Trying to buy back another ATC spot; TiAlN on non-ferrous?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    45
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    3

    Default Trying to buy back another ATC spot; TiAlN on non-ferrous?

    So I have a Haas Minimill (10 tool ATC.) I keep T1-T4 occupied with my probe, spot drill, chamfer tool and facemill.

    I've been looking at buying Nine9's Indexable 145°/90° Spotting/Chamfering Tool to consolidate my spot drill and chamfer-er into one tool number.

    Only hang up is that they only make the inserts coated in TiAlN. I only cut aluminum, steel, and plastics- with flood coolant. I read that TiAlN is a no-no for anything non-ferrous, but it also seems like people are saying that in the context of high-heat ops like dry-milling or drilling.

    Given that I'm only chamfering and spotting, does anyone think it's not worth buying back that extra tool slot with this?

  2. #2
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,659
    Post Thanks / Like
    Likes (Given)
    1261
    Likes (Received)
    1425

    Default

    Quote Originally Posted by TheWolfOfWalmart View Post
    So I have a Haas Minimill (10 tool ATC.) I keep T1-T4 occupied with my probe, spot drill, chamfer tool and facemill.

    I've been looking at buying Nine9's Indexable 145°/90° Spotting/Chamfering Tool to consolidate my spot drill and chamfer-er into one tool number.

    Only hang up is that they only make the inserts coated in TiAlN. I only cut aluminum, steel, and plastics- with flood coolant. I read that TiAlN is a no-no for anything non-ferrous, but it also seems like people are saying that in the context of high-heat ops like dry-milling or drilling.

    Given that I'm only chamfering and spotting, does anyone think it's not worth buying back that extra tool slot with this?
    TiAlN is technically a no-no for aluminium specifically, not non-ferrous as a whole. Aluminium tends to bond to the coating causing BUE and clogged flutes, and ultimately broken tools.

    It's manageable if the necessary precautions are taken - dry cutting aluminium with TiAlN is a really, really bad idea, MQL is also dodgy. With flood, you can get away with it if your concentration is high enough - it's all about lubricity, not cooling. If you're full slotting you need to heavily reduce the feedrate to minimise the volume of chips evacuating the flutes, etc. etc.

    If you try full slotting aluminium with a TiAlN coated tool at the same cutting data you'd use for an aluminium specific tool, you'll have a broken tool friction stir welded into your part in very short order.

    For chamfering it's no issue, I use TiAlN coated solid chamfer mills in aluminium all the time.

    One thing to consider is that those indexables have only one cutting edge, so while they are a reasonable compromise for spotting, they really suck for chamfering compared to a 4 flute solid carbide chamfermill.

  3. Likes Red James liked this post
  4. #3
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    45
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    3

    Default

    Thanks for the experience. And excellent point about the flutes. Not sure why I didn't think of that but with my 6K spindle that would definitely slow chamfering ops down....As for coolant I do keep my concentration on the higher end but it does drop quickly in the summers and I'd hate for that to catch me by surprise

  5. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,048
    Post Thanks / Like
    Likes (Given)
    1611
    Likes (Received)
    1880

    Default

    We use these day in and out for spotting and 'light' deburring - chamfering of aluminum.

    https://www.mscdirect.com/product/details/06298541

    Yes, it is technically the wrong coating as greormarwick pointed out, but has never caused us issue with flood coolant. We often spot up to full diameter (.187") for 8-32 taps and such, and then use them to run a light (.001-.005") chamfer to break edges. All of our work is fairly small, not sure you would have same results with say a 1/4"-3/8" tool. We do use the same coating on our 1/2" chamfer mill, but it doesn't see everday use (for the record)....

  6. #5
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    388
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    137

    Default

    Quote Originally Posted by Mike1974 View Post
    We use these day in and out for spotting and 'light' deburring - chamfering of aluminum.

    https://www.mscdirect.com/product/details/06298541
    It always amazes me when I see what I think are experienced machinists using 90 degree point angles for spotting. I see it all the time on Youtube too. What gives? Mine as well use a lathe center drill for all the good it's doing.

    Do yourself a favor and draw up the chamfer and drill combinations used and then look closely. What you're getting is the extreme outer corners of the drill being the first thing to hit the material. IMO there are few things that could be worse. Also there is little there in the way of positioning help, which is the main reason a person would spot drill in the first place. (I know... chamfer too.)

    An excellent combination is the 120 deg spot and 118 deg drill. Not only does it give the drill tip all the guidance it could ever ask for, and frankly needs, it leaves the outer edges in the clear where they belong at that moment of contact. Top it off with the fact you're left with a chamfer that exactly matches the 60 degree standard thread angle of 90% of the threads most if us are producing. Talk about lead in.

    Use a 140 degree spot for 130 -135 degree drills if you really think you need it, but it's not as magical as the combination above. Many times when drilling with the 135 degree I'll chamfer with the 120 or 90 after. Don't forget your G98 retract to initial height cycles in these situations. It's easy to calculate the -Z R height needed using drill constants to make hole chamfering fly by in a second or less.

    My apologies if it seems I hi-jacked this thread. Just got so surprised on this Sunday morning with what people are doing who IMO might know better.

    Dave

  7. Likes Dupa3872, Garwood liked this post
  8. #6
    Join Date
    Jul 2010
    Location
    corvallis,or
    Posts
    876
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    368

    Default

    You do a lot more with a chamfer mill than threaded holes. You going to chamfer your entire part with a 120 degree spot drill? The point of the OP was how to save a spot in the ATC.

    A 90 degree spot/chamfer mill works fine to locate holes as long as you keep your spot diameter to slightly larger than the web of the following drill.

    Teryk

    Sent from my XT1710-02 using Tapatalk

  9. #7
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,392
    Post Thanks / Like
    Likes (Given)
    887
    Likes (Received)
    1496

    Default

    We chamfer aluminum with AlTiN coated 1/4" chamfer mills all the time with no issues.

    We have aluminum-specific (uncoated) chamfer cutters loaded in the machines, but they're larger in diameter. Sometimes we need to use the smaller cutter for clearance reasons.

    Even with 15K spindles, we just can't get the 1/4" cutters to spin fast enough to where chip welding is a problem, especially in a light chamfering op.

    4/5-flute AlTiN endmills would be a different story. Those never touch aluminum.

  10. Likes TheWolfOfWalmart liked this post
  11. #8
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    388
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    137

    Default

    Quote Originally Posted by mTeryk View Post
    You do a lot more with a chamfer mill than threaded holes. You going to chamfer your entire part with a 120 degree spot drill? The point of the OP was how to save a spot in the ATC.

    A 90 degree spot/chamfer mill works fine to locate holes as long as you keep your spot diameter to slightly larger than the web of the following drill.

    Teryk
    I know... I already apologized for getting a bit off track. An unspoken point was better to deal with what you got then use 90 degrees for spotting. There is no diameter created by that 90 deg tool, be it smaller or greater then the follow up drill size, that is beneficial to the drill that follows. Seriously... draw it up and see what is being presented to that poor drill at the tool work interface. Better off using screw machine length without spotting and chamfering after with whatever tool suits your fancy.

    IMO the tool the OP was looking into is better, at least at spotting, then a 2 flute 90 deg chamfer tool like suggested later.

    Back directly to the OP problem. I'd drop the face mill if anything. I personally do tons of work without ever facing. Or at least facing that can't be done with an end mill needed elsewhere. If anything the op can program in M00 or M01's, and hand change a tool here or there with separate offsets already stored and programmed. And messages on the screen to direct the operator to the needed task.

    Dave

  12. Likes Pete Deal liked this post
  13. #9
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    698
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    749

    Default

    Pocket5 in my MiniMill has been loaded with a 90 degree, 1/4" Carbide Mill-Drill for a very long time. (as a matter of fact all of my mills have exactly the same first six tools). I use that tool for spotting drilled holes, all of my edge breaks, and 45 degree chamfers. Any odd sized chamfers or larger than .125 deep chamfers are done with a ball endmill (also always loaded in pocket 6). For the above objection on using a 90 degree tool to start a 118 degree hole... I don't care. I do protos and short runs, drill are cheap and time is expensive. If I need remarkable accuracy on a drilled hole location; I helically interpolate the start to 1x D with a flat EM, then drill, then come back and circle mill my edge break.

    This seems to maximize my ATC and minimize the number of times I need to load a tool. Not remarkably efficient for production, but for MY work it is perfect.

  14. Likes Vancbiker, bryan_machine liked this post
  15. #10
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,709
    Post Thanks / Like
    Likes (Given)
    854
    Likes (Received)
    2554

    Default

    I too only have 10 tool magazine. Like a couple others above, I use 1/4" solid carbide chamfer mills for spotting and, chamfering, edge breaks, etc. For spotting, I only make a tiny spot. Just a bit wider than the web of the drill. After the hole is drilled I may come back and put a chamfer on.

  16. Likes G00 Proto liked this post
  17. #11
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    388
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    137

    Default

    Quote Originally Posted by Vancbiker View Post
    I too only have 10 tool magazine. Like a couple others above, I use 1/4" solid carbide chamfer mills for spotting and, chamfering, edge breaks, etc. For spotting, I only make a tiny spot. Just a bit wider than the web of the drill. After the hole is drilled I may come back and put a chamfer on.
    Okay I give up. :-)

    I can see in tool count limited machines where using a chamfer drill might work. The few who mention using this tool are creating just over chisel edge or web thickness size spots only. In a pinch this doesn't strike me as crazy or not up to the task. I will say on smaller drills, and hence the even smaller spot that will precede it, that 90 degree fragile razor point doesn't present itself well as a cutting tool. At least not a robust one.

    Curious how in this application do the 90 deg mill/drills work in steel, steel alloys and stainless. So much gets talked about sometimes that really only works in things like aluminum where you can get away with murder.

    Dave

  18. #12
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    698
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    749

    Default

    Quote Originally Posted by 13engines View Post
    Okay I give up. :-)

    I can see in tool count limited machines where using a chamfer drill might work. The few who mention using this tool are creating just over chisel edge or web thickness size spots only. In a pinch this doesn't strike me as crazy or not up to the task. I will say on smaller drills, and hence the even smaller spot that will precede it, that 90 degree fragile razor point doesn't present itself well as a cutting tool. At least not a robust one.

    Curious how in this application do the 90 deg mill/drills work in steel, steel alloys and stainless. So much gets talked about sometimes that really only works in things like aluminum where you can get away with murder.

    Dave
    They are pretty fragile in SS and steel alloys. I still use Mill/Drill tools, but I need to run a very conservative feed rate. I was running them in 316L for the last couple of weeks and was pushing them at 250 SFM and 2 IMP feed. If I pushed them much harder they would fracture. Fortunately, I was only going in .050" to start the web of the drill so it wasn't a big enough deal to swap it out with a more robust spot drill.

  19. #13
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,709
    Post Thanks / Like
    Likes (Given)
    854
    Likes (Received)
    2554

    Default

    Most my work is aluminum so you can get away with a lot. For the small amount of steel or stainless that I do chamfer mills are OK as long as you feed gently. For low volume stuff no problem. For production I'd go with a proper spot drill.

  20. #14
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,959
    Post Thanks / Like
    Likes (Given)
    1156
    Likes (Received)
    1210

    Default

    I haven't seen a measurable difference in hole location spot or no spot so I don't spot. Carbide drills do make a measurable difference in hole location, at least the holes I have measured in some 6061 parts with .126" holes.

  21. Likes Garwood liked this post
  22. #15
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    45
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    3

    Default

    Quote Originally Posted by 13engines View Post
    Do yourself a favor and draw up the chamfer and drill combinations used and then look closely. What you're getting is the extreme outer corners of the drill being the first thing to hit the material. IMO there are few things that could be worse. Also there is little there in the way of positioning help, which is the main reason a person would spot drill in the first place. (I know... chamfer too.)
    Harvey has a really good technical paper or whatever illustrating it. I didn't really 'get' spotting until I read it but it gives me the puckers to imagine spotting the wrong angle and having the corners of the drill hit before the webbing does.

    Quote Originally Posted by 13engines View Post
    An excellent combination is the 120 deg spot and 118 deg drill. Not only does it give the drill tip all the guidance it could ever ask for, and frankly needs, it leaves the outer edges in the clear where they belong at that moment of contact. Top it off with the fact you're left with a chamfer that exactly matches the 60 degree standard thread angle of 90% of the threads most if us are producing. Talk about lead in.
    Good point about the thread angle. But that does make me wonder know if 140° is good enough to both cover 118° and 135° drills.... Do you have any experience with that?

    Quote Originally Posted by Orange Vise View Post
    Even with 15K spindles, we just can't get the 1/4" cutters to spin fast enough to where chip welding is a problem, especially in a light chamfering op.
    Just to clarify, this is with flood coolant correct? Kind of a dumb question but that would be a good reference point as to the difference between TiAlN vs the uncoated I've chamfered miles with

    Quote Originally Posted by 13engines View Post
    Back directly to the OP problem. I'd drop the face mill if anything.
    Idk why but I hadn't really considered that. I have to setup for pretty much every job but my facemill is pretty much the only tool with a dedicated holder. I could just write the height offsets on the holder and put it in before hand. Maybe G10 in-situ. Hmmmmm.....

    Quote Originally Posted by G00 Proto View Post
    Pocket5 in my MiniMill has been loaded with a 90 degree, 1/4" Carbide Mill-Drill for a very long time. (as a matter of fact all of my mills have exactly the same first six tools). I use that tool for spotting drilled holes, all of my edge breaks, and 45 degree chamfers. Any odd sized chamfers or larger than .125 deep chamfers are done with a ball endmill (also always loaded in pocket 6). For the above objection on using a 90 degree tool to start a 118 degree hole... I don't care. I do protos and short runs, drill are cheap and time is expensive. If I need remarkable accuracy on a drilled hole location; I helically interpolate the start to 1x D with a flat EM, then drill, then come back and circle mill my edge break.
    So has spotting a 90 hole made a difference on the life of your drills? FWIW I only have my shitty set of HSS TiN drills (I replace with cobalt as they wear and break.) I love the idea of interpolating the start for the holes. Do you ever get blemishes/nicks at the top of the hole when you do that?

  23. #16
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,267
    Post Thanks / Like
    Likes (Given)
    201
    Likes (Received)
    1593

    Default

    Here's what I have done for maybe a quarter million holes, mostly in Al, for some pretty picky customers that would have told me by now if there were location or edge issues:

    OSG EXGold drills (yes, they're expensive)
    90* MA Ford carbide spotting drills, 3/16" to 3/8" depending on hole size
    Make a spot that is .01" bigger than the hole size, so .260" for a 1/4" hole
    Drill

    Spotting oversize gives you a chamfer.

    Regards.

    Mike

  24. Likes Mike1974, coffeetek liked this post
  25. #17
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    197
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    78

    Default

    I would recommend a drill-mill as well. I have never had an issue using TiAlN coated tools on aluminum as long as I have flood coolant and am not doing heavy cutting. Even on our machines with 20-24 tools, with 10 standard tools it doesn’t take long for real estate to be taken up by drills and taps and end mills and so on, so having one tool that can do a lot is ideal.

    Same with spotting with a 90-degree tip, been doing it that way for five+ years and have not seen any issue. In aluminum, steel or stainless, spotting large enough to pre-chamfer the holes. The only exception is when using carbide drills, but even then for our mainly short-run applications I see no effect on tool life or location.

    I also have direct experience with the Nine9 inserted tool and I’m not a fan. Being single fluted makes it half as fast feed wise. I like the concept but in practice it didn’t work for me.

    And lastly, if you go with a drill-mill, go with Accupro or Melin. We have switched to a brand called Monster Tool because it’s cheaper, and it is for a reason. They don’t hold up near as well.

    The only bad thing about drill-mills in my opinion is inconsistency of the tip flat, which can make chamfers need a little tweaking from one tool to another, but it’s typically a very small difference.

  26. #18
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    388
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    137

    Default

    Quote Originally Posted by TheWolfOfWalmart View Post
    Good point about the thread angle. But that does make me wonder know if 140° is good enough to both cover 118° and 135° drills.... Do you have any experience with that?
    For your 135 degree drills which are likely split point, and the fact that you're tool pot limited, I would not spot for 135 deg drills but drill and chamfer after. Use the G98 retract to initial plane drilling regime with a -R input to get the chamfer down the hole close to the cutting height quickly so your chamfering operations fly by in a hurry.

    I still think when you leave aluminum and are working in other materials, the 90 deg spot mill/drill is a poor choice. Interpolating a start hole doesn't strike me as the way to go either. To each there own I guess. A lot of times in tougher materials and using 130 - 140 degree drills, I'll do like stated above and no spot chamfer after.

    Dave
    Last edited by 13engines; 01-04-2020 at 11:56 PM.

  27. #19
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    736
    Post Thanks / Like
    Likes (Given)
    106
    Likes (Received)
    381

    Default

    Quote Originally Posted by 13engines View Post
    Use the G98 retract to initial plane drilling regime with a -R input to get the chamfer down the hole close to the cutting height quickly so your chamfering operations fly by in a hurry.
    Interesting how many people don't realize this "trick" (if you wanna call it that)

    How many times do you see people starting at positive values, 0.100" or .05 or .02 or something. Wait all day while that c'sink cuts air before it gets to it's final .01-.02 or so where it actually cuts. Crazy.

    Just rapid into the hole like .01" shy of contact, then you're only feeding .03" or so to make your c'sink.

  28. #20
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    401
    Post Thanks / Like
    Likes (Given)
    155
    Likes (Received)
    143

    Default

    Having done the same thing, I got rid of both my spotting drill and my face mill, and went to only using carbide drills. Surface finishing is done with good end mills now and I don’t spot my drills.

    Cobalt and HSS drills are cheap but carbide drills just work and don’t fuss. No spotting, they’re fast, they don’t gum up in soft steels like cobalt can, they last a long time.

    Face mills seem like a requirement on a CNC but I’m happy to not use one now. Good end mills, particularly super end mills, leave a great finish. Face mills are great in a lot of applications, but consider if it makes sense for what you do or if you could live without it.


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
  •