Thread percentage vs broken taps. 5

[todd920]

Hello to you. I would like to "pick" your brains about thread percentages. Just to give you some background, I have been employed as a machinist for the last seven years. A problem persists in industry with broken taps. I believe from my experiences that a bigger tap drill would do the trick. But how big of a drill can we go to without losing percentage? I was once told that 51% thread engagement is all we need. Seems like a small percentage to me? Now one will ask what the material being tapped is. I guess lets just say good old hot rolled steel. We "started" the threads at my last shop and finished them by hand. That was done with hss drills and coolant for tapping. The shop I work at now uses carbide drills. I know they drill to the smaller side. So I usually go bigger by a few thousandths on my tap drill. And here we use oil on our taps and tap to depth. Broken taps are a plague when using coolant. It may be a coolant issue? but really? I guess I would like to know what is an exceptable thread percentage based on an engineering stand point. gimme some ideas please. My theory is no oil on taps and tap to depth with no broken taps, There are other variables too. like depth of hole. refractometer reading of coolant, manufacturer of tap etc. Thank you very much. I figured why not go to the source. That source is you guys. If anybody would know it would be you. Thanks again

 

[hydtools]

60-75% thread. Blind tapping? Chips are packing.

How many threads, or thread length? 1-1/2 to 2 diameters for steel. From engineering viewpoint.

What type tap?

Ted

 

[todd920]

Smaller taps up to half inch. I usually drill to china on my tap drills. Deep. Trying out peck tapping in my G84 line. Fanuc controls. No sychronized tapping. Familiar? Been going bigger on drills- so,so. My goal is no broken taps and full depth. No thread milling

 

[BrianE22]

Have you tried thread forming taps? I've yet to break one.

 

[mrainey]

I worked for several years for a major manufacturer of large electric motors. Their manufacturing documents specified a 55% thread for cast iron and low-carbon steel. I don't recall hearing of any thread failures.

Software For Metalworking

http://closetolerancesoftware.com

 

[todd920]

Yes to threadforming. Inspection frowns upon that though. Thanks for the help

 

[arlieb]

Ok, There are a few things that need to be ironed out first.
1- are you checking the concentricity of the tap in the tool holder or are you just mounting it and tapping?
2-Where are you getting the speeds and feeds for your taps at?

1a- your concentricity should be less than .001
2a- you need a book or chart from the tap mfg. that will give you a good starting point in the material your working with.

I would guess that your concentricity is bad and your tapping too slow.

This is from my own personal experience. I have been a machinist / programmer / lead man for 17 yrs in the Milling dept. at my shop. I have seen this a 1000 times, everytime we hire a new guy I go thru this with them and their reply at a later date will be I had no idea you could tap like this.

My .02
Arlie

 

[TVP]

For best results, ie no breakage, tapping should be done with a good cutting oil/tapping fluid, not water-based coolants. You need the lubricity of the oil to reduce friction and torque. The percentage of thread is usually specified as ~ 60% minimum, but may be as low as 55% in some materials as noted by mrainey. Also, are you using the appropriate tap type, meaning a spiral flute tap for blind holes in materials that form long chips?

 

[btrueblood]

I love spiral flute taps. We've yet to break one to my knowledge, used to snap off a straight flute tap every month or so, and this was just for chasing threads in cast iron and mild steel.

 

[mfgenggear]

Normally the tap drill is specified on the Engineering drawing. ie minor dia specified.
I agree with the above replies

Must make sure the tool is indicated in.
the right lubrication
the correct geometry style of tap
starting & finishing tap.
the correct feed & speeds.

Mfgenggear

 

[BillPSU]

Broken taps have a myriad of causes one of which is tap drill size. All of the following items could impact how a tap performs.

Material, hardness, blind hole or through hole, length of thread, tap drill size, cutting fluid or coolant,application equipment, tool alignment, speed, work hardening, temperature, chamfer length, cutting edge design, flute design, web thickness, tap type (cutting/thread forming).

There is no easy button to almost any machining process. Lets talk material for example. Mild steel 15-25 carbon, gray iron, and ductile iron, thread forming only works on ductile material. Gray iron cannot be tapped properly with thread forming tap. Chip control in steel is very important while gray iron not so much. What strength ductile iron has an impact. Now consider 4140 annealed, or normalized or heat treated. Even in the annealled condition the 4140 will be tougher to tap. Then consider "soft" materials which present spell challenges. Aluminum can be very gummy depending on the aluminum grade and condition. Try tapping copper or a composite such as fiberglass reinforced resin or silicon carbide reinforced aluminum. There is no simple answer.

 

[saberblue]

A large percentage of the energy necessary to "drive" a tip comes from the flank of the tap rubbing on the freshly cut threads thus the deeper you go the bigger the problem. Thus applying coolant or oil can make a big difference. when selecting the fluid you are looking for a fluid that has the maximum hydro dynamic lubrication possible thus high viscosity oil is better than low which tends to be better than soluble oils etc. etc. -- Soluble oils with high oil content and or large particle size works better than low oil semis or synthetics.

A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com