Results 1 to 11 of 11
  1. #1
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    935

    Default Helical Drilling with Carbide

    I need to bore some Dia 35 holes 17 mm deep into black steel.
    Looking at helical drilling with carbide tooling on a CNC turret mill.

    Tried a 10 mm 4-flute centre cutting solid carbide end mill programmed to cut Dia 15 mm.
    Helix was 1 mm lead, feed at 75 mm/min, spindle 2500 RPM, no coolant.
    Did not pre-drill to provide chip relief.
    A stunning result, just perfect.
    Repeated to bring hole out to Dia 19 mm.

    I thought I would try a single-tip carbide end mill holder.
    Purchased a Dia 12 mm from H&F with Sumitomo APMT 103504 tip, Cat:M519.
    Programmed same helical path set to open hole out to 23 mm diameter.
    It seemed like the tip, tool, machine, and me, were straining !
    Quit without and apparent effects.

    Time to research best practice.
    Started searching for recommendations on speed feed, ramp angle etc.
    Also a show-stopper, this tool only good to 16 mm deep, then it rubs on the shank.
    So I may have to go up to the next size, Dia 16 mm with 2 tips.

    Can anyone offer some suggestions on how to do helical drilling with carbide tipped end mills ?

    John

  2. #2
    Join Date
    Dec 2007
    Location
    Adelaide
    Posts
    589

    Default

    I'm not CNC expert but I would expect speeds and or feeds would need to be altered when going from a 4 flute cutter to a single point/1 flute cutter - at the same speeds and feeds, a single point cutter would be trying to remove 4 times the amount of metal per cutting edge than that of a 4 tooth cutter, so you'd need to reduce the feed rate or increase the spindle speed (or possible both) when moving from a 4 point to a single point cutter - I have attached a basic chip load chart - metric - which would give a good starting point.


    An internet search should turn up an online chip load calculator that just needs you to plug in the spindle speed, feed rate, and number of flutes/cutting points, I use Fusion360 which gives the chip load as Feed per Tooth for the selected cutter, feedrate etc.
    Screenshot 2024-05-03 121121.jpg

  3. #3
    Join Date
    Nov 2017
    Location
    Geelong, Australia
    Age
    57
    Posts
    2,722

    Default

    My experience on a manual mill is the APMT style insert cutters behave completely differently to traditional endmills. Pretty much smashing material off rather than cutting it.
    Particularly trying to cut shoulders with them which youre sort of doing with the helical milling.

    Id suggest playing around with the insert cutter just straight ramping for a start and try to find the settings it likes.
    Being sumitomo they should provide recommended feeds/sppeds/ramp for the tool.

    Steve

  4. #4
    Join Date
    Mar 2014
    Location
    South of Adelaide
    Posts
    1,244

    Default

    I on a small hole like that i normally go 0.5mm stepdown and 0.15mm per tooth, but that is on a proper machining center so you might not have that much rigidity. Another factor is those inserts you are using are at least 2 tooling generations old, modern inserts have much better cutting geometry and will cut smoother than older style inserts.

    If you have a lathe just turn the shoulder back on your endmill to get more depth, i do it all the time, shank will only be 30-35Hrc so can be turned with normal carbide inserts.

    With your machine i think you would be better off sticking with solid carbide tools. for bore milling i would recommend going to a endmill with corner radius instead of a square corner, 10 or 12mm with 1.5-2mm corner rad would be ideal. the reason for going to a radius is you are cutting only on the tip of the tool and a larger radius will not wear as fast as a sharp corner.

  5. #5
    Join Date
    Mar 2014
    Location
    South of Adelaide
    Posts
    1,244

    Default

    Quote Originally Posted by OxxAndBert View Post
    Being sumitomo they should provide recommended feeds/sppeds/ramp for the tool.

    Steve
    My oldest catalogue from them is 2017 and there is no technical info for APMT in there. the APMT inserts were replaced by the WEX line of tools with AXMT inserts, that was replaced a 2-3 years ago by WEZ and AOMT inserts.

  6. #6
    Join Date
    Oct 2011
    Location
    Norwood-ish, Adelaide
    Age
    59
    Posts
    6,605

    Default

    I went away from APMT inserts a while back - they seemed very fragile and would break at the slightest mis-use (and the screws always seemed to be breaking). Possibly they were designed with CNC in mind and the designers expected feeds and speeds to be tightly controlled. From memory all the tooling I had was side cutting - the inserts I had were something like 6mm across the narrow edge, so to feed it vertically the hole would have to be pretty close to the finished size anyway.

    Steve mentioned ramp angle. That's going to be less than the relief angle on the bottom of the tool and for HSS it is typically only a degree or two. Depending on geometry, a cutter set up with APMT inserts could be worse so that would be worth checking. A 35mm diameter hole with a 1mm step down is a bit over 1/2 a degree, so it's not going to take much before you are rubbing and not cutting.

    Michael

  7. #7
    Join Date
    Dec 2014
    Location
    melbourne
    Posts
    73

    Default

    With helical drilling you need a center cutting end mill because you are ramping down using the end face of the cutter.
    If the cutter you are using is not capable of plunging,in general it is not suitable for helical drilling.
    There are special insert cutters for ramping down but I know of none first hand. the only one I have seen was for aluminium.

    Robert

  8. #8
    Join Date
    Mar 2014
    Location
    South of Adelaide
    Posts
    1,244

    Default

    Quote Originally Posted by shedeng View Post
    With helical drilling you need a center cutting end mill because you are ramping down using the end face of the cutter.
    If the cutter you are using is not capable of plunging,in general it is not suitable for helical drilling.
    There are special insert cutters for ramping down but I know of none first hand. the only one I have seen was for aluminium.

    Robert
    Sorry that is completely incorrect, you don't need a center cutting tool for helical boring. I use Insert endmills up to 80mm diameter all the time, Just need to stay withing the manufacturers parameters for ramp and cutter overlap, for example a sumitomo 50mm WEZ endmill can ramp at about 0.5 degrees and minimum hole size is about 95mm while the 25mm version can ramp at about 4 degrees in a minimum hole of about 45mm.

  9. #9
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    935

    Default

    All the suggestions greatly appreciated.

    I spent some time over the weekend with my CNC mate and we have changed tack (a little).
    He agreed that the tipped cutter not ideal for this job, use the solid carbide only.

    We have decided to break the job down to even out tool wear:
    - drill to depth Dia 8.
    - helical drill to depth out to 15 mm,
    - helical drill to depth out to 22 mm,
    - pocket to half depth (8.5 mm) out to 35 mm,
    - second pocket to full depth out to 35 mm.

    Test part is fine.
    45 more to go.

    For the tipped carbide, I trialled different facing cuts and got excellent results.
    My mate helped me get over the reluctance of the heavy cuts necessary.
    I will use this cutter in future for trimming parts to size, square etc.
    But, all the suggestions will be taken on board and helical drilling attempted again.

    Keep well,
    John.

  10. #10
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    935

    Default

    A comment on the ramp angle.

    The Sumitomo data sheet that I discovered lists the APMT insert end mill ramp angles increasing as the diameter is reduced.
    At 14 mm diameter the ramp was listed as 7 degrees, so 12 mm diameter will be something greater.

    I trialled the tipped tool at 3 degrees in a straight line without any problems.

    A 1 mm helix lead at 35 mm diameter is about 1 in 110 mm path length, or about 1/2 degree.

    Keep well,
    John.
    Last edited by electrosteam; 5th May 2024 at 11:47 PM. Reason: spelling

  11. #11
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    935

    Default

    Photo shows result of a helical drilling exercise using the tipped tool.
    The starting hole was Dia 22 mm done with the solid carbide.

    Initial try was cut at 2 mm width (radial) and 2 mm depth (helical lead) into the wall (Z axis).
    The mill was complaining and I was stressed.

    Reduced cut to 1 mm width and 1 mm depth, to hole depth of 16 mm.
    I will clean bottom to 17 mm depth with the solid carbide.

    Mill was certainly being used, more than I normally push it.

    Did multiple passes, each 2 mm more on the diameter, with cut last pass 0.5 mm width (to Dia 35 mm).
    Finish is excellent.

    Odd observation is the helical witness marks in the upper part of the hole.
    And rougher surface (visual only, no feel) in bottom half of the hole.

    My working hypothesis is that the tip side edge (at the top) rubs on the hole side.
    Then the rubbing upsets the tip, causing the rougher surface finish.
    The tip clamped in the tool holder may be at fault, or bad geometry design.
    I will review closely with my mate when he visits next.

    Please, no comments on the slim wall thickness left for the bearing fit.
    I queried the customer, and supplied a sample with Dia 33.5 hole, to no avail.
    Customer says this design used without any problems for 20 years.
    Apparently the bearing has a rubber liner when it goes into the hole !

    Helical Drill Tipped Tool compr.jpg

    Keep well,
    John.

Similar Threads

  1. Helical gear maker?
    By nadroj in forum METALWORK GENERAL
    Replies: 66
    Last Post: 27th May 2021, 10:19 PM
  2. video: cutting helical gears
    By StrayAlien in forum METALWORK GENERAL
    Replies: 8
    Last Post: 12th May 2020, 11:32 AM
  3. Cutting helical gears
    By Michael G in forum METALWORK GENERAL
    Replies: 12
    Last Post: 1st Apr 2015, 10:12 AM
  4. Helical gear confusion
    By Ueee in forum METALWORK GENERAL
    Replies: 4
    Last Post: 10th Apr 2012, 01:10 PM
  5. Helical milling
    By Michael G in forum METALWORK GENERAL
    Replies: 1
    Last Post: 21st Oct 2011, 01:37 PM

Posting Permissions

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