Poor Tool Life Tapping 0-80 Thread in 360 1/2 Hard Brass

[Nerdlinger]

I'm a bit late to the party, but I would personally use...

- correct size tap drill

- uncoated tap

- lubricating oil (not "cutting" oil)


A forming tap works much better with a bit of high-pressure lubricant (e.g. old-school 90-weight differential oil or something like STP). It's a forming process, not a cutting process.

Yeah, I like to use the correct size tap drill sometimes haha!

I never thought about using different lubricants for form tapping vs cut tapping! I just don't know how I would do that, short of swapping out the entire machine's coolant reservoir.

Why no coating on the tap? Is coating detrimental when forming brass??

Thanks!

 

[Ox]

.052 after forming is not the same as .052 before cutting per strength, b/c it is .058 (?) in the valleys between, and the .052 crest is unsupported.


-----------------

Think Snow Eh!
Ox

 

[Nerdlinger]

.052 after forming is not the same as .052 before cutting per strength, b/c it is .058 (?) in the valleys between, and the .052 crest is unsupported.


-----------------

Think Snow Eh!
Ox

Yeah, I guess you're right!! I wonder if there are different specs for minor diameters that are formed and minor diameters that are cut for that reason. Like you said - a formed .052 will probably be weaker than a cut .052

Regarding THESE parts specifically, there actually is a torque spec we check the part against...we put a screw in and it has to support a minimum amount of torque without stripping. The formed parts DID pass the test, but I know what you're saying!

 

[eaglemike]

Yeah, I guess you're right!! I wonder if there are different specs for minor diameters that are formed and minor diameters that are cut for that reason. Like you said - a formed .052 will probably be weaker than a cut .052

Regarding THESE parts specifically, there actually is a torque spec we check the part against...we put a screw in and it has to support a minimum amount of torque without stripping. The formed parts DID pass the test, but I know what you're saying!

You could test to see which is stronger - some threads are stronger after form tapping, due to grain structure. So I was told long ago. I do a LOT of form tapping, and I've never had a thread failure issue. For my own products, I don't even worry about getting more than 60 percent thread, and it has always been plenty.
I used to run screw machines long ago, and always used oil when tapping brass. I know you've solved it now (hooray!), but forming always needs more lube than cutting.
Good luck!

 

[guest]

We have a .052" no-go pin gage, so I guess that makes sense! Maybe I'll check with a variety of pins to see where we are at in the .0465-.0514 range and see if I need to get a slightly-different (metric) drill for next time. Thanks!

There's not a lot of wiggle room in the available drill sizes.

If you need to tweak the minor you can bump up the H value on your tap. This will increase the pitch diameter a little, and squeeze down the minor.

 

[Delw]

Yeah, I guess you're right!! I wonder if there are different specs for minor diameters that are formed and minor diameters that are cut for that reason. Like you said - a formed .052 will probably be weaker than a cut .052

Regarding THESE parts specifically, there actually is a torque spec we check the part against...we put a screw in and it has to support a minimum amount of torque without stripping. The formed parts DID pass the test, but I know what you're saying!

There is ABSOLUTELY NO difference in thread spec for threads from forming or cutting.
a thread spec is a thread spec many ways to get there. if your print calls for a 2b thread that was the minors I gave. (2b is the common for most applications that dont have specs called out)

the reason you drill a tad bigger on the minor when using a form tap is because the tap forms the thread which pushes the material into the minor.
a cut tap will usually cut leaving the minor the same hence why you drill the minor to the size you called out. smaller threads you make get some burrs in there that will make the minor smaller than drilled after tap.

That all being Said The guy making the part is responsible for making sure your minor is correct to spec. ALWAYS check the MINOR after parts are ran. more scrap is made by people Assuming becuase they used the right drill size your thread is good Thats far from true.

Also when playing with small threads under .125 dia a .001 or .002 can make a huge difference in the thread and the minor as its finished especially on form taps. 0 00 and 000 are very prone to drill size being exact and it doesnt take very much to break a tap or make a bad thread.

Thread specs are super easy to look up theres tons of apps also for your phone and online.
the % rule that people talk about is Garbage. in 30+ years of machining I have never seen a print with a 75% 80% etc thread call out or what ever. Save that for guys in the garages and hacks that dont know any better.

most thread will be called out by 1a 1b 2a 2b 3a 3b There is a spec for them.
"A" is o.d. threads
"B" is id threads
"1" is sloppy as shit like throwing a hot dog down a hallway.
"2" is commonly used
"3" is tight

 

[Nerdlinger]

There's not a lot of wiggle room in the available drill sizes.

If you need to tweak the minor you can bump up the H value on your tap. This will increase the pitch diameter a little, and squeeze down the minor.

"What's obvious to you is obvious to....YOU!" I didn't think of that! I believe I am good since it passes the the functional test and the .052" no go but that is a good idea! Thank you!

 

[Nerdlinger]

Also when playing with small threads under .125 dia a .001 or .002 can make a huge difference in the thread and the minor as its finished especially on form taps.

For sure! My pic a few posts back shows the effect a .003" difference in drill diameter made!

sloppy as shit like throwing a hot dog down a hallway.

Where the hell do you get this stuff!?!?

 

[eaglemike]

Where the hell do you get this stuff!?!?

The comparison to throwing a hot dog down a hallway has been around a loooong time. It's often used in another context, that one would not often used in mixed company.


I form tap a lot of the holes in my parts because I'm lazy. Getting chips out of blind holes can be a royal PITA. Even with a spiral flute tap, doesn't always work. Maybe now, since I have Brother machines I could use a chip breaking cycle and not lose enough time to matter, but no need. I always form tap when I can. I've reamed holes at times prior to tapping to end up with the proper minor diameter.
About forever ago, when I was young, I went to a Greenfield sponsored seminar on tapping. I remember that the biggest part of getting it right, after choosing the right tap and lube for the material, was preparing the hole properly, whether form or cut tapping. Round, smooth, right size. (sometimes I had to relearn the hard way if I took something for granted.)
I enjoy reading about other's experiences here, and learning from them. Stay safe!

 

[Nerdlinger]

Just for the record we finished the job with over 1,500 holes on the tap and you could not see any wear on it even under a microscope! I do not know how much the oil was helping. I’m sure it wasn’t hurting, but we may still try it dry next time just to see if there is any noticeable difference in tool life. Thanks, again, for all your help! I am pretty embarrassed that this one largely boils down to a simple case of using the wrong tap drill!

 

[Delw]

Just for the record we finished the job with over 1,500 holes on the tap and you could not see any wear on it even under a microscope! I do not know how much the oil was helping. I’m sure it wasn’t hurting, but we may still try it dry next time just to see if there is any noticeable difference in tool life. Thanks, again, for all your help! I am pretty embarrassed that this one largely boils down to a simple case of using the wrong tap drill!

oil makes a huge differnce in cutting oil. I ran 2 omni turns running nothing but electrical components in brass and copper alloys very rarely changed insets

 

[eaglemike]

Just for the record we finished the job with over 1,500 holes on the tap and you could not see any wear on it even under a microscope! I do not know how much the oil was helping. I’m sure it wasn’t hurting, but we may still try it dry next time just to see if there is any noticeable difference in tool life. Thanks, again, for all your help! I am pretty embarrassed that this one largely boils down to a simple case of using the wrong tap drill!

I ran a LOT of free machining brass in B&S screw machines long ago. I really don't think tapping dry is a good idea. I would not even try it. Especially form tapping.
I wish you luck!