Need Help! Thread mill steel


Results 1 to 12 of 12

Thread: Thread mill steel

  1. #1
    Member
    Join Date
    Mar 2010
    Location
    UK
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Thread mill steel

    Hello I have a piece of 1/2" cold rolled steel I wish to make a fixture plate for a SMW Mod vise on my 770. I have chosen to thread 1/4 -28 rather than 1/4- 20.
    My Cam software supports thread milling. (VisualMill) I think each pass is of equal amount. As I use metric in pathpilot I will have to convert thread pitch to mm
    I have not used thread milling before and would like advice on Spindle speed and depth for each pass. I have no issue with how long this takes and would prefer not to break the cutter I have ordered from Tormach. I have about 30 holes to thread
    I can raise plate to allow coolant and chips to go through which I think will help.
    Thanks in advance.
    John.

    Similar Threads:


  2. #2
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5728
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    1/4" is a bit small for thread milling. I'd use a tap instead. If you've got a Procunier or other tapping head, this would be in its sweet spot.

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  3. #3
    Member
    Join Date
    Mar 2010
    Location
    UK
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    With the absence of advice, apart from do it another way! I am going to try a step over of 0.2mm, (0.008" ), a feed rate of 90 mm /min (3.5" /min) and a spindle speed of 7000 RPM and see how I get on. Hopefully the tool will hold out.



  4. #4
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    I have never threadmilled anything, but the rpm sounds a bit high for steel?? 3500 may be better to start.

    mike sr


  5. #5
    Member
    Join Date
    Nov 2013
    Posts
    4283
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Hi,
    you have not told us anything about the tool. Is it a single disc cutter or is a 28tpi thread mill?. Is it carbide or HSS? Is it coated?
    How thick is the shank...that is to say the narrowest bit just above the cutter....its the most tender part of the whole thing.

    I use a single point carbide boring bar and I spin it at 24000rpm, and that will do down to 3mm threads, its small and tender, and I've broken three of them over several years.
    You tend to break them rather than wear them out.

    Craig



  6. #6
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Threadmills need to climb-mill, so for a right hand thread, start in the centre bottom of the hole, and helix into the cut going CCW, and screw out. This avoids re-cutting chips that tend to wear/break the root radius on the cutter.
    Through coolant (best) or flood required.
    RPM is of lower importance (get it close to OEM specs), but feedrate is. Depending on tool diameter, you may only be doing a 0.080" circle, so start slower.

    Gun tap would be the cheapest, fastest, least risky method around for a through hole.
    Machine tap for blind holes.
    Threadmill if you have the know-how, and tooling



  7. #7
    Member
    Join Date
    Mar 2010
    Location
    UK
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Many thanks guys. I know this is not the easiest way of making threads but I really don't want to hand tap 30 holes.
    A good point made regarding going in slow for its first cut.
    The thread mill has not arrived yet, which is a single point carbide, coated cutter. I guess the cutter will be about 5 mm dia and the narrow shank about 3 mm x 1/2" long.
    If I can get it to survive the first few holes, it may complete the job without breaking. One way or another I will learn something useful !!



  8. #8
    Member
    Join Date
    Nov 2013
    Posts
    4283
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Hi,
    with a 5mm diameter cutter that suggests 6367rpm is a surface speed of 100 m/min, which is about right for coated carbide in steel.

    The real issue is that the shank is very tender and will break if you attempt to load the tool overmuch. On the other hand you can try to be 'so gentle' that the
    tool is no more than rubbing the material....you need to fin a balance in between.

    I use a lot of small diameter (sub 1.5mm) tools and as a rule of thumb I use 1% of tool diameter per tooth per revolution. For example a four flute 1.5mm tool at 24000rpm:

    0.01 x 1.5 x 4 x 24000=1440mm/min

    In your case i would suggest:

    0.01 x 5 x 4 x 6367=1273mm/min Note this assumes the cutter has four teeth. Note also this is just a rule of thumb......you could and probably should reduce this to 1/4 or less
    until you have established that its suitable.

    The next question is the depth of cut per pass. That has to be gauged on the strength of the shank. It also depends quite a bit on the Gcode.
    For instance if you repeat exactly the same path but at increasing depth at each pass the vertex of the tool travels the same path and both flanks of the flute/tooth
    engage the material. If however the toolpath shifts the path the vertex follows such that only one flank of the tooth cuts it halves the torque borne by the tool.

    May I suggest before you use your expensive tool you try some experiments. When I first tried thread milling I used a HSS tap and ground every tooth off it bar one, and
    reduced the shank such that the one remaining tooth could cut to full depth but the shank of the tool did not touch the surface of the material. It was slow and a learning
    curve...but it worked. That is where I discovered the idea of moving the toolpath say 0.05mm per pass to ensure that only one side of the cutting tooth was working.
    This idea I got from lathe practice where expert operators try to arrange successive passes such that one side only (of the tooth) is cutting.

    I use a tiny carbide boring bar now. It has one tooth, conveniently 60 degree included angle, just right for a thread. The shank is about 1.5mm square so you have to be gentle with it!!!!
    The clamp is 1 inch....just to give you a hint of the scale....its small.

    Craig

    Attached Thumbnails Attached Thumbnails Thread mill steel-microboringbar-jpg  


  9. #9
    Member
    Join Date
    Mar 2010
    Location
    UK
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Craig,
    Many thanks for taking the time to reply in such a clear and detailed way. Much appreciated. I have a simple cutter grinder and will take up your advice.

    John.



  10. #10
    Member scott216's Avatar
    Join Date
    Apr 2012
    Location
    United States
    Posts
    159
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Saunder's NYC CNC website has a page on threadmilling. It has links to videos and spreadsheets to help with calculations:

    https://nyccnc.com/how-to-threadmill/

    --Scott

    "You can't teach stuff in a school that you would learn in real life unless the real life people are in charge of the school." - Gene Sherman


  11. #11
    Member
    Join Date
    Mar 2010
    Location
    UK
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    Many thanks to those to replied to this.
    All 30 threads have now been threadmilled . The cutter is still sharp and still in one piece! Settled on three passes, 4000 rpm and a 85 mm/min feedrate.

    John.



  12. #12
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: Thread mill steel

    My hats off to you John!
    30 holes and never threadmilled before, cutter stil in one piece, small hole to boot. I figured you would have broken at least one tool in the process!

    mike sr


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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Thread mill steel

Thread mill steel