Small metric tap feed question

[John13]

Good morning, could somebody tell me a good starting point for feed for a 1.4 x 0.3mm metric tap. I have it converted to inch, however I am getting 4158 spindle speed and a feed rate of 352044.7 when I click Calc. Speed/Feed

 

Now if I have the Metric values box selected, I get a 6000 Spindle Speed and a Feed rate of 2.79. Is this more reasonable??

 

Material is aluminum, what would be a good starting point, I do not want to break any taps, at least not to many, trying to figure this out. Thank you for your help.

[Bryan Johnson]

I find 20 IPM good for most all tapping.

When using a metric tap in an inch program, be careful with the toll definition that you set the TPI correctly.

[chris m]

.3MM pitch comes up to .0118, so 6000 RPM would give you 70.86 IPM. 6 grand is a lot unless you have a tapmatic or similar device and is probably a lot for that, too. Thru or blind? Cut threads or formed threads?

 

First effort I'd try 1386 rpm at .0118ipr

[John13]

Blind holes, form tap, .130 deep

[chris m]

With a form tap you can run the speed up higher, but you'll start to run into synchronization problems if you rigid tap with too much RPM. If you run a tension-only tap holder and underfeed by 2% or so you can probably go a little faster than rigid but you'll have to make sure you have a little clearance under the tap because the tap will most likely overshoot the depth a bit that way.

 

If the machine will tap at 2079RPM I'd give that a go [same IPR, obviously] and start .200 above the hole to give the synchronization a little room to get locked up

[John13]

Thank you, I'll start at 2079 RPM, giving me feed rate of 24.458. Thanks for the help. .2 above part.

 

rigid tapping using a tap collet, and I drilled .175 deep and am only tapping .130. hopefully hitting bottom will not be an issue.

[Flycut]

It might not make any difference but I like to find whole numbers to tap with.

 

In this case 30 ipm and 2540 rpm.

 

I find it looks better in code and there is no rounding out of the last decimal.

I find it's easier to start with a feed and match the rpm to suit.

 

HTH

[chris m]

2079*.0118=24.53IPM; with a small tap like that you might want to go for the G95 if the machine will do it.

 

C

[chowquoe^]

I use the G95 as chris has mention as my perfered method, ****Note**** do not forget to change back to G94..... I did once , can you say PUNCH PRESS, spot drill running 1200rpm and 6ipr was kinda fun to watch.

[Jerosu]

http://www.balax.com/catalog.pdf

 

Great reference material- pg.67 has recommended starting speeds.

[35K chipper]

I use a lot of small metric roll taps in alum. rigid tapping with taps .9mm to 1.4mm in inch mode. on a 1.4mm x .3 i use 1500 rpm at .01181102 pitch. my control will take 8 dec. places. with small taps .0001 ether way is alot. at your depth of .130 deep or 11 revolutions or .0011 . use more places if your control will handle it. i start at .05 above the hole. i use a 1.25mm carbide circuit board drill for the hole. hope this helps

35k

[Bruce Caulley]

Another reason for the US to go metric!! There are no metric to imperial problems such as this

 

Bruce

[35K chipper]

many times you don't design the part you just make it!!!!!!!!

[CNC-ERIC]

To 35K CHIPPER,

 

Could you please tell what kind tap holder you use?

Did you ever use Lyndex Positive Drive for such small tap? how deep for 1.4mm tap?

do you use lub. oil while tapping?

 

thanks

 

Eric

[CNC-ERIC]

Hi, guys,

 

1/8-27 NPT, through hole, aluminum 6061 T6, HAAS VF-2(20 HP) Rigid Tap, spiral flute tap, what is the suggested RPM?, do I need tap ream the hole?

 

thanks

 

Eric

[chris m]

I would not ream a 1/8-27; just drill and tap it. I'd start around 10SFM and would consider peck tapping that hole [maybe 2 pecks] if the machine doesn't have a gearbox. 20hp sounds nice but the belt-drive machines have about 2 lb-ft of torque at low RPM which can cause troubles with tapered threads.

[PeterM]

When solid tapping on a Haas the exact feed is required Fx.xxx I have found that 127 is a sort of magic number for metric taps. take any metric pitch yours for example .3mm = .11811024 * 127 = 1.5 find a multiple of 127 in the expected range that you wanted to run the tap at and voila'. If we use Chris's 2079, the nearest multiple of 127 is 2032,

that gives me a feed of F24.

[Tinny]

If you define a tap in inches then the pitch is threads per inch.

 

If you define in metric then it is a pitch distance.

[PeterM]

My example is for rpm in inches for a metric tap. Our shop practice is inch not metric and I am unwilling to program in both flavors, too much room for disaster.

[Guest CNC Apps Guy 1]

I thin 5,000 is the max RPM you can tap at in any machine.

 

When I tap I ALWAYS tap in IPR, that way I can tweek the speed to suit the material/conditions without having to give a thought to the feed.

 

With a blind hole, I'd roll tap that sucker though.

[35K chipper]

eric

i use an er tap collet rigid all the way. no oil just coolant. i do M0 to blow chips from the drill holes. i'm tapping 0.200 deep. 50 holes

35k

[35K chipper]

eric

1/8 27 npt thread mill it...

35k