0-80 Threading

[Jake L]

I have some 0-80 threads I need to machine in 6061 aluminum. The problem is the depth of the hole is called out as .200+/-.01 and the min thread depth is called out as .130. Also, there's 35 threaded holes per part and we have to make 50 parts, so I'm hoping whatever method is used results in good tool life.

I was hoping I could buy a 0-80 bottoming tap but I have not been able to find one of those. It seems form tapping is the usual method for 0-80 threads, but I'm not sure I have the blind hole depth to get the called out thread depth.

I'm sure someone on this forum has done this before and knows a good method of machining this feature. Any help is very much appreciated.

[JParis]

Typically I can get an 0-80 rollform .010/.015" off the floor using rigid tapping...the guys will creep down it

.070 is plenty of clearacne for a rolltap

[dolphin1]

so is the depth of the hole to bottom of hole or body diameter for drilling. if its to depth then the drill tip is .012 for a .055 drill with 135deg and you can run a form tap within .010 to .015 of the body depth. shouldn't be a problem. at .175 tapping depth you should end up with a thread depth of .135-.140

[Jake L]

Depth of hole is .200+/-.01 body diameter. Our shop is just starting to use form taps. It seems like we are going to save a lot of time threading holes with these things. I didn't realize you could get so close to the bottom of a blind hole with a form tap.

The only other question I have is, is there an easy way to figure out what size you have to drill and/or ream the hole for a form tap? Or is trial and error our best bet?

[Clamper Todd]

This has served me well...

https://www.balax.com/holesizecharts

[JParis]

46 minutes ago, Jake L said:

The only other question I have is, is there an easy way to figure out what size you have to drill and/or ream the hole for a form tap? Or is trial and error our best bet?

There are form tap charts...they do take a different(larger) size than cutting taps...make certain that wherever you get it that it IS a form tap chart

[cruzila]

These charts are the bomb!

 

https://www.balax.com/_files/ugd/dd22b6_06e8f9c929be4a23ae8e485f4228463f.pdf

[Tim Johnson]

Here is a thread calculator..

https://www.guhring.com/Tech/tapdrill

[rickt]

The size of the hole for form taps are much more critical.  Even more so for small screw sizes.  A little small and you will break taps.  Too big and you will get almost something like a double start thread.

Something to keep in mind are chips in the hole.  Even a small sliver could break a tap.

Not to scare you, just things to keep in mind.  I love form taps in blind holes and have done 1000's of 0-80s just need to cover the details.

Rick

[Leon82]

5 hours ago, rickt said:

The size of the hole for form taps are much more critical.  Even more so for small screw sizes.  A little small and you will break taps.  Too big and you will get almost something like a double start thread.

Something to keep in mind are chips in the hole.  Even a small sliver could break a tap.

Not to scare you, just things to keep in mind.  I love form taps in blind holes and have done 1000's of 0-80s just need to cover the details.

Rick

Yes, i've had m1.6 hole gauge fine with a plug gauge and a screw would basically push into the threads from a chipped drill.