ON topic - more tapping ?

So for years now have been form tapping when I can, using various tapping heads on a VMC. Did lots of cut taps in the selfsame tapping
heads until I discovered form taps, but mostly #6 and up sizes. The other day needed to use some 4-40 cut taps. No problem, done that in the past, but not a lot.
Drilled some test holes in 6061, in goes the first (High quality $$ tap), BAM! Crap What the...? So I get out a hand tap, first 6-7 turns not so bad, increasingly WAY tight after that, (need to go to 13 turns) No Wonder the tap broke!
Specifics: Greenfield GH2 EM-NI, black oxide, spiral flute bottoming tap. hole size .089, no taper measured. O.K. so the tap was designed for Harder Nickel/stainless, but I can see that making a big difference in tap life, not so much for tool pressure. Hmm... In the old days, we had like 4-5 taps. spiral, bottom, hand, coated, uncoated. Now there are 2 dozen choices, mostly for production gains.
So how do you guys do this. Do you create a hole size chart specific to material/tap size/tap style when doing tappng heads, rigid tapping with cut taps? Or did I just pick the wrong type tap? I haven't found, yet a chart showing using a larger hole for bottoming taps.
This doesn't seem to be as critical with the larger taps.
ca
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Ahm certainly no 'spert, but my buddy would proly say plug/taper tap first, then bottom tap.
But since yer using a vmc, and the hole is not that deep anyway, why not just peck, make sure you've got the highest-pressure coolant aimed at the tap (1/16 nozzle), to get rid of chips?
The softness of alum is proly a factor. Also, you can get bum alum now and then, real gummy stuff.
Lots of people drill oversize from the gitgo, just as a hedge. No one admits it, tho. :) :)
--
------
Mr. P.V.'d (formerly Droll Troll), Yonkers, NY
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
clay wrote:

Clay, I didn't look up your specific tap, but given that it's for SST and NI alloys I would think it would be 3 flute. Wonder if there is enough chip clearance?
I use lots of two flute OSG spiral flute bottoming taps with no problems. 295 is the series.
You might want to paw through this OSG site:
http://www.osgtool.com/Technical.asp?tid=1
Best, Steve
--


Regards,
Steve Saling
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I'll second the OSG list 295, solved my problems in 6061. Also Black oxide is the last choice for alum. It likes to stick to the oxide.
Thank You, Randy
Remove 333 from email address to reply.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

What percentage of thread are you trying to get? If you can open up the hole a few thou and still get enough thread (you're going beyond a couple of diameters), you may get better results. I'll bet your tap chart says "75%" on it somewhere, when 65% might be plenty good enough. There's a formula in the handbook for calculating hole size.
Later,
Charlie
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Charlie Gary wrote:

60% was what I saw on a chart after the fact today, so that was a surprise. I think Steve may be onto something with his 3-flute idea, chip clearance I seem to recall using a lot of uncoated 2 fluters in the past. It is only relatively recently that I have been buying the the higher performance coated taps. I have done very little aluminum until recently again. Have lived in the stainless, copper and high nickel world for a long time now.
ca
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

the
for
http://www.besly.com/catl/catl4113H.htm
--


Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Tapping is one of those magical machining issues right up there with reaming, when things go well it is good......when they go bad well...... the issue that I have come across is the high performance drills will drill to size or within .0005 of diameter and if you compare this to a standard drill chart of 'probable hole size' your thread percentage is very high. I wrote myself an excel program that will give me the percentage to actual diameter, this works excellent as I have a project with 316 ss and I am going for 60 to 70 percent thread. Another resource for me was this web site http://www.eisc.com/support/threadholesize.htm which goes into more detail.
Dave
Life is good, work sucks.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
DL wrote:

this makes sense, as there was a thread, long ago about using lower thread % now, as the drill charts were developed when drills were not as accurate, and commonly drilled oversize.
thanks for the link.
ca
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
4-40? 6061?
.1015 hole, roll tap, hands down, done 1000's of those
"D"
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Clay,
I've rigid tapped lots of 4-40's in aluminum, mostly bottom tapped, I think part of the problem is the tap you are using, for aluminum, I use the bright uncoated ones or TiN coated onse and seem to have few problems. I am a bit surprised that you would have a problem with this, perhaps the tap is really not setup for aluminum, but heck, if it's set up to cut through stainless, I would think that 6061 would be no problem.
I have cheated from time to time and used 3/32 instead of .089, since if you are engaging more than about 4-5 threads it will make no strength difference. Usually what kills a tap when I am rigid tapping is if a chip gets in the way and is "sucked in" because it was sitting on top of the hole when the tap went in.
I assume you were using some sort of cutting fluid when you did the hand tapping, and were guided.
I can look up some of the taps I normally use.
John

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
clay wrote:

If you haven't tried spiral flute taps before, you really ought to. I even use them on through holes, because the chips are stringy, like drill chips, and clear off the tap easily, not like the typical spiral-point taps that leave a lot of chips in the hole. The deal is most of the chip comes up the flutes, rather than causing binding in the hole.
Jon
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.