cut taps with less "tool pressure"

[jeff]

Do they exist?

We have parts where a bolt circle is close to a tight tolerance bore and they mushroom out about .0005" on the diameter making the fitting part not go in, forcing us to polish out the bores.

 

Right now we're using standard M8 Guhring 3 flute plug taps after using a carbide drill with thru coolant, if there is a tap that cuts free-er (is that a word?) I'd try it.

 

Thread milling is not an option because of thread depth.

 

materials are 4150pht and 8620 that's been carbeurized.

[AMCNitro]

How deep is the thread?

[jeff]

they range from 1.5" to 2" thru.

[cncchipmaker]

Why don't you cut the bores after you tap?

[AMCNitro]

they range from 1.5" to 2" thru.

WOW! I see what you mean about thread mills.  How about cutting the threads before finishing the bore?

[jeff]

Why don't you cut the bores after you tap?

Because they are helical gears, od is flame hardened and the lathe finishes the ID before the mills so it's round and we have something to pick up.

Then we locate off the bores to mill the parts. 

Finishing the bores after milling would require another op in the lathes.

 

I wonder if a tap with more flutes will help?

[Machineguy]

Re think your processes.

8620 and 4150 will move in heat treat.

tapping is a high pressure op unless you thread cut them.

Why aren't you drilling and tapping the holes OS before heat treat. True position not big enough?

The bore is the main Datam for location and size.

sometimes you need to add a op to make the part right.

 

 

Just thinking out loud here.

 

Machineguy

[jeff]

Re think your processes.

8620 and 4150 will move in heat treat.

tapping is a high pressure op unless you thread cut them.

Why aren't you drilling and tapping the holes OS before heat treat. True position not big enough?

The bore is the main Datam for location and size.

sometimes you need to add a op to make the part right.

 

 

Just thinking out loud here.

 

Machineguy

 

Because there is more mill work than just the tapped holes.

There are dowel holes and tight tolerance slots as well.

 

Actually we do cut the 4150pht parts before heat treat, but the 8620 we cut after carb and the teeth are flame hardened.  The mill work is nowhere near the flame hard spots.

 

The process for the 8620 parts is:

Lathe green turn

Customer rough cuts teeth

Customer sends to heat treat

customer finishes teeth

finish turn

mill

assemble

ship.

[Mjölnir]

we usually turn to our Emuge sales rep for difficult tapping jobs. 

 

http://www.emuge.com/emuge-tapping-tools

[specv]

you might want to see if there are skip-taps for that size. I know we had an issue like this and it was fixed by using a skip-tap.

[jeff]

you might want to see if there are skip-taps for that size. I know we had an issue like this and it was fixed by using a skip-tap.

 

Is that a tap similar to the interrupted NPT style taps? Where every other tooth is ground off?

[specv]

Is that a tap similar to the interrupted NPT style taps? Where every other tooth is ground off?

 yes, 

Also Helical flute taps put less pressure than straight flute as well.

[specv]

http://www.besly.com/store/home.php?cat=312&&sort=title&sort_direction=0

[mkd]

what dia threads @ 2" deep?

hard to believe thread mill is not an option.

buddy used to mill 2-56 and 4-40 in inconel.......

 Reading comprehension: M8

 

now i'll argue with the designer: that thread depth far out weighs the strength of the bolt minor dia. What is he thinking?

 

skip-taps

 

learn something new every day.

[specv]

Also called interrupted taps,

Emuge makes them http://www.thomasskinner.com/default.aspx?page=item+detail&itemcode=EMU-B01210010080&catlist=3338

[jeff]

what dia threads @ 2" deep?

hard to believe thread mill is not an option.

buddy used to mill 2-56 and 4-40 in inconel.......

 

 

learn something new every day.

M8 thread

[RaiderX]

Prob some better suggestions already posted but OSG exotaps come to mind.

[mkd]

might be interesting what the designer has in mind: bolting from both sides, where a continuous thread thru is not needed or he just got lazy with the callout.

[jeff]

Ok, I was incorrect.

They are M10 taps, thru hole but only tapping 1-3/4 deep.

I asked my guy and he said that tap has been in use for many many holes (stupid me assuming he tried a new tap), so we're going to pop in a brand new one and see how that works.

Thanks for all the suggestions!

[jlw™]

Skip tooth taps is all we run in NPT and BSPP. Emuge would be my first choice.

[Colin Gilchrist]

Can you open up the tap drill size? It would give slightly less thread engagement, but would also require less tool pressure to cut the thread. I like the ideas already given for skip tooth, and helical flute taps.

[cncchipmaker]

Because they are helical gears, od is flame hardened and the lathe finishes the ID before the mills so it's round and we have something to pick up.

Then we locate off the bores to mill the parts. 

Finishing the bores after milling would require another op in the lathes.

 

I wonder if a tap with more flutes will help?

You are already adding another op by having to rework the bores.

[jeff]

You are already adding another op by having to rework the bores.

Only when the mating part doesn't fit.

The problem arises about 1 every 10 parts or so, and we only do about 30 a month. So it's not really THAT big of an issue, but it's just something I am wanting to prevent.

Going to a new tap seems to help fix the problem, as long as the lathes hold the bore to the high limit and the mating parts are ground towards the low limit giving us .0006" of flexibility.

[jlw™]

Chamfer them at least deep enough to be larger than the major diameter.

[jeff]

Just a quick update:

We just drilled the holes and checked the bore before tapping, it's the tap drill that is pushing the material not the tap.  

Guhring solid carbide, thru spindle coolant drill, it's in great shape,but we're swapping it out for a brand new one and running another part.