[behindpropeller]

CNC/HAAS newbie here....


I keep breaking taps. I'm trying to tap some 10-32 holes in aluminum. The holes are drilled .159 and I have countersunk them a bit for a good lead in. I was using a spiral flute tap to tap some holes in 1/2" thk aluminum. I talked to HAAS this afternoon but was not at the machine to verify that rigid tapping is actually turned on (I'm 99% sure it was turned on when we bought the machine with the option). I was trying to run them at 500RPM with a feed of 15.625.

Ok...now reading this I see 15.63 in the code...is that my problem?

Here is the code...with the tool previous to it. This is programmed in HSMworks.

Thanks for your help.

Tim

N2010 T3 M06
N2015 T11
N2020 S2500 M03
N2025 M08
N2030 X7.435 Y-7.75
N2035 G43 Z0.8 H03
N2040 G04 P5.0
N2045 Z0.4
N2050 G81 Z-0.5978 R0.2 F20.
N2055 X7.935 Y-6.75
N2060 X7.435 Y-5.75
N2065 X7.935 Y-4.25
N2070 X7.435 Y-2.75
N2075 X7.935 Y-1.75
N2080 X7.435 Y-0.75
N2085 X2.565
N2090 X2.065 Y-1.75
N2095 X2.565 Y-2.75
N2100 X2.065 Y-4.25
N2105 X2.565 Y-5.75
N2110 X2.065 Y-6.75
N2115 X2.565 Y-7.75
N2120 G80
N2125 Z0.8
N2130 G28 G91 Z0.
N2135 G90
N2140 M09
N2145 M01
N2150 T11 M06
N2155 T5
N2160 S500 M03
N2165 M08
N2170 X7.435 Y-7.75
N2175 G43 Z0.8 H11
N2180 G04 P5.0
N2185 Z0.4
N2190 G84 Z-0.55 R0.2 F15.63
N2195 X7.935 Y-6.75
N2200 X7.435 Y-5.75
N2205 X7.935 Y-4.25
N2210 X7.435 Y-2.75
N2215 X7.935 Y-1.75
N2220 X7.435 Y-0.75
N2225 X2.565
N2230 X2.065 Y-1.75
N2235 X2.565 Y-2.75
N2240 X2.065 Y-4.25
N2245 X2.565 Y-5.75
N2250 X2.065 Y-6.75
N2255 X2.565 Y-7.75
N2260 G80
N2265 Z0.8
N2270 G28 G91 Z0.

[Donkey Hotey]

I keep breaking taps. I'm trying to tap some 10-32 holes in aluminum. The holes are drilled .159

Blind holes or through holes? Spiral point should be a through hole so it can push the chips. Spiral flute may be correct for blind holes but I suspect that it's very fragile at that size.

I've had much better luck with forming taps. They work really well in those smaller sizes--especially if you're going to the trouble of making a lead-in chamfer.

If not that, then go up a size or two on the drill. An extra 0.003-0.005" ain't gonna' kill your threads but they'll tap much easier.

Also: are you absolutely sure that your predrill is deep enough? I had one where I thought I was going nuts, but the drill had pushed into the chuck on the first hole, causing them all to go shallow. I broke three taps before I figured out what happened.

[Geof]

I think your drill size is a bit tight especially going 0.55" deep in one go.

I am going to wander out and check what size drill my little chart suggests.

.159" it is, I guess I am the sloppy one because I habitually use #19 which is several thou larger. Try pecking.

[mrainey]

Definitely drill deeper if possible.

[Dualkit]

Class 2 or 3 threads have a max minor up to .164 go up on drill size. Are you using 2 flute taps? They tap easier than 4 flutes. Also Chinese Aluminum is gummy, hope you are using USA made.

[Delw]

I've had much better luck with forming taps. They work really well in those smaller sizes--especially if you're going to the trouble of making a lead-in chamfer.

Funny you should mention roll taps, I have a 200 hole job with both thru and blind holes , been using 10-32 cut taps for the last 1 years on this particular job occasionally break a few, last week I started using roll taps on 10-32's and WOW I love those things on alum. No chips very very small burrs and the thread comes out perfect every time, not to mention the finish is like glass.

has anyone used 1/4-20 roll taps on alum?

Delw

[behindpropeller]

1. Holes are drilled through. I took the bit out of the chuck and it slipped through the stock.

2. Material is USA made.

3. I will switch to a spiral point and up the drill size a bit today.

4. I will try some roll taps in the future for 10-32.

Tim

[extanker59]

Tim- What was the result when you changed the feed from 15.63 to 15.625?

Delw- in the 90's, when I was doing aluminum production parts, we switched to roll taps (including 1/4-20) and our tap usage dropped to almost zero. Very rare to break a roll tap in aluminum. I remember someone accidentally tapped into a 1/4" thick plate that was missing the pilot hole. Messed up the plate and the tap but the tap didn't break. Just galled up.

[woda]

What kind of toolholder do U use? Is it going with any floating?
A holder with microfloating would be to prefer..

excuse my bad english..

[behindpropeller]

Found out the problem....

Rigid tapping was never turned on. We bought it with the machine!!!

I'm pissed....I wasted a day messing with it.

Tim

[Donkey Hotey]

Yup, that'll do it every time.

[Geof]

Found out the problem....

Rigid tapping was never turned on. We bought it with the machine!!!

I'm pissed....I wasted a day messing with it.

Tim

Before you try peck tapping check that Repeat Rigid Tapping is turned on also.

[Mr.Xtreme]

Sorry for the small thread jack, but how do you peck tap?

[Geof]

Just have sequential G84 commands each with a slightly deeper Z.

It is not exactly pecking because that suggests you have a Q value in the G84 line; Haas does not support this.

[Mr.Xtreme]

Thanks Geof,

I was hoping for a canned cycle with like a "Q" or something.


Paul

[Mic6]

has anyone used 1/4-20 roll taps on alum?

Delw

All the time. Run in at 1000rpm and out at 2000. Within .02 of the hole bottom. I bet alot of people run faster, but I'm comfortable at 1000 rpm :cheers:

[gabby]

Just a thought is the turret in line with the spindle if you have had a knock this can be over looked. In the past I have made a bush by machining the bush on the machine. turn up a blank put this in the turret then drill and ream to size using the chuck to hold the drill. A bit long winded but garantees tap alignment