR carbide boring bar held in an ER16 collet. Stick-out is about .8". The inserts are Mitsubishi CCGT03S102L-F in VP15TF. I initially ran the same program and tooling as my buddy did.

    Originally I'd get 60-80 good parts before I had to switch insert edges. Good part to me meant shiny bore (no profilometer here) and within +/- .00005". The problem is in between those good parts were about 15-25% scrap. Suddenly a bushing would have a rough bore and be undersize by .0005"-.001" or so. Next one would be good to go. The scrap rate usually went up the more parts there were on the insert edge. My inexperienced steel machining gut was telling me its probably BUE.

    A Mitsubishi rep came by and suggested the same insert but with the MS6015 coating (supposed to be slicker). They left a worse finish and didn't last as long, with the same suspected BUE scrap issues. I went back to the original insert.

    I was using Qualichem Xtreme Cut 250c, which works great in aluminum, and was passible in the very little steel work I did before. My Qualichem rep said that I probably needed chlorinated paraffins to help eliminate the BUE so he sent me a pail of 251c to try. It was the only pail available at the time, so after I filled the sump and my coalescer it was at about 8% concentration. He had suggested 7-10%. I ran the 250c at 10%+ concentration on my aluminum parts. Now my bore finish is worse. The bushing bores look like glass for the first 8-10 parts, but after that the bores have a more matte finish, and things start to go out of spec by about 40 bushings. The scrap rate for the bue/size issue has gone down (now 8-12%), but I'm getting even less parts per insert edge. I can't increase the coolant concentration until either some water evaporates off or I get more 251c. Two other pails of 251c will be here mid-month.

    About 200 parts before the coolant swap I went from my buddy supplied material (Ryerson) to my own supplied material (Speedy Metals). I did get about the same finish (and issues) as before the coolant swap, near as I can remember, but I'm getting forgetful in my old age. I checked hardness on both the Ryerson material and the Speedy material and they are about the same, RC 25 or so. I know that's lower than what's expected for 4140HT, but that could be my hardness tester being uncalibrated. Could material selection cause my new finish issue?

    Getting this boring bar aligned is a royal PITA. The reason I've got a .8" stickout when I only need to bore .450" deep is I'm trying to hold a parallel on the end of the tiny flat of the boring bar while tightening the collet nut...all while trying to keep things from rotating out of alignment. Not enough hands and not exactly precise. I found and tried a 5mm to 3/4" boring bar sleeve. That was worse. I'm not sure if there was some kind of chatter due to the slight amount of clearance there has to be between the bore of the sleeve and the shank of the boring bar? How critical is it for the insert tip to be on centerline? I've got a y-axis so I can fudge it up and down, but I didn't notice any change with +/- .005" or so. I'm boring .450" deep on a .375" deep part because I had some chip packing issues that would occasionally leave a step in the bore the last .050" or so. I try my best to get coolant shooting down the bore to keep the chips clear but it isn't perfect.

    Generally I run these bushings with a feed rate of .003" roughing and .001" for the finish pass. I rough at .003" per side and finish at about .002" per side. Surface speed is about 330FPM. I've tried all kinds of variations of speeds/feeds/DOC, but nothing really seems to help. Remember this is a 5mm boring bar so I can't really push it much.

    I'm running out of ideas. Is there anything glaringly wrong with what I've tried so far? What can I do to keep my surface finish good and lower my scrap rate?

    Any help is appreciated!

  2. #2
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,563
    Post Thanks / Like
    Likes (Given)
    1662
    Likes (Received)
    2134

    Default

    At that hardness your surface speed is pretty close to half what I'd usually run at, but I guess you're RPM limited.

    If I was doing that part (the smallest one for example), I'd drill to like 5.2 or something like that, open up to a few thou under with a 5mm endmill in a live tool (in polar mode, not XY, for best case concentricity), then I'd use a tcmt or dcmt bar and plunge in at the bottom of the bore and bore outwards. Obviously you can't bore outwards with a ccmt, but if you have a different tool I'd try that.

    At those diameters, centre height is absolutely critical, and very difficult to set accurately enough... Normally I will indicate the shank in to zero on XY with the indicator mounted on the chuck, then I will indicate whichever flat is parallel or perpendicular to the centreline plane to get the rotation right. Most bars have a perpendicular flat on the back edge behind the insert that you can indicate in Y - at least Sandvik do and they are my most commonly used bars.

  3. #3
    Join Date
    Feb 2004
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,948
    Post Thanks / Like
    Likes (Given)
    1196
    Likes (Received)
    1958

    Default

    If you don't take enough of a cut your going to get a lousy finish.
    If you don't take enough of a cut your going to be rubbing and wearing our your tools edge.


    CCMT is nice and sharp, stay away from coatings as the reduces sharpness.


    Something that small...I'd give a solid carbide bar a try. It should hold up well in 4140, very sharp and the size you need is right in line with insert cost. True you'll need to adjust bar compared to changing inserts...but if it works they have them with holders and flats that are quick to replace after the bushing is set...just release set screw to move bar and screw orients the bar.
    Mari sells the standard boring bars as does Lakeshore and others.

    We do a bunch of small tight tolerance jobs and that is my guys go to for Alloys, SS 316 etc. In 4140 I'd expect it to hold up for a minimum of several hundreds parts. Just going to have to find that sweet spot of cutting enough not to start rubbing and wearing the edge...but not pushing to chip edge with required finish.

    But that's alway the trick to machining.

  4. Likes CORONA VIRUS liked this post
  5. #4
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,519
    Post Thanks / Like
    Likes (Given)
    808
    Likes (Received)
    662

    Default

    I used to work for Doosan! The Lynx is a great machine!
    OK -

    So, for one thing, I'm not familiar with the Mitsu tooling, but I use Kennametal in a very small 80 deg diamond. I would run about 500 SFM or so. What tool radius do you have? Usually a .032" radius will give a nicer finish and a bit longer life, if possible. Your cutting parameters sound about right.

    I use the same coolant, and have had very good results with it. Next up, tho, is there enough pressure?

  6. #5
    Join Date
    Nov 2019
    Country
    CANADA
    State/Province
    Ontario
    Posts
    596
    Post Thanks / Like
    Likes (Given)
    921
    Likes (Received)
    142

    Default

    I would guess that you don't have any live tooling? If I did, I would be drilling just undersized and a small endmill to size without having a 10K or 15K spindle.
    as for the insert, I might see if there is anything that might be a smaller radius and a harder type of insert.

  7. #6
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    3,265
    Post Thanks / Like
    Likes (Given)
    7926
    Likes (Received)
    2802

    Default

    My guess regarding insert grades, is that your Mits rep needs to do his homework. VP15T is a fairly hard, universal grade for them. Used for a lot/most of their carbide drills? If my memory serves me well, it's a hard, thin PVD coating. Useful in drilling, where low-friction is pretty darn important. 6015 is a steel grade with a thicker, CVD coating. Better for roughing as more heat resistance, but infinitely worse for your application, as the thicker coating makes for a more rounded cutting edge. No surprise that it left a worse finish.

    I would be tempted to try some inserts for aluminum myself. You're cutting that pretty slow in speed/feed, as dictated by RPM limit, etc... I think there might be something there. These inserts are going to have the sharper edge that you'll need at that depth of cut, speed & feed. (You will need a coating however. Uncoated carbide cutting steel begins a chemical reacting where the carbon is sucked out of the carbide, into the steel.)

    My gut tells me to try some of the newer DLC coated aluminum-specific inserts. However, I'd want to call the manufacturer first, to confirm if these will work, of if you'll get the same chemical-diffusion, since the coatings are carbon-based.

    PDL010 / PDL025 - DLC Coating for Aluminum



    If that won't work, then look into inserts for finishing Titanium. They'll have the same sharp cutting edges, but will most likely offer some kind of hard, thin PVD coating that'll retain the sharp cutting edge.

    All of that said, your VP15T insert probably isn't a bad choice.





    Also - If you're indicating the tool for center- height, by using an indicator mounted to the chuck, then beware, that the whole indicator rig will sag a few thou. When the indicator shows you to be on-center, you're actually a couple thou low. Just something to remember.




    On another note - I wonder if a coolant/air-blast mix wouldn't help as well. I didn't catch if these were thru, or blind bores. Perhaps a coolant/air mix would help evacuate chips?

  8. Likes avto762 liked this post
  9. #7
    Guest Guest

    Default

    Quote Originally Posted by Eric U View Post
    Originally I'd get 60-80 good parts before I had to switch insert edges. Good part to me meant shiny bore (no profilometer here) and within +/- .00005".
    I just got done spending 10 years with data capped internet, so I was just recently reintroduced to You Tube. I have never had to hold tighter than +/-.0002 on shallow bores and we checked those with gauge pins, even on medical surgery items and they never were rejected. How do you check a bore down to +/- .00005 accurately without spending a lot of time and or money?

  10. Likes michiganbuck, Bobw liked this post
  11. #8
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    557
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    304

    Default

    Quote Originally Posted by Dualkit View Post
    I just got done spending 10 years with data capped internet, so I was just recently reintroduced to You Tube. I have never had to hold tighter than +/-.0002 on shallow bores and we checked those with gauge pins, even on medical surgery items and they never were rejected. How do you check a bore down to +/- .00005 accurately without spending a lot of time and or money?
    Ok, I’m probably not “accurately” measuring to .0001”, but am trying to have relative accuracy from part to part, and between different size parts. I’m using a bore micrometer and gauge pins. Even though the bore mic is only labeled down to .001”, I’m guesstimating the tenths. By my guesstimations I can tell when the gauge pin will have a snug slip fit and when the pin won’t go in at all by my guess on which .0001” it is reading. No 250k cmm’s here. I do chase 10ths as the machine warms up and when the insert wears, but it’s pretty darn stable after running for 30 mins or so.

    Quote Originally Posted by Jashley73 View Post
    On another note - I wonder if a coolant/air-blast mix wouldn't help as well. I didn't catch if these were thru, or blind bores. Perhaps a coolant/air mix would help evacuate chips?
    Blind holes and bores. I try to drill within .010”-.040” under bore size to start. I don’t have that many carbide drills and don’t want to be changing drills all the time.

  12. #9
    Join Date
    Dec 2007
    Location
    Idaho Falls
    Posts
    64
    Post Thanks / Like
    Likes (Given)
    27
    Likes (Received)
    13

    Default

    I would suggest in your application checking if Mitsubishi makes the insert you are using in cermet. They tend to give a lot nicer finish and you should not have trouble holding size for days on that light of a cut.

  13. Likes Jashley73, mbraddock liked this post
  14. #10
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    3,265
    Post Thanks / Like
    Likes (Given)
    7926
    Likes (Received)
    2802

    Default

    Quote Originally Posted by csteen View Post
    I would suggest in your application checking if Mitsubishi makes the insert you are using in cermet. They tend to give a lot nicer finish and you should not have trouble holding size for days on that light of a cut.
    ^ He beat to it. I was day dreaming of something else, thought cermet, and then suddenly remembered this thread.

    User Oldwrench has a lot of experience with cermets, and his overwhelming recommendation is Kyocera. Browsing their catalog, they do have an unusually large selection of cermet inserts.

    It may be worth it to PM him, and invite him to this thread...




    Turning Grades for Steel - KYOCERA Precision Tools

  15. #11
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,365
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    847

    Default

    I'd look at something from PH Horn or Simtek / Sandvik for those smaller bores like that. When I see the oddball bore like that I always suspect a chip is getting caught and rubbing. Nesting can be an issue with the small inserts (I've found it harder to dial in a chip break) but I've solved that with back-boring or with a quick rub against a wire hook to remove the birds nest.

    Both of the product lines I mention have auto-centering features to keep your Y axis in the right place.

  16. #12
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,563
    Post Thanks / Like
    Likes (Given)
    1662
    Likes (Received)
    2134

    Default

    Quote Originally Posted by Rick Finsta View Post
    I'd look at something from PH Horn or Simtek / Sandvik for those smaller bores like that. When I see the oddball bore like that I always suspect a chip is getting caught and rubbing. Nesting can be an issue with the small inserts (I've found it harder to dial in a chip break) but I've solved that with back-boring or with a quick rub against a wire hook to remove the birds nest.

    Both of the product lines I mention have auto-centering features to keep your Y axis in the right place.
    Problem is those tools are massively more expensive than inserts, and don't last nearly as long. I use them all the time and they are fantastic, but for thousands of parts they'll make a huge dent in the profits.

  17. #13
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    3,123
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2989

    Default

    Hi Eric:
    At that kind of tolerance is honing, ballizing or roller burnishing an option?
    I'll bet a diamond hone would pop those out to within 50 millionths without much pain and fast too, if you get the pre-bore consistent within a half a thou or so, especially if you put two tools down it in succession...the first to make the holes super consistent; the second to bring them to final size and finish.

    Pricey tool, but pretty reliable from what I've heard (I've never run a diamond hone on a production job but I've heard wonderful things from buddies who have)
    Ditto for roller burnishing.
    Ballizing is a pain in the ass but works too for holding tight tolerances.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

    Whoops...didn't read the thread properly...you have a gazillion bore sizes to deal with.
    Ignore all I just said!
    MC

  18. #14
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    5,106
    Post Thanks / Like
    Likes (Given)
    1335
    Likes (Received)
    2908

    Default

    Were it me, I'd buy the best, slickest, wazzoo Drill ever. I have maintained tolerances like that woth an MA Ford Twister drill. Everyone makes it, 3 flute, high helix carbide Drill. I'm not implying this is THE solution, but I'd try it.

    Aligning tiny bars can be a bitch. I usually align it in an ER-11 collet chuck, with a comparator, because the chuck has a flat on it, or I'll put one on it. Alignment is key to boring this small. .0002" shim stock and all.

  19. #15
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    557
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    304

    Default

    Quote Originally Posted by Jashley73 View Post
    ^ He beat to it. I was day dreaming of something else, thought cermet, and then suddenly remembered this thread.

    User Oldwrench has a lot of experience with cermets, and his overwhelming recommendation is Kyocera. Browsing their catalog, they do have an unusually large selection of cermet inserts.

    It may be worth it to PM him, and invite him to this thread...




    Turning Grades for Steel - KYOCERA Precision Tools
    I've sent off an inquiry to Kyocera. Thanks for the heads up.

  20. #16
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,365
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    847

    Default

    Quote Originally Posted by gregormarwick View Post
    Problem is those tools are massively more expensive than inserts, and don't last nearly as long. I use them all the time and they are fantastic, but for thousands of parts they'll make a huge dent in the profits.
    My (albeit limited) experience for tool life is the exact opposite. I had those little 0.027" ID grooving tools make thousands of grooves before the corners would go away. I just bought a bunch of CoroBore MB inserts (another Simtek product) and they were only $20 a piece, and the holder was only $125. That doesn't raise my eyebrows as being particularly expensive for inserted cutters.

  21. #17
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    2,268
    Post Thanks / Like
    Likes (Given)
    247
    Likes (Received)
    2194

    Default

    I never had good luck with 1/4" or smaller indexable boring bars. Insert moves in the pocket. Looks like that is what is happening to you. Check out internal tool and Micro100, they have some nice solid carbide boring bars. Also this would also work...

    Multi Extension Boring Bar 3/16 Shank X 2.0 Long X .007 Radius MariTool

  22. #18
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,563
    Post Thanks / Like
    Likes (Given)
    1662
    Likes (Received)
    2134

    Default

    Quote Originally Posted by Rick Finsta View Post
    My (albeit limited) experience for tool life is the exact opposite. I had those little 0.027" ID grooving tools make thousands of grooves before the corners would go away. I just bought a bunch of CoroBore MB inserts (another Simtek product) and they were only $20 a piece, and the holder was only $125. That doesn't raise my eyebrows as being particularly expensive for inserted cutters.
    The MB are much cheaper than the XS.

    A 5.2mm min bore coroturn XS lists at £32, which is about $44. The ccgt OP is using is presumably under $10. Even if you are paying well under list price it's still going to be more than twice the price for half as many edges.

    I've done a lot of basic boring with coroturn XS bars, admittedly mainly in materials like 17-4, and they are definitely a tougher grade of carbide than a harder grade. Presumably by necessity to prevent them just breaking off at the shank. Not really ideal for high production in 4145HT, unless it really is as soft as OP reckons it is.

  23. #19
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    557
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    304

    Default

    Quote Originally Posted by fmari --MariTool- View Post
    I never had good luck with 1/4" or smaller indexable boring bars. Insert moves in the pocket. Looks like that is what is happening to you. Check out internal tool and Micro100, they have some nice solid carbide boring bars. Also this would also work...

    Multi Extension Boring Bar 3/16 Shank X 2.0 Long X .007 Radius MariTool
    Ok Frank, I'll bite. I need to order a couple of collet chuck nuts anyway so I'll try a couple of your little boring bars. My smallest bushing sizes are actually a bit under my 5mm bar minimum so your 3/16" solid bars would fill the ticket. Loose insert pocket would explain a lot...

  24. #20
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    215
    Post Thanks / Like
    Likes (Given)
    531
    Likes (Received)
    57

    Default

    One tenth tolerance? No wonder he dumped those parts on someone else.
    It's hard to consistently hold that kind of tolerance especially with such small boring bars. 15-20% out of tolerance doesn't sound too bad in my opinion.


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
  •