Rigid Tapping #8-32

I just bought the Tormach Modular Tension/Compression Tapping Head Kit:
https://www.tormach.com/store/index....07&portrelay=1

I am working on a new product that requires a high quantity of #8-32 threads tapped into 1/4" thick aluminum. This is my first time rigid tapping in a mill but I gave it a shot. I pre-drilled with a #29 (0.136") with a 0.030" chamfer to help guide the tap. I ran the tap at 1000 rpm and the feed is automatically calculated in Fusion 360 using the "Tapping" cycle type. I did not add a dwell in Fusion 360. As you can see in the picture below (see album link) hole #3 & 4 from the left have issues with the top two threads. It looks like the might be getting ripped out on the retraction. The operation is practically silent and I can't see anything wrong in the operation until I inspect the threads.

https://photos.app.goo.gl/EslwpvZ6YhZYGf962

I tried speeding up the RPM to 2000 but I broke the tap on the first hole... Does anyone have some suggestions on what is going on here?

Thanks!

Here is the g-code:

%
(8-32 Test Cuts 4-6)
(T11 D=0.136 CR=0. TAPER=118deg - ZMIN=-0.5 - drill)
(T20 D=0.375 CR=0. TAPER=45deg - ZMIN=-0.04 - chamfer mill)
(T45 D=0.167 CR=0. - ZMIN=-0.425 - right hand tap)
G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G20 (Inch)
G30


N10(29 Drill)
T11 G43 H11 M6
S5100 M3 M8
G54
G0 X1.9408 Y-1.5
G0 Z1.
G0 Z0.5
G98 G73 X1.9408 Y-1.5 Z-0.5 R0.1 Q0.05 F15.
X2.4211
X2.9013
G80
G0 Z1.
M5 M9
G30


N20(2D Chamfer1)
M1
T20 G43 H20 M6
S5100 M3 M8
G0 X2.4106 Y-1.5003
G0 Z0.6
G0 Z0.2
G1 Z0.08 F20.
G1 Z-0.04
G1 X2.448 Y-1.4993 F100.
G3 X2.3941 Y-1.5007 I-0.027 J-0.0007 F80.
G3 X2.448 Y-1.4993 I0.027 J0.0007
G1 X2.4106 Y-1.5003 F100.
G0 Z0.2
G0 X1.9303 Y-1.5
G1 Z0.08 F20.
G1 Z-0.04
G1 X1.9678 F100.
G3 X1.9138 I-0.027 J0. F80.
G3 X1.9678 I0.027 J0.
G1 X1.9303 F100.
G0 Z0.2
G0 X2.8908
G1 Z0.08 F20.
G1 Z-0.04
G1 X2.9283 F100.
G3 X2.8743 I-0.027 J0. F80.
G3 X2.9283 I0.027 J0.
G1 X2.8908 F100.
G0 Z0.6
M5 M9
G30


N30(8-32 Rigid Tap)
M1
T45 G43 H45 M6
S1000 M3 M8
G0 X1.9408 Y-1.5
G0 Z1.
G0 Z0.5
S1000
G98 G84 X1.9408 Y-1.5 Z-0.425 R0.5 F31.3
X2.4211
X2.9013
G80
G0 Z1.
M5 M9


G30
M30
%

This isnt rigid tapping FYI.

That said there are a couple things to check. Once you get everything figured out, its pretty repeatable.

First, if you slow your chamfer op speed way down, and add a little dwell you wont get that chatter

I run my tapping at 500 RPM, you need to check that the VFD says thats what it doing and I used a laser tach with reflector on the spindle to verify it too

Check your retract height, if set too low the TC head doesnt have that extra few seconds to fully retract (you will see it pop) If set too high it'll snap the tap

What kind of coolant are you using?

What kind of tap are you using?

Through hole? Blind hole?

First, you are NOT rigid tapping. If you were, you would not be using T/C head.

If you're pulling threads out on the retract, then you're simply not retracting far enough. With a VFD, you have very poor control of spindle speed, so it pays to be very conservative. I normally retract at least 1/4", to be sure the tap is fully disengaged. But the correct value depends on how accurate your spindle speed is, and how quickly the VFD can reverse at the bottom. You have to tune the cycle to suit YOUR machine.

1000 RPM is pretty fast for tapping. I do most tapping at 250-500 RPM. And a #29 drill is ok for hand-tapping, but a bit small for machine tapping, especially if you're not using lots of good oil. I would go up to a #25 or even a bit larger. You might also consider form taps, which are stronger, make smoother threads, and don't make chips. They require even larger holes.

Regards,
Ray L.

+1 for form taps, even more so if you are having to tap a lot of holes in one run

I guess I didn't give everyone enough information. I tuned the VFD for the RPM that I was using with a laser tachometer. This is a through hole so there is plenty of chip clearing. I have a massive flood coolant system so the cut is well lubricated. I did slow the chamfer speed way down but I shared the earlier recipe. The retract height was really low so I will increase that and run again. I will also try running at 500 rpm. I am hoping I have enough torque because I can't switch the belt to low gear in a production setting. I need to crank out parts fast!

That did the trick! 500 rpm and a larger retract height! Thanks everyone!

Maybe I missed it, but what sort of tap are you using? For through holes you'd probably want spiral point taps (aka gun taps). Form taps might be a good option, as others have pointed out, but mind the hole size, which is larger than the hole for standard taps.

Also, you may find that your flood or mist coolant doesn't work as well with tapping as it does with cutting, especially in aluminum. I have much better luck by manually applying a few drops of Tap Magic Aluminum than I did with Hangsterfer S-500 or Qualichem 251C flood or mist coolant.

I use Cool Tool II for tapping. Just a few drops in each hole. No coolant.

I am using a spiral flute tap:

https://www.tormach.com/store/index.php?app=ecom&ns=prodshow&ref=33403&portrelay =1

For flood coolant I use 251C and honestly it cut really well. I do have Tap Magic on hand because it is really great stuff but I try to run the machine unattended for production runs and the tapping is the last operation. It seems like the retraction height was my problem. I didn't think about the lag that the tap has due to the axial motion of the tapping head. This is something to consider because the simulation won't match what actually happens. I ran a test program with 30 more holes after I got the recipe dialed and the results were excellent. Great thread fitment, absolutely silent operation and I didn't break another tap! I'll have to order a form tap just to play around and see the difference in thread quality. Thanks for all the help!

Quote:

---

Originally Posted by MichaelHenry

Maybe I missed it, but what sort of tap are you using? For through holes you'd probably want spiral point taps (aka gun taps). Form taps might be a good option, as others have pointed out, but mind the hole size, which is larger than the hole for standard taps.

Also, you may find that your flood or mist coolant doesn't work as well with tapping as it does with cutting, especially in aluminum. I have much better luck by manually applying a few drops of Tap Magic Aluminum than I did with Hangsterfer S-500 or Qualichem 251C flood or mist coolant.

---

Quote:

---

Originally Posted by sidetrak06

I am using a spiral flute tap:

https://www.tormach.com/store/index....03&portrelay=1

......I didn't think about the lag that the tap has due to the axial motion of the tapping head........

---

I don’t know if it would impact retraction lag because I haven’t used my Modular TC head much, but I noticed when I got mine that axial motion was VERY rough when pulling/releasing the sliding portion by hand. I ended up taking the whole thing apart and using fine emory cloth to take the machine marks off all the sliding surfaces.


Sent from my iPad using Tapatalk

Fairly new to tapping with the T&C head - 500 RPM, 0.5s dwell with m5 spiral point tap and 4.2mm drill. It works well except I get a build up of birds nest on the tap that I have to try and clear with a brush between holes. Any suggestions on how to stop the birds nest from happening?

Thanks,

Dave.

form taps :)

I tap a LOT of 8-32 holes and the way I do it, I haven’t broken a tap in over 40,000 holes.

The program I use is as follows:

Prep commands
S500M3
T?M6
G0G90G43H?X?Y?Z?
Z.25
G1Z-(your depth)F14.0635 (calculated feedrate minus 10%)
M4
G4P.25
G1Z.25F17.1875 (calculated feedrate plus 10%)
M3
G4P.25
(Move to next hole, copy and paste above)

I have tapped holes as small as 2-56 using this method.

The formula is RPM TIMES THE PITCH TIMES 90% going in and RPM TIME PITCH TIMES 1.1 coming out.

I use the ER16 TC tapping head.

That’s about as near rigid tapping as I have been able to do on my PCNC1100 running on MACH III.

If you have any questions, please feel free to give me a call at
714-420-2453 any time between 8:00 AM AND 8:00 PM “WEST COAST TIME.

[QUOTE=Steve Seebold;2156026]I tap a LOT of 8-32 holes and the way I do it, I haven’t broken a tap in over 40,000 holes.

Is the idea here to let the pitch of the thread drive the tap through the hole so that if the RPM/Feed don't match perfectly you aren't pushing the tap through the hole with the z-axis? That makes a lot of sense. I was thinking about this when my tapping head showed up. Assuming the RPMs were perfect, it seems like you would want the feed rate on the way in to be the calculated feed rate or less but definitely not more.

Regarding the birds nest at the top of the tap I just watched a Haas youtube video with what I thought was a great solution. Reverse the spindle direction for a few seconds an the nest is thrown off, then proceed.

Quote:

---

Originally Posted by Steve Seebold

I tap a LOT of 8-32 holes and the way I do it, I haven’t broken a tap in over 40,000 holes.

The program I use is as follows:

Prep commands
S500M3
T?M6
G0G90G43H?X?Y?Z?
Z.25
G1Z-(your depth)F14.0635 (calculated feedrate minus 10%)
M4
G4P.25
G1Z.25F17.1875 (calculated feedrate plus 10%)
M3
G4P.25
(Move to next hole, copy and paste above)

I have tapped holes as small as 2-56 using this method.

The formula is RPM TIMES THE PITCH TIMES 90% going in and RPM TIME PITCH TIMES 1.1 coming out.

I use the ER16 TC tapping head.

That’s about as near rigid tapping as I have been able to do on my PCNC1100 running on MACH III.

If you have any questions, please feel free to give me a call at
714-420-2453 any time between 8:00 AM AND 8:00 PM “WEST COAST TIME.

---

Hi Steve,

I just a beginner, but I have tapped a few holes with my (Tormach) T/C head.
I've always found the threads are a bit too loose, to be honest.

I was talking to a mate the other day, who is a very experienced machinist. When I explained the problem
I was having, he just laughed. He explained that he found this problem years ago when using a T/C head.
The answer was to reduce the feed rate to 90%. He said that there was more than enough "elasticity" in
the head to cope with the standard withdrawal feed rate.

He started telling how to code this and at that point, I must have had a "blank" look on my face, because
I had absolutely NO idea of how to do this.

I have tried Internal thread milling and it seems to work ok, but the thread mills are poisonously expensive.

Seeing the code laid out, as you've done here really makes sense. But to be honest, I don't "hand code"
anything because I'm a (beginner) hobbyist and certainly not a machinist. I use Fusion 360 and I'm slowly
getting used to it.

There doesn't seem to be any provision in Fusion to adjust (just) the feed rate. Is it possible to modify the
Tormach Post Processor. So that if a tapping cycle is called, that it would automatically make the correct
adjustment?

Thanks for your time.

Michael

I forgot to mention, I NEVER use cutting taps. I will ALWAYS use thread forming taps.

Form taps are also WAY stronger than cutting taps, and yes, they do cost a little more.

You need to drill your hole a little larger but that information is available on line.

I learned a long time ago “GOOD TOOLS MAKE CHEAP PARTS”.

My signature line says “ YOU CAN BUY GOOD PARTS OR YOU CAN BUY CHEAP PARTS, BUT YOU CAN’T BUY GOOD CHEAP PARTS”.

I am interested in switching over to a formed tap given how this discussion has gone but I am worried about the torque of the machine. Can anyone chime in here to let me know if I could tap 1/4" thick aluminum with an #8-32 forming tap using the HI gear on a Tormach 1100. It is critical that I use the Hi gear because it won't make sense for me to switch the belt over on every pallet. The cutting tap works great at 500 RPM in HI gear.

Thanks!

it wont be a problem at all. I've tapped up to 5/16-18 with a form tap and never had an issue (im sure you can go larger too)

Quote:

---

Originally Posted by joshetect

it wont be a problem at all. I've tapped up to 5/16-18 with a form tap and never had an issue (im sure you can go larger too)

---

You did that all in the high belt position? That's great!