Tapping versus Thread Milling

[dandrummerman21]

My answer and suggestion would be related to the following: do you anticipate doing more m16 holes? I'd tap that every day. But I've got several m16 taps, and we use em a few times a year. At least its a standard and a tap might be 30 bucks give or take a few.

You don't anticipate doing more, but you anticipate doing more oddball metric threads of around the same size, with maybe some oddball pitches mixed in? Threadmills are neat. More expensive but neat.


If you don't have a thread gage, I would tap it as well. A new bolt is not quite a thread gage. Will get you in the ballpark but bolts vary a lot. A tap is unlikely to cut much oversize, and certainly won't cut under. If you threadmill it, you need to verify you put the thread within limits.

 

[dandrummerman21]

Hi mhajicek:
You wrote in post #7:
"I've used form taps in Ti6Al4V-ELI on short run production of 000-120 threads."

You are one brave dude if I do say so myself.
Form tapping 000:120 in Ti6Al4V?...you have my undying respect for making that happen.

And I thought I did some crazy shit.
Just goes to show yet again, that nobody knows it all and we can all learn something from one another.
I just learned something new and very cool from you today, so thank you for that!

If you'd pitched it to me, I'd have sworn you'd never get away with it.
Of course I'd have sworn thread milling it was going to be the Devil's very own too.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

I just threadmilled some #2-56 holes .200 deep in CP2 Ti and I nearly broke the threadmill looking at it. (single form threadmill).

This was only after scrapping a few parts using an OSG form tap. The form tap actually "cut" the thread oversize, my nogo went in. Minor diameter was perfect after threading but not the pitch diameter. I can't figure out why that was. So I bought a threadmill instead.

I think harvey tool sells threadmills down to a #00. That'd make my #2 look huge.

 

[david n]

Speedio tappin a M16(1:05) and a M33(2:38) in steel..........................

 

[crossthread82]

Speedio tappin a M16(1:05) and a M33(2:38) in steel..........................

Better yet that's a M16 form tap which takes way more torque to drive than a M16 spiral point cut tap.

A coated spiral point tap cut tap up to about a M20 in MS will run in any speedio. For bigger taps or bigish form taps you'd want the 10kHT spindle like in the demo video above. I probably wouldn't try a M16 form tap in MS though in a non HT machine but in aluminum it would likely be fine. Though ymmv, @BROTHERFRANK might be able to shed some more light.

 

[drcoelho]

I've got a 16K spindle on my machine

 

[BROTHERFRANK]

Being a through hole helps. You can run a tap with more lead which reduces torque required. Run that with a good collet that will not allow the tap to slip. Is the pitch 1.5? Program with G77 I1.5 . I would run around 800 rpm or so. Do you have a spare piece of material you can test tap so you don't scrap your work piece? Make sure your coolant has enough concentration and lubricity. Have fun...

 

[Mechanola]

As can tapped holes when the machine has Rigid Tapping, as it was said to be assumed by the OP. Simply adjust the Z Start position to get the required orientation.

You are right.

 

[mhajicek]

I just threadmilled some #2-56 holes .200 deep in CP2 Ti and I nearly broke the threadmill looking at it. (single form threadmill).

This was only after scrapping a few parts using an OSG form tap. The form tap actually "cut" the thread oversize, my nogo went in. Minor diameter was perfect after threading but not the pitch diameter. I can't figure out why that was. So I bought a threadmill instead.

I think harvey tool sells threadmills down to a #00. That'd make my #2 look huge.

If you need to go smaller:

WhizThrill Micro Thread Mills

WhizThrill micro thread mills by WhizCut.

www.whizcut.com

 

[dandrummerman21]

If you need to go smaller:

WhizThrill Micro Thread Mills

WhizThrill micro thread mills by WhizCut.

www.whizcut.com

No I choose to pretend threads smaller than a #0 don't exist.

 

[implmex]

Hi dandrummerman:
You wrote:
"No I choose to pretend threads smaller than a #0 don't exist."

That was BRILLIANT...I just about pissed myself laughing this morning.

May I do the same?
It will simplify my life quite a bit.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Wsurfer]

FWIW, S500 speedio.
I do1offs's in SS and 1018. I'm also a chicken, and peck tapping has worked well for me. Run 7% trim 685 coolant as I do mostly Aluminum. 1/2-13 is the largest I've done so far.

 

[DouglasJRizzo]

For the most part, I tap threads that are smaller than 3/4 and thread mill anything larger.
Running large taps is kinda scary to me, and even tho I've done a lot, I much prefer thread milling on the larger threads. A lot easier on the spindle, too.

 

[cosmos_275]

drcoelho, if you don't have a thread mill, they are nice to have and a good skill to have. I like them for bigger stuff and pipe taps. You need gauges though. With my CAM, I always end up iterating to get it just right. So, do a test piece. As already mentioned, they are slower and more expensive. I use Maritool single point thread mills. I think I have three and they cover 11-48 TPI.​

 

[cosmos_275]

Running large taps is kinda scary to me

Same here. I don't even like seeing the holder for a big pipe tap in my machine. Now, watching the thread mill rapid to the bottom of the hole takes some getting used to as well

 

[Mtndew]

Such a general description of the application you got there. Instead of explaining my thoughts further... Let's just take bets and see how it goes... I say tap failure is likely. Ofc as previously stated idk how stout a speedio is. Other people say 16mm is a cake walk for it. We shall see! Wish the op success for sure either way!

General description? I quoted you! And what I described is exactly what the OP needs to do to his parts.
I don't know WTF kind of taps you're using, but if they can't last 20 holes in mild steel 1" thru, then you need to buy better taps. Any decent tap should last hundreds of holes in mild steel. You DO know what mild steel is....right?

 

[Rstewart]

It's still generally preferable to Thread Mill from the bottom of the hole, particularly when a blind hole, simply because you're leaving the swarf behind rather than heading into it.

I like the ones you can go from top to bottom personally. The only problem I have with the bottom-up method is the engagement all at once if your threadmill has multiple teeth. It can be chatter city for some set-ups.

 

[implmex]

Hi Rstewart:
I seem to be missing something...I always thought the whole benefit of using multiple tooth threadmills was that you could engage them all at once, do a single circuit around the periphery of the hole and have all your threads done.

If that is so, I believe you will not chatter any more when climb cutting up from the bottom than conventional cutting down from above, because you will have almost the same number of teeth engaged, and as Bill (angelw) points out, upcutting out of the mess of chips you make at the bottom of the hole has benefits.

If you are considering spiraling down many turns from the top of the hole, why would you want a multi tooth tool...most of the teeth wouldn't be doing anything.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[crossthread82]

Hi Rstewart:
I seem to be missing something...I always thought the whole benefit of using multiple tooth threadmills was that you could engage them all at once, do a single circuit around the periphery of the hole and have all your threads done.

If that is so, I believe you will not chatter any more when climb cutting up from the bottom than conventional cutting down from above, because you will have almost the same number of teeth engaged, and as Bill (angelw) points out, upcutting out of the mess of chips you make at the bottom of the hole has benefits.

If you are considering spiraling down many turns from the top of the hole, why would you want a multi tooth tool...most of the teeth wouldn't be doing anything.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

What he may be referring to is a blind threadmill from OSG. No start hole, just helix the threadmill top to bottom through solid. It's still climb milling though b/c it's a left hand tool aka. spin it CCW. They're pretty neat, they make them for hard steel and aluminum. Really beneficial in a speedio where you have limited tool changer pockets but lots of speed available.

https://www.osgtool.com/at-2-inch

https://www.osgtool.com/at-2-r-spec

 

[angelw]

I like the ones you can go from top to bottom personally. The only problem I have with the bottom-up method is the engagement all at once if your threadmill has multiple teeth. It can be chatter city for some set-ups.

Hello Stewart,
Exactly as Marcus points out. If staring from the top, with the lead tooth of the Thread Mill doing the work, say your money and just use a single point, Thread Form cutter.

Regards,

Bill

 

[XanderB]

Any decent tap should last hundreds of holes in mild steel. You DO know what mild steel is....right?

Uh huh, so any decent tap of any size & pitch should be capable of producing 20x holes 1" through in MS. If you say so...Bob.