Tapping 2-56 holes (Haas mill)

[Chris Parish]

Hello:

 

we seem to have run into a situation lately for tapping 2-56 holes with a form tap.. I am using a 2mm drill making hole size .079 dia... sometimes the holes size in aluminum after tapping is ranging from .074 to .08 minor diameter.. Therefore the nogo thread gage threads in... Does anyone have some advice for me ?  please advise

 

Thanks,

Chris Parish

[crazy^millman]

Ream the holes and use a floating tapping holder. Drilling that small is not accurate enough to roll tap, you must ream the holes has been my experience. 

[Chris Parish]

56 minutes ago, Chris Parish said:

Hello:

 

we seem to have run into a situation lately for tapping 2-56 holes with a form tap.. I am using a 2mm drill making hole size .079 dia... sometimes the holes size in aluminum after tapping is ranging from .074 to .08 minor diameter.. Therefore the nogo thread gage threads in... Does anyone have some advice for me ?  please advise

 

Thanks,

Chris Parish

Thanks Ron.. I'll purchase a reamer and give it a try...

[crazy^millman]

Well 2 things happen when you ream the hole. You get a much nicer surface finish which helps with roll tapping as well as holding the hole size. People forget it is a cold forming process that is forming the thread and drilling tends rip the material where as reaming tends to cut the material. The voids that drilling creates does not create the uniform surface needed for making good threads roll forming does. 

[BCW]

What is your R value on G84 line? In my experience Haas like to start .2 above the part to get synced properly.

What is the angle on your drill point? Make sure your spot drill has a larger included angle.

 

[balnh]

A quick fix would be replace drill. I've had this happen many times. The drill is drilling slightly oversize on you. Causeing the minor to not form up to correct diameter. Reaming like Ron said is bullet proof but pin hole size when you are done drilling. Hell, I barely even order metric drills. I'd go at it with 5/64 drill if that was all I had. It's only aluminum. 

[jeff]

8 minutes ago, balnh said:

 It's only aluminum. 

It's only aluminum, but it's still a pretty small tap 

[BCW]

5 minutes ago, balnh said:

A quick fix would be replace drill. I've had this happen many times. The drill is drilling slightly oversize on you. Causeing the minor to not form up to correct diameter. Reaming like Ron said is bullet proof but pin hole size when you are done drilling. Hell, I barely even order metric drills. I'd go at it with 5/64 drill if that was all I had. It's only aluminum. 

Why is the drill going oversize? Its either running out in a bad drill chuck or its kicking off when entering the spot... why I mentioned spot angle above.

[crazy^millman]

Guess I am too old school and would rather know what I know by knowing what I know by spending the extra time to ream the hole and know I got a hole sized exactly what it should be to make the best part possible. Why risk a chip or anything creating a possible problem when reaming the hole is about as bullet proof as I know to get.

[civiceg]

Under 1/8 diameter Titex drills, easy +/- .001 on Aluminum. When you are doing hundreds of thousands of 2-56 and 0-80, way too much time lost reaming. 

Job I did with a .026 titex drill, +/- .0005. Every hole was checked. Few thousand or so holes now. 

Decent keyless chucks or collets. And checking runout is key. 

[crazy^millman]

9 minutes ago, civicegg said:

Under 1/8 diameter Titex drills, easy +/- .001 on Aluminum. When you are doing hundreds of thousands of 2-56 and 0-80, way too much time lost reaming. 

Job I did with a .026 titex drill, +/- .0005. Every hole was checked. Few thousand or so holes now. 

Decent keyless chucks or collets. And checking runout is key. 

Okay on this I concede the point.

[balnh]

2 hours ago, BCW said:

Why is the drill going oversize? Its either running out in a bad drill chuck or its kicking off when entering the spot... why I mentioned spot angle above.

This is true. My point is it doesn't take much of an oversize hole to have bad threads with a 2-56 roll tap. Always check the drilledhole so you know what you r diameter is. I have had drills drill .001 oversize that come out of the same pack. 

[jlw™]

I'm there with Ron.  Hole size has to be money for form taps.  Especially small ones.  If you buy the right drill and reamer you can do it faster than drilling alone with the wrong drill.

 

On drill only applications I've had great luck with YG1 dream drills in alu.  No spot required, size perfect, and you slam a 1/8in drill in at 25ipm.  The human eye can't tell the difference between cutting and rapid.

[Newbeeee™]

+1 to YG dream drills. They are carbide and hold size really really really well. And straight in.

But they are restricted on size availability - 0.1mm dia increments.

For this job (ally small hole) we'd be using OSG SUS GDS drills - available in 0.01mm dia sizes and cheap, split point so no centring - straight in.

Out of interest, what's the consensus for R value when tapping? We always start 5mm (0.2) above the hole to allow spindle sync (same as latheing - screwcut starting 5 mm infront of the part)

 

[jlw™]

I don't know what machines you're running but everything I've ever ran stops to sync on the first hole of the G84 call.  It doesn't matter if you start at .2 or 12. or Z0.

For any thread tho, I always start 1xpitch above the hole.  Tapped or threadmilled.  Just a habit I've had for years.

[Guest]

While I agree that hole size, especially on smaller holes is very important, I can't say I have ever had to revert to reaming a 2-56, or any size for that matter.

In the situation Chris has described, I would look very hard at the coolant.....something is causing the roll tap to gall and leave extra stock....I would check to make sure the concentration is correct and that sufficient coolant is making it onto the tap.....

Also, is this issue with 6061 or 2024? The 2024 can be very gummy and trouble to roll tap.....

 

As far as how far to start above the hole, the only time I have had to start higher than my standard .100" is on a lower end machines(Fadal)

 

Edited April 8, 2017 by Guest

[jlw™]

I can't believe it's not getting Keenserts in alu.  If threads are being rolled for strength maybe the application needs inserts instead.

[AMCNitro]

How about trying a smaller H number?

[civiceg]

Haas requires .2 above the hole to give the spindle and z axis time to sync. Also, if you are tapping the same hole more than once, then the "repeat rigid tapping" setting must be on. 

 

Everything FANUC, my default is .05 above the hole. 

[Newbeeee™]

8 hours ago, JParis said:

Also, is this issue with 6061 or 2024? The 2024 can be very gummy and trouble to roll tap.....

 

6000 series ally has high elongation in comparison to 2000 series which is high copper content - it work hardens, higher tensile and a lot less elongation. I've never tried to roll it.

Ref machines - VMC's here are all fanuc and lathes are Siemens. We've never had an issue with the R value, but have always used the 5mm (0.2) value.

It may have been from reading here or practical machinist - I can't remember - we've never tried less which will probably work by the sounds of it, but never had a problem so never done anything different.

[mkd]

+1 to hole size and coolant concentration. I've done 1000s of 0-80s to 4-40s in 6061. Cheap screw machine length drills @10,000rpm gets it done, but you do have check hole size is within +/-.001 consistency. I just buy packages of 12 drills of the sizes near the recommended.

 whenever the roll tap breaks on the way out of a blind hole it is without a doubt coolant concentration.

2 cents

[Charlie Pierson]

The proper hole size and accuracy is not so much a function of the Major dia. of the roll tap , but the pitch (in this case read height) of the thread.

5/16-56 hole size is just as critical as #2-56.