4-40 Thread Forming Tap Breakage

[secretpickle]

I was using an OSG thread forming tap, at 1000 RPM. #4-40 size. After about 90 holes the tap broke. The hole was drill with .0995 drill, and the the drill appears to still be sharp. The hole is a through hole. The tap was held in one of those special tap holders that compensate for spindle/feed synchronization (or lack of). Water based coolant was used, but not sure of the brand. Oh yea, and the material was extruded 6061 aluminum.

My question is what the possible cause of breakage is? It seems like the tap got stuck in the hole, and the fracture pattern looks like it was twisting when it yielded. This is my first time using a forming tool so I'm not sure what the life expectancy should be.

Thanks in advanced, sorry if this is maybe in the wrong forum. Kind of new to posting in this forum.

[Caprirs]

How deep are you tapping? What H limit is the tap? Have you checked the hole size with a gauge pin after drilling and before tapping? You should be able to run that tap through ten thousand holes.

I've done a lot of 4-40 holes in parts that were to be anodized using an H5 tap so the threads would not close up too much after anodizing. The .0995 drill was too small so I used a .1015 drill. Still got good thread when checked with a go/no-go gauge.

[secretpickle]

I think it's an H3 and I did not check w/a gage pin. I should probably open the hole up a bit.

http://www.osgtool.com/product_detail.asp?id=1400105300

That's the form tool. I'm only tapping about 1/2". What RPM do you usually use that tap, and do you use some type of oil based lubricant?

Matt

[Caprirs]

Definitely verify the hole diameter after drilling.

In 6061, I use flood coolant (full synthetic) at about 8%. On my machine, I hold the tap in a DA collet, no extension/compression and program 1000rpm.

You can try verifying that the spindle is properly in synch also. It's unusual but sometimes the machine is off due to something like belt slippage. To check, run a tap in air. For example, G84 Z-.500 R0. E40 S100. Then count the revs until the spindle reverses. Obviously, you should get exactly 20 revolutions.

Do you have a large backlash compensation for the Z axis that might move the Z at the bottom of the hole?

[secretpickle]

The spindle is not synchronized w/the z-axis. After the Z-axis stops, the spindle does a few revs before reversing, which extends the tap down the hole.

Matt

[Caprirs]

Ah, that would be a difference between your machine and mine. Mine is rigid tapping, yours is synchronous tapping. I'm not familiar with those types so I don't know what the tricks are. But from your description, it sounds like the spindle's extra few revolutions may be using up all the extension in the tap holder?

[secretpickle]

Maybe, but it did consistently machine about 90 holes w/out a problem. Will slowing down the RPM cause there to be more wear on the tap or should I be okay?

Matt

[Astonlee]

Caprirs is right about the tapping drill, has you will need to experiment with the size of dill you are using, unlike convention taps, all fluteless tap manufacturers only suggest the tapping drill size you start with.