Thanks Thanks:  0
Likes Likes:  0
Needs Pictures Needs Pictures:  0
Picture(s) thanks Picture(s) thanks:  0
Results 1 to 7 of 7
  1. #1
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    754

    Default Pockets and Rounding Cutters

    The photo shows the first 'paid' job on my CNC mill.
    This is a trailing wheel for a 5" gauge live steam loco, 18 mm thick and 105 mm diameter, made from 1045 bar.
    The spokes are recessed 2 mm from the rim, so the spoke thickness is 14 mm.

    GB Trailing Wheel Prototype 15Jun20 compr.JPG

    My mate made the disc on a Mori Seiki CNC lathe, my job is to mill out the pockets between the 7 spokes.
    This is a prototype wheel, with 20 production wheels to follow.

    The pockets are about 18 mm triangles with corners 5 mm and 3 mm radii.
    I drilled through on the curve centres at 9.5 mm and 4 mm, then milled out the pocket with a 6 mm solid carbide end mill.
    Cutter was 1200 RPM with feed at 100 mm/min, depth of cut 2mm, giving 8 steps.
    Side step-over was specified as 0.3, giving 3 paths for the pocket.

    The next job is to round off the spokes with a corner rounding HSS end mill, 1 mm radius.
    Single cut at 1 mm depth with speed 1000 RPM and feed 100 mm/min.

    Problems:
    a) the 6 mm carbide cutter rattles as it goes into the corner holes,
    b) the corner rounding cutter leaves witness marks at top and side and the rounding has a poor presentation.

    Discussions:
    a) I intend re-doing the design to specify the corner radius as something greater than 3 mm, say 3.1 mm.
    I have also been told that a single large hole in the middle of the pocket is preferred. A 13 mm drill is practicable.

    Do the speeds, feeds and cuts seem efficient ( with 20 to come ! ),
    Single 13 mm drill ?
    Coolant ?

    b) I think I need to increase the rounding cutter radius to 2 or 3 mm, but contact with the hub and rim is a risk.
    Perhaps a different cutter shape would be better.

    Any suggestions on how to get a nice rounded spoke edge ?

    Keep well,
    John.

  2. #2
    Join Date
    Jan 2012
    Location
    Melbourne
    Posts
    118

    Default

    Hard to avoid a chirp in the corners, engagement angle and all that.
    Maybe try leaving .05mm and then a full depth finish pass ? Needless to say minimize the cutter stickout, a short cutter with four 16mm flutes would be good.
    If your CAM will handle it: model the wheel, then, after the 2D work, pick out the the fillet surfaces and cut them 3D with a 6mm ballnose.
    Neil

  3. #3
    elanjacobs is offline Apprentice gear maker and machine doctor
    Join Date
    Aug 2008
    Location
    Melbourne
    Age
    30
    Posts
    476

    Default

    As a rule, your cutter radius should always be less than any internal corner radius you need to cut to avoid it grabbing as it makes full contact.

  4. #4
    Join Date
    Mar 2014
    Location
    South of Adelaide
    Posts
    683

    Default

    problem A: I don't think R3.1 will be enough to stop it chattering, you may need to go R3.5 or use a 5mm cutter. Are you programming by hand or using CAM? if CAM what program?

    Problem B: you will need to adjust your tool offset to get the rad to blend properly, I'm yet to have a corner rounder cut properly with theoretical values.

    Speeds and feeds: the feed per tooth is about right on the endmill, but the RPM is very low, i normally work on 80-100 M/min, but not sure on the capability of your machine or quality of your endmill.

  5. #5
    Join Date
    Apr 2009
    Location
    Kingswood
    Posts
    754

    Default

    I will discuss with my 'customer' the R3.5 question, and/or his supply of a Dia 5 mm cutter.
    Tools are LibreCAD and CamBam.
    CamBam lists a facility to import STL files, but its ability to generate code for a ball mill is unknown.

    Tonight I tried a HSS V cutter to add a 45 degree chamfer in lieu of the rounding in one of the pockets, looks interesting.
    Intend a shopping trip to Mick Moyle and McJing soon with one of the items being rounding cutters.

    At 100 m/min rated cutting speed for carbide on steel, the spindle would be at 5000 RPM, not safely achievable at the moment.
    I can get there in theory, but friends have suggested the bearings may only be rated to 3500 RPM.
    The finish is OK (it is a railway wheel !), but a higher speed will be tried.

    The various pockets were done one at a time over a couple of days, and datum registration has been lost.
    Made a Dia 10 mm pin held in the large curve of the pocket to pick up the registration for the rounding, but errors inevitably creep in.
    A couple of 'learning experiences' didn't help.

    Hopefully, production wheels will be done on a fixture at one setting, with a general improvement.
    The fixture will have a fairly deep cavity below the wheel for the chips to drop into.

    Keep well,
    John.

  6. #6
    Join Date
    Mar 2014
    Location
    South of Adelaide
    Posts
    683

    Default

    I'm unfamiliar with CAMbam, but the other Cam software i have used, Fusion 360 and Featurecam, have milling strategies that will keep the angle of engagement of the cutter constant when machining tight corner. Eg. As the cutter goes further into the corner the radial depth of cut decreases. This would help reduce chatter in the tight corners, but might make your cycle times too long considering the speed of your mill.

  7. #7
    Join Date
    Nov 2014
    Location
    Derbyshire
    Posts
    2

    Default

    Quote Originally Posted by electrosteam View Post

    The pockets are about 18 mm triangles with corners 5 mm and 3 mm radii.
    I drilled through on the curve centres at 9.5 mm and 4 mm, then milled out the pocket with a 6 mm solid carbide end mill.
    Cutter was 1200 RPM with feed at 100 mm/min, depth of cut 2mm, giving 8 steps.
    Side step-over was specified as 0.3, giving 3 paths for the pocket.

    The next job is to round off the spokes with a corner rounding HSS end mill, 1 mm radius.
    Single cut at 1 mm depth with speed 1000 RPM and feed 100 mm/min.

    Any suggestions on how to get a nice rounded spoke edge ?

    Keep well,
    John.
    Can you have a draft on the sides of the spokes? I made two wheels for a model engine for a friend and have had some good results using a tapered ball nosed cutter with a side angle of 5 degrees, I made an STL file to round over the spokes and clean down to depth the sides so leaving a nice round over finish with tapered sides.

    I'll see if I can dig out the STL and post it here to give you an idea what I am saying.

    Keep safe
    Phill

Similar Threads

  1. Sunderland gear cutters and cutters
    By Somedayplumbing in forum EBAY, GUMTREE, and other off forum sales sites
    Replies: 2
    Last Post: 28th Aug 2019, 10:34 PM
  2. Gear tooth rounding
    By caskwarrior in forum METALWORK GENERAL
    Replies: 8
    Last Post: 6th Apr 2019, 09:15 AM
  3. Rounding key ends
    By bob ward in forum METALWORK GENERAL
    Replies: 15
    Last Post: 31st Oct 2018, 07:11 AM
  4. Replies: 8
    Last Post: 4th Sep 2017, 09:13 AM
  5. cutters ?
    By morrisman in forum METALWORK GENERAL
    Replies: 4
    Last Post: 4th Sep 2014, 10:36 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
  •