×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

drilling and tapping Inconel
4

drilling and tapping Inconel

drilling and tapping Inconel

(OP)
i never worked with inconel and need to know what kind of drill and taps i'll need and any tips on coolant and feeds and speeds .             thanks hooked

RE: drilling and tapping Inconel

4
1. Cutting fluid/coolant: for slow operations like drilling, boring, & tapping, use heavy lubricants, like sulfurized oil.  Water-based fluids are preferred for high-speed turning, milling and grinding because of the greater cooling effect.

2. Drilling: use steady feed rates-- don't allow the tool to dwell, which causes work hardening at the bottom of the hole, and makes cutting more difficult once it resumes.  Set-up should be as rigid as possible, using stub drills and jigs where possible.

Heavy-duty high speed steel drills with a heavy web can be used.  Grades T15, M41, M42, & M43 are recommended. Carbide tools are also used.  TiN coated tools will have lower friction, hence reducing tool temperature and wear.
To minimize work hardening, use positive rake angles with adequate relief.  Cutting pressures are reduced and a positive effective rake maintained if the web is thinned at the chisel point.  Increasing the point angle to 135 degrees can be helpful.

Feeds and speeds: For unaged condition, speed should be 3-4 m/min, or 10-12 sfm.  Aged condition is 2-3 m/min, or 8-10 sfm.  Feeds depend on diameter:

Drill diameter    Feed
mm                mm/rev       
<1.5              0.0125-0.025
1.5-3             0.025-0.05
3-4.75            0.05-0.10
6-8               0.075-0.125
9.5-11            0.10-0.175
13-17             0.15-0.25
19-25             0.20-0.38

3. Tapping: Drill size should be 50-55% of thread depth.  Speeds should be ~ 1.5-3 m/min or 5-10 sfm.  Inconel alloys are best tapped using serial taps, which are standard taps modified in diameter so that each successive tap increases the thread diameter proportionately.  Tap in the unaged condition if possible.  Ample cutting fluid is necessary for either hand or machine tapping; chlorinated waxes being the preferred type.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources