Thread Milling >50 HRc Steel

[dfedwards]

Does anyone have any success stories for thread milling 5/16-18 unc-3B in 4140 heat treated to 50+ HRc? Traditional threadmills are not holding up and we have 60 holes to thread. If anyone could suggest tools for this. I have found some in Metric but to get the tools in Inch would be a special and the lead time is 6-8 weeks. Need something that is hopefully available off the shelf. Thanks.

[McLaren]

Vardex H3/8".205"-I18UNCTM

 

EDIT: That part# might be invalid. Checking now.

[McLaren]

Coolant thru 1.5X D:

HC31242L04-I18UNCTM VTH

EDP# 80363

 

Link to all of the options:

http://www.vardexusa.com/files/Solid%20Carbide%20Catalog%20_Inch%5B171109%5D.pdf

[dfedwards]

Thanks McLaren, I will give them a try.

[jeff]

How fast are you running it?

What is the actual Rc of the part?

50Rc isn't that hard to cut, but 58 it starts to become not fun.

[Mr. Wizzard]

Carmex

[[email protected]]

Carmex

 

YES! I've used these on 420ss 60Rc 3/8-16 with air blast and they cut great. I ordered 2 but only used 1 on 20+ holes

[bogusmill]

I cut RC52 Vascomax 350 threads with Scientific single flute thread mills and they last quite a while. MSC carries them.

[peon]

I didn't know 4140 could be heat treated properly through the thickness of the steel. I thought you could only case harden that stuff. If that is the case, the holes you need to threadmill may be soft (less than 30 RC).

[MIL-TFP-41]

http://www.lakeshore...hreadmills.aspx

 

great stuff....and beats carmex prices by a long shot....tho carmex is an excellent tool also

[dfedwards]

Thanks for all the input, the parts are checking to be 56Rc which is at the top of the blueprint callout. Didn't try Lakeshore yet, Carmex is working extremely well, I decided to let well enough alone, we have threaded 60 holes so far without even adding any cutter comp for wear yet.

[Hardmill]

Thanks for all the input, the parts are checking to be 56Rc which is at the top of the blueprint callout. Didn't try Lakeshore yet, Carmex is working extremely well, I decided to let well enough alone, we have threaded 60 holes so far without even adding any cutter comp for wear yet.

 

 

 

What are the speeds and feeds your running at ??

 

Ive had great success with up to 60rc and 10-32 holes.

 

 

 

 

 

 

 

PEACE

[dfedwards]

120 SFM (Ø.236 = 1950 RPM) and .0012 IPT (3FL = 7 IPM)lasting approx. 60 holes after that we start having to chase the P.D. with cutter comp so we just change the tool at that point. Is this inline with your results Hardmill?

[Hardmill]

120 SFM (Ø.236 = 1950 RPM) and .0012 IPT (3FL = 7 IPM)lasting approx. 60 holes after that we start having to chase the P.D. with cutter comp so we just change the tool at that point. Is this inline with your results Hardmill?

 

 

 

Nope

 

I was doing about 1000sfm .0003-.0005 chip load.

I know it might seem excessive but that the nature of hardmilling.

 

Gotta throw out conv machining thoughts and go for it. It a diff animal for sure.

 

What type of machine do you have and what are the limits of your speeds and feeds.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[dfedwards]

Mazak Variaxis 500-5XII 5-axis. 12k spindle. I am running high speed toolpaths all over the shop using chip thinning with great results, guess I never thought to apply to thread milling - just took the mfg's suggestions and went with it. We typically do not machine materials above 50Rc, We cut a lot of Titanium, 15-7, 17-4, 13-8MO and carbon steels that usually are under 43Rc and quite a bit of aluminum too. We cater mostly to aerospace and defense and are branching out into oil industry (getting nervous about having so much of our customer base in the defense industry).

 

Sorry, wandered off-topic. Back to threadmilling at 1000sfm, do you take that in multiple passes or one pass?

[Hardmill]

 

Sorry, wandered off-topic. Back to threadmilling at 1000sfm, do you take that in multiple passes or one pass?

 

.001-.002 per pass but at those speeds it goes really quick with great results and repeatability.

I always thow a spring pass in for good measure also.

 

Air through the spindle is best. Coolant at those speeds will just destroy your tool.

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE