[weaston]

We are using spiral flute taps for both through and blind holes. Through holes have worked out pretty well so far, blind holes have not.

Recently we used a FEW M8 tap. We tapped close on 200 through holes into Mild Steel. The next job had blind holes. On the first hole the tap broke. We drilled 30mm deep and tapped 25mm deep. It broke when it was at the bottom of the hole.

I know there could be many causes but it is stange that we continually break taps on blind holes....

Any suggestions as to what we are doing wrong, or is this just the expected lif of the tap. The supplier claims that the tap should do approx. 400 holes.

[Crevice Reamer]

Taps are hardened, therefore brittle. A tap will ALWAYS break if it hits the bottom of a blind hole. You must drill deeply enough to prevent this--Bearing in mind that the hole depth needs to be deeper than you think. A certain percentage of the bottom of the tap is a ramp for starting and does not actually thread.

CR.

[davereagan]

You did not mention what material you are cutting or your tap drill size or your lubircant or your tapping speed or your peck increment. Even when I tap 1018 steel, which is easier than most, I have learned to drill .005"-.010" bigger than the chart says for blind holes and spiral flute taps. That reduces the torque significantly. So I would use a J letter drill (.277") for an M8 blind hole 30mm deep. I would use Tap Magic with EP, and tap .400" the first time, .700" the second time and .980" the third time, all at 300 rpm or less. Maybe even four pecks, especially if you drill smaller. I used to try to save 10 seconds on another pass and lose an hour re-running the part. Also, a hi performance tap is great even with mild steel. One that can handle stainless can handle most other materials. Email me at [email protected] if you need a lead on good taps or parameters for another grade of steel.

[juergenwt]

Weastone - You can not use spiral fluted taps for blind holes Unless you have enough clearance at the bottom for the chip to go. You need a tap that pulls the chip up.
Lock at this PDF site from JEL - look for a tap called "Tarex" I will check if there is an English site. But the taps are available in the US. I am sure you can find one from a US supplier.
http://www.jel.de/kataloge/a1_dt_n.pdf

Could not find it in English, but scroll down a few pages to " Gewindebohrer - Sacklöcher" and you will find "Tarex" for different materials listed on the left. It shows you a picture of the tap that will give you an idea what to look for. As you will see - the flutes are designed to bring the chip to the top.
Looks like JEL is part of the "Komet" group. Here is the website -
http://www.kometgroup.com/kometgroup/DE/home.html
You can call Komet to find out where to buy JEL taps.
We found they have the best selection for any type of hole and material.

[dertsap]

Weastone - You can not use spiral fluted taps for blind holes You need a tap that pulls the chip up.
http://www.jel.de/kataloge/a1_dt_n.pdf

a spiral flt does bring the chip up , are you sure your not confused with spiral point


do you have sufficient coolant pressure to remove the chips from the holes after drilling , you may need to add an M0 in order to blow the chips out of the hole with the air hose ,
if you have high pressure thru spindle coolant then put the tap in an er collet ,it will help to clear the holes
davereagan brought up a good point about the drill size , the machinist handbook will show you the max hole dia according to the depth your tapping , push it to the max but be carefull you tolerance according to the class of thread called for on the drawing

[shay z]

on vertical nachines and small blind holes i prefer thread mills.

[weaston]

Hi Guys,

Thanks for all the suggestions. I am a bit pressed for time at the moment so I will have to give some better feed back at a later stage.

In the mean time, however, I found out that our operators have always used the following cycle for tapping.

G84 (Tapping cycle) with a delay/pause comand at the bottom of the hole before the retract P500

I would imagine that this would be ok under normal circumstances, however, we are attempting to tap without using a tapping chuck. ie. I want to do rigid tapping using the M29 code.

Could our taps have been breaking because we have not been using the rigid tapping code?

[shay z]

for rigid tapping you must work with very low feeds.

[dertsap]

on a decent machine g84 should work ok , my preference would be to use g95 (inches/rev) and set the feed to 5 decimal points

[ragman]

for rigid tapping you must work with very low feeds.

Feed is dictated by the thread lead. You cannot feed at anything other than the lead value. Are you thinking rpm?

In my opinion, if you were to use M29 and a slightly larger drill for your blind holes, your problem would go away.

[shay z]

it is obvius that feeds and RPM are rigidly connected when speaking of taps.

when i made 3/4 BSP rigid tapping i had to go down to 40 RPM.

I didn't break the tap but got Z AXIS SERVO ALARM (daewoo H50 horizontal machine BT50 toolholder). I built tap holder that can compensate axial movements and now i am working in 230 RPM.

[KTD1]

We tap blind holes on a regular basis. We use the G94 & M29 (FPR & Rigid Tap Mode) and thread form taps. Form taps don’t create any chips so you can run the tap very close to the bottom of the hole. Formed threads are also stronger than cut threads.

[davereagan]

KTD1,
Can you tell me what materials you form tap in? Also, the largest, coarsest from tap you would run in that material and the lubrication (flood or oil?) Thank you.

[KTD1]

KTD1,
Can you tell me what materials you form tap in? Also, the largest, coarsest from tap you would run in that material and the lubrication (flood or oil?) Thank you.

Most of the time we are machining A-36 or 1040 steel and 6061 or 7075 aluminum. The highest quantity of blind holes with form taps would be ¼-20 holes in 6061 aluminum. We have tapped hundreds of holes using the same tap. As for the largest, I tapped about 50 holes (M12 x 1.75) in 6061 aluminum a month or so ago without any problem. In steel, we’ve had the same results. I haven’t tried the M12 yet. Not that I wouldn’t, just haven’t had a calling for it yet.

All of our CNCs run Castrol Syntillo 9954 coolant. We run it rich at 7%-10% concentration and usually get away with only coolant on taps.

I am by no means an expert on form taps. I started using them only a couple years ago when my hands were killing me after bottom tapping about 250 holes by hand. The more I use them the more I like them. We do a lot of 1 or 2 piece quantities and don’t put a lot of concern into taps until the quantities go up.

There are many different brands and coatings and lubes etc. that might be the best suited for your application. If anyone is production tapping blind holes with cutting type taps, I strongly recommend they consult their suppliers about form taps. I know they have form taps for most all ductile materials.

[juergenwt]

Dertsap - You are absolutely right, I was thinking about spiral point taps. Sorry!

[HuFlungDung]

When tapping blind holes, I take the following precautions:
1. Grind the point off the tap, if it has a male center point. This will allow more good thread to be cut to a greater depth.
2. Run the tapping cycle in air first to see how much overtravel the Z axis takes before reversal occurs. By comparing the coordinate display with the commanded depth, one can see perhaps .05" overrun and allow for this.

I've run hundreds of holes with a #0-80 tap in 303 SS this way, at 1000 rpm. Drilled depth .265" and tapped depth .195" I peck tap this hole because I use ordinary plug taps, as spiral flutes are not available in this size, and they are too weak anyway. I always tap these with a dedicated tapping fluid, not just coolant.

I've used #2-56 spiral flutes ( and larger) and they do tend to chip a tooth far sooner than an ordinary tap. So frequent inspection of the tap with a magnifier is a good plan.