Hi all,

I've got a Haas VF-1 with Rigid Tapping and I'm trying to tap some 1/4-20 holes. I have no idea what to use as a spindle speed. I guessed and chose 400 rpm, which gives me a feed of 20. I just broke the second one after a few holes. Any suggestions?

Also, I'm just spraying flood coolant during the tapping cycle. Should I manually be squirting rapid tap or something on the tap.

(I'm tapping them .55" deep)

Thanks!

what material are you tapping? What type of tap are you using? is this a thru hole or blind? If it's blind try roll form

It is 6061-T6, it's a spiral flute. It's a thru hole.

Thanks!

You did not mention a lot of important factors to consider, so presuming aluminum 400rpm should not be a problem. I am a chicken when it comes to tapping, at least compared to post I have read, I use 200-250rpm for most everything I tap, but then I am not involved in production considerations, if it is deep I use rigid peck tapping and always take time to use tap-magic and blow out the chips between pecks.

I had a lot of problems using flood coolant and spiral taps, but did use a lot higher RPM then.

Yes it takes me a bit longer now but......No broken taps since. :)

EDIT, as Lakeside mentioned, form taps in aluminum are a real winner.
They take a different clearance hole so watch that.

are you using a spot drill to put a chamfer lead in and are you use a two flute tap. I still like roll form

I'm not putting a chamfer lead in. Just spot drill it, then peck drill the hole.

It's a 3 flute tap.

I'm not worried about the speed, it's faster getting a nice tapped hole instead of breaking them.

I could switch to roll form. I'll need to figure out what clearance holes for em.

Thanks!

Loading,
If you end up trying form taps, here is a little tip, when spot drilling for the clearance drill go a little deep because the form tap will have rolled up a little mound at the hole entrance after tapping from the metal displacement.

here some data on 1/4-20 roll form

Check machinery's handbook for tap drill sizes for form taps. I highly recomend form taps or spiral point two flute tap for thru hole in aluminum. Alot of the other guys on here have great success with tapping around the speeds you said you tried, personally I tap 1/4-20 thru aluminum at 2500rpm and I haven't broke one yet. I've got around 110 holes on one form tap and it still looks as good as the day I bought it. I usually just have the flood coolant on but around every 20 holes or so I will coat the tap with a dry graphite film spray, I don't know that it does much after the first 1 or 2 holes but it can't hurt.

With form taps though just be sure you have the right size or a hair bigger hole drilled for the tap as a hair under will cause problems, I already coated one 5/16-18 tap with aluminum- not pretty. Also with form taps use a 90 deg spot drill and run it down far enough so that the tapped hole will be chamfered when all said and done, as the form tap displaces material, with no chf on top they will quite often roll material up above the top of the hole.

JP

Lakeside, where did you get the neat chart program

JP

Tap drill 13/64", spiral point or spiral flute for through hole, 1000 rpm, 50.0ipm flood coolant. You should be able to do hundreds of holes with a single tap.

JP,
Since Mike is off wandering around other post.....

MEPro

It is the best $100 I ever spent.

http://www.cncci.com/products/cncmepro.htm

I'll need to figure out what clearance holes for em.Thanks!
are you using an endmill to size hole instead of drill This could be your issue?

Thanks Ken

JP

JP,
Since Mike is off wandering around other post.....
MEPro
It is the best $100 I ever spent.
http://www.cncci.com/products/cncmepro.htm
Ken, I have to keep reminding my wife and boss. That it not me wandering around,it's the ADD side of me.
ME PRO for $100 "Good Stuff" That about 5 good endmills

Nope, I am using a drill. Thanks for all the replies. I just ordered a couple more spiral flute (technicut didn't have any 2 flute spiral flute)

I also got 2 form roll and a 5.7 mil drill for em. I also ordered a couple 90 degree spot drills.

Thanks!

(technicut didn't have any 2 flute spiral flute)
I also got 2 form roll and a 5.7 mil drill for em. I also ordered a couple 90 degree spot drills.
Thanks!
If they could not supply a two flute tap,it would be the last time I called them.Also you may want to buy adleast three then if one breaks you still have a back-up here a link to msc for next time. http://www1.mscdirect.com/CGI/N2SRHI?PMSECT=728

That it not me wandering around,it's the ADD side of me.

:D

I'm up in Canada, so I don't have the largest selection of suppliers.

I've been going through technicut, and so far they've been pretty good, except for the no 2 flute 1/4-20 taps. They usually get stuff to me next day.

Thanks again for all the help.

Oh, what speed should I run these form taps at?

Try 1000 rpm? :) (That frightens me--a lot)

personally I tap 1/4-20 thru aluminum at 2500rpm

JP,
At what max depth are you doing this?

Maybe at 1/4 depth I might have the nerve :D

Is there some import of tool issue I see a lot of post with this problem?Shipping can't be all that bad is it?

Ken, thats through 1.00" of 6061 I had to grind the shank of the tap down a little bit just so I could go that deep too! :D
Course I also run a 5/16-18 through .750" of 6061 @1800rpm

JP

No import issue. I just want to get these by monday. If I order from the states that's very very unlikely. Then with importing stuff, it'll randomly get stuck in customs which means your waiting a couple weeks for 20$ worth of tools, then you pay import fees, custom fees, and a more expensive initial shipping cost.

If I could wait, then I'd just order from the states, but I want to get these parts going monday morning.

The other thing to consider is that when buying taps you get what you pay for. I don't buy cheap taps anymore, If I am tapping 316ss I go right to OSG and get a tap specifically designed for that material. The form tap I use in alum is from OSg and is made for alum.

JP

Soak the tap in lye. (Use powdered lye drain cleaner). Lye will attack the aluminum but not the steel. It took a few hours to get the aluminum off a mill I had messed up.

Ken

Check machinery's handbook for tap drill sizes for form taps. I highly recomend form taps or spiral point two flute tap for thru hole in aluminum. Alot of the other guys on here have great success with tapping around the speeds you said you tried, personally I tap 1/4-20 thru aluminum at 2500rpm and I haven't broke one yet. I've got around 110 holes on one form tap and it still looks as good as the day I bought it. I usually just have the flood coolant on but around every 20 holes or so I will coat the tap with a dry graphite film spray, I don't know that it does much after the first 1 or 2 holes but it can't hurt.

With form taps though just be sure you have the right size or a hair bigger hole drilled for the tap as a hair under will cause problems, I already coated one 5/16-18 tap with aluminum- not pretty. Also with form taps use a 90 deg spot drill and run it down far enough so that the tapped hole will be chamfered when all said and done, as the form tap displaces material, with no chf on top they will quite often roll material up above the top of the hole.

JP

Soak the tap in lye. (Use powdered lye drain cleaner). Lye will attack the aluminum but not the steel. It took a few hours to get the aluminum off a mill I had messed up.

Ken

Holy #$%^& that worked. I just tryed that with a tap I hap lolipoped and in like 3 minutes it was completly clean of aluminum.

Thanks for the tip, I knew lye was powerful stuff I just never thought of applying to machining before.

JP

Try a MTX tap... 2632 Rmp and calculated to last for 76585 holes..

Holy #$%^& that worked. I just tryed that with a tap I hap lolipoped and in like 3 minutes it was completly clean of aluminum.

Thanks for the tip, I knew lye was powerful stuff I just never thought of applying to machining before.

JP

Two hints; 1, you will dissolve almost as fast as aluminum so keep it off your skin;2, the bubbles coming of are hydrogen so don't do this near a source of ignition including electric switches.

Doesn't anyone like MollyDee? :(

Just bought MEpro a week ago... Money VERY well spent. :)

I'm tapping 1/4"-20 UNC through holes in 6061-T651 plate. It's a hanson and whitney plug 2 flute G8 tolerance. I've used mist coolant and I have tried 2 of the slowest speeds I have on my mill. One I broke one tap, the other was hard on the tap but didn't break. I liked tapmagic too.. which I tried at my friends' shop.

I'm using a tapholder and tap collet setup in a NMTB 40 holder.

I have to drill 5/16 holes in the plates.. they are tooling plates I hold small parts on.

Greg

Some how I wouldn't think breaking 1/4-20 taps would be much of a problem with 5/16 holes :D
I think you have the wrong drill size there unless that is for something else alltogether.

JP

They are different holes in the plates for an entirely different purpose. They hold 5/16" pins for indexing a hole in a part.

Greg