UNJF thread

[David Colin]

Hi,

I have #10-32UNJF internal threads to machine. I usually do that with cutters from Horn-CPT or Vargus but on this one i need to follow standards from an american plane builder...

That means for a #10-32UNJF internal thread, i have to machine a root radius between 0.0025"/0.003". I checked all cutters i usually use but they are grinded flat.

Anyone knows of suppliers (with French/European representatives...) of thread cutters complying with this root radius?

[So not a Guru]

The UNJF spec (we use AS8879 for aircraft work, as required by our customer) does not require a root radius on the internal thread, only on the external thread. The only difference from a UNF thread for internal threads is a larger minor diameter hole size.

[David Colin]

Yes, i know that and this is how i always did it. But here we need to comply BACD2086 specifications from B****G which requires a root radius on internal thread (Rmax=.096p/Rmin=0.075p)

[So not a Guru]

Harvey tool, I believe, will make a custom threadmill for you.

[So not a Guru]

An interesting article on the arbitrary nature of this change.

 

http://www.ring-plug-thread-gages.com/ti-UN-BACD-2086.htm

[David Colin]

This was interesting and it probably improves part mechanical qualities but... it's really annoying to find the tool to do it^^ However, this standard has been created in 1987 and it seems it's still not really popular for toolmakers.

[Newbeeee™]

Be careful of the single point tool manufacturers. They always are near sharp and sometimes have a good couple of degrees tolerance on the 60degree.

Amazing (to me) fact - for ISO metric threads covered by the British Standards, there is no tolerance for the 60deg flank angle.

It appears that as long as the OD, Root, and Pitch Diameter all fall within their tolerances, the flank angle doesn't matter...

[gcode]

3 minutes ago, David Colin said:

This was interesting and it probably improves part mechanical qualities but... it's really annoying to find the tool to do it^^ However, this standard has been created in 1987 and it seems it's still not really popular for toolmakers.

Is this an old part you're building... calling out an obsolete spec ???

maybe you could get a variance to use a modern spec

[David Colin]

This is a not so old part (B777 aircraft) and my customer won't change this... I tried before to ask here^^

[?Mark]

Good luck measuring it.

 

"The UNJF spec (we use AS8879 for aircraft work, as required by our customer) does not require a root radius on the internal thread, only on the external thread. The only difference from a UNF thread for internal threads is a larger minor diameter hole size. "

 

+1 to so not a guru ^^

[MIL-TFP-41]

I have had to deal with this before....a controlled root radius on an internal thread. Boeing & Parker have their specs for this. When I was doing alot of manifold work, this was all we saw. Unfortunately, custom tools were the only solution. We had OSG make special taps, but $$$ (but worth it for 1000's of holes). Threadmills were much more affordable.  It also requires a custom Go/No Go gage....the OD of the gage must be truncated in order for it to clear the root radius.

[David Colin]

I know... but it's easy to check tool geometry so if they come in my shop to tool list and tool definition, they will discover i'm using a standard tool.

[?Mark]

90% of my work is JSF, so J type threads are the most common forms with Lockheed. Thankfully, we only make external J threads.

In your case, just get a single point from Micro1000 (I prefer Micro100 over Harvey in single point tread end mills) and have either them or someone else modify the corner to a radius instead of flat.

[Watcher]

My take on this... 

If a custom tool is required anyway, I'd start with a custom tap. 2nd option thread mill. 

I'd get a tap made by one of the big players (OSG, Emuge, Titex, etc) because they master this sort of profile and are well familiar with the standards. 

[David Colin]

Thank you all. I ll go with a custom single point mill because of time, I will quote taps but I usually prefer threadmills with that combination material(15-5PH 360/400HB)/small hole size deep 3xD.

Thank you for Go/No go gage. I would have probably forgot it.

[MIL-TFP-41]

I know from bad experience on the truncated go/no go gage

It is possible to open up the threads till a regular go gage runs in. Unfortunately by the time you do, the pitch diameter is going to be oversize.