[_Lou_]

I'm trying to tap hole with a 6-32 tap .700" deep in a 1" hole but my taps keep breaking. The material is an Aluminium casting and I'm using a size 36 drill bit (.01065"). I've tried speeds at 300, 650, and 960 RPM's with the matching feeds. I have plenty of coolant hitting the tap. There is about 1.5" length of the tap coming out of the tool holder. I've even stopped the program to clear what little chips might be in the hole before the tapping cycle begins. Do any of you have any suggestions for me? Should I up the RPM's? Thanks in advanced!

[coherent]

You didn't say how you're tapping which is a major part of the equation, but since you mention different rpms I'm assuming you either have a tapping head or other means of power tapping? 600-1000 rpm may be high, but it depends on exactly how you're tapping and your setup/tooling. You might want to try around 100-200 rpm (or even a little under 100) and see what kind of results you get. Taps can get expensive fast, and i'd personally rather get the task accomplished slower than break taps.
Are you rigid tapping and was it selected. Are you using a tension-compression holder? If so remove it and try a rigid holder. If that doesn't work, try a try a tension only holder (no compression). A good lube makes a big difference with aluminum to avoid gumming up the tap. Many folks say use an uncoated form tap for best results with small taps.

Many tap/drill charts show the correct drill size for 6-32 is a #35 ( 7/64ths - or .1100), some show a number 36. You said .01065 you must have meant .1065. The 36 will be ok for through holes, but the 35 would be a little better for blind holes if you're breaking taps.
Also you don't say what kind of tap you're using. Don't get offended that I mention this, but you can't use a standard tapered hand tap for power tapping, they will definitely break. You should be using a spiral tap or even a gun tap for thru holes. If you are already using a spiral tap, use a #35 drill bit.
Good luck.

[heilcnc]

use a form tap they work better for small taps the tap drill for 6-32 is 1/8

[_Lou_]

Awesome thank you! I'm rigid tapping and using an ER Collet holder. I was looking at the Starett drill chart which recommends a #36 drill for a 6-32 tap but I am going to try a #35. The shop I work at only has 1 cnc machine and a limited number of supplies. Long story short is that I had little experience with CNC machines when the company I work for moved me from manual drill presses to CNC department Then, a couple months later the head CNC guy quit so now they are sending me to school while expecting me to fullfill all the same duties as the last guy but with 5% the experience. So please excuse my lack of knowledge!

Yes I meant .1065 and not .01065 woops. And yes I was using a standard tapered hand tap so I'm sure that one of the main causes of my problems.

Thanks again!

[coherent]

And yes I was using a standard tapered hand tap so I'm sure that one of the main causes of my problems.

Yep.. that was the issue most likely then. A Spiral tap will excavate the chips out the top of the hole eliminating the need for reversing to clear ships from the cutting flutes. a "Gun" tap used for through holes "shoots" them ahead out the bottom of the hole.

[woffler]

There are drill and tap charts for different materials get a drill size for steel and use it on aluminum , that way it will give the extra clearance for the chips and help with tap sticking problem.
Use a number 32 drill.1160 and 100 rpm and use a spiral bottom tap ! i have had this problem with small taps and this always seem to solve the problem and the quality of the tap matters greatly with the little Bugger's.