508,289 active members
2,853 visitors online
Register for free
Login
Results 1 to 10 of 10
  1. #1
    Junior Member
    Join Date
    Nov 2010
    Posts
    8

    Gear hobbing on a cnc mill

    I would like to hob a gear on my cnc mill using the 4th axis and need some help.Its an xyz 1020 vmc running Siemens 828 controls.It works with both Sinumeric or Fanuc style g code programming.I have a 0,3 module gear hob.Please note this is a hob, not an involute cutter , and so it needs to run at a set speed in relation to the 4th axis.The cutter needs to turn 100 times faster than the 4th axis to cut a 100 tooth gear.This bit i can do. If i program S495 and a feed of 1800°/minute for the A axis. That relates to the 4th axis turning at 5rpm.All fine and well, and that will give me the 99 teeth on the gear that i need.

    Now, how can i program a different feed rate in mm/min to contol the actual motion of the x and y axes to work in conjunction with the A axis?Surely there must be a way of doing it, either with f groups or possibly with a feed inversely proportionate to time? One of the G codes in the 90's does this. Any advice would be most welcome !

  2. #2
    Gold Member
    Join Date
    Aug 2011
    Posts
    2517
    for a straight spur gear the correct dual sync'ed rotation creates your required gear teeth.

    I don't have info about your exact hob or the way its set up but normally the feed is not related to the rotation and gear-forming process. feed the hob like you would any other milling tool.
    if your hob is spinning at 495rpm and it has 8 teeth and you want to take 0.05mm per tooth then 495 * 0.05 * 8 = 198mm per minute.
    however this is not like cutting a thread on a CNC lathe as the axis are not really in sync. It will work for one pass but if you move off the part then try to go back (for example to take a finish pass) the rotation of the hob will not be in sync with the rotation of the part.
    for machines that are equipped to do hobbing usually there is a G-code to sync the axis so you can move about anywhere and still be in sync (like on a CNC lathe while cutting a thread with G76 for example.)

    just test the theory first on a scrap piece of material and you will soon figure out what's going on.

  3. #3
    Junior Member
    Join Date
    Nov 2010
    Posts
    8
    Thanks for the reply.What i was trying to get across was how do i program in a feed in degrees per minute to drive the 4th axis in the right ratio to the spindle speed,ie 99 times slower than the spindle and get a feed rate for the x axis at the same time? I have come up with a way of doing it , with a bit of a cheat involved.Hope to try it out tomorrow. I have programmed in SPOS=0 to get the spindle to always start in the same place and A0 before the spindle starts.Tried using an extension of G95 and linked the 4th axis to the spindle rpm, but was more hassle than its worth.Got the program written with 2 passes, looks good so far.

  4. #4
    Registered
    Join Date
    Nov 2005
    Posts
    195
    Hobs need to be set at an angle. Can this be done in your mill?

  5. #5
    Junior Member
    Join Date
    Nov 2010
    Posts
    8
    Yes i can.On my old shw mill it would have been alot easier though! What i have done is machined a spacerplate that fits under the 4th axis,the top of which is at 20° to the bed of the mill.That will give the the required 20° pressure angle.Milled that awhile ago but was too big for my little surface grinder,so have had to send it out to a friend of mine for surfacegrinding. Only problem with friends and favours is you cant hurry them along too much if you want to keep them as friends:stickpoke

  6. #6
    Registered
    Join Date
    Nov 2005
    Posts
    195
    A spacer plate with the correct angle should work fine. You don't set it to the pressure angle though. Is there another angle written on the hob? I'm not sure of the correct term. Lead angle? Helix angle?

  7. #7
    Registered
    Join Date
    Mar 2006
    Posts
    2712
    Pressure angle is controlled by the shape of the hob teeth.

    As T Ted said, the angle of the tilt is the lead angle. If this angle is not correct, the resulting tooth form will not be correct. The gear will not have a true involute which produces a rolling action. If the tooth form is incorrect, you may end up with a sliding action or even a binding action. Either will not be good.

    Dick Z
    DZASTR

  8. #8
    Registered
    Join Date
    Nov 2005
    Posts
    195
    I'm thinking this probably won't work even if he gets the angle correct. The hob & workpiece need to be in sync. If you program the table to turn 60 rpm & actually get 59 rpm then you'll end up with a helical intead of a spur gear or maybe you'll just be milling down the OD. I'd take a trial cut just a .001 or .002 deep.

  9. #9
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Posts
    4826
    If the OP's method works at all, I'd be surprised. Why do we bother with rigid tapping if we can just guess a spindle speed and run a tap down the hole?

    That said, you could 'hob' the gear by using a rigid tapping cycle, and run the hob past the gear just as though it were a worm running across a stationery gear. Then index the gear one tooth and rigid tap the next one. It would be a lot of tapping cycles!

    I've cut worm gears this way with a single tooth flycutter. Typically, I'd cut several times around with advancing depths. Then when full depth is reached, I do a partial index of the gear blank (say 1/2 a tooth), change the height of the rigid tapping cycle, and run it through again. This time, the cutter takes just a light shaving off the tooth face to help generate the involute curve. Do this in about 6 different positions, and you get a reasonable facimile of a hobbed tooth.

    Now if you actually have a hob, then you might get away with fewer partial indexings to generate a nice tooth.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  10. #10
    Registered
    Join Date
    Nov 2005
    Posts
    195

    Where'd he go!

    We seem to have lost the original poster.

Similar Threads

  1. Mini-Mill Gear hobbing
    By andypugh in forum Benchtop Machines
    Replies: 3
    Last Post: 04-03-2010, 02:52 AM
  2. Gear hobbing
    By Dooda in forum Mazak, Mitsubishi, Mazatrol
    Replies: 0
    Last Post: 11-16-2009, 03:54 PM
  3. gear hobbing....
    By Chris D in forum General Metalwork Discussion
    Replies: 23
    Last Post: 02-27-2009, 08:41 AM
  4. Gear hobbing on a VMC
    By dcoupar in forum Fanuc
    Replies: 1
    Last Post: 09-11-2007, 10:11 PM
  5. gear hobbing on mach3
    By rasta in forum Mach Wizards, Macros, & Addons
    Replies: 0
    Last Post: 07-30-2007, 12:56 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
  •