Looking for help with tapping steel with 1100 and Tormach Tension/Comp head

Hello Forum,

I am looking for constructive help on threading 1/4x20 holes in .50" 1144 steel, using my PCNC 1100, Fusion 360 and a Tormach tension/compression tapping head.
I tried doing this today and had some trouble. I spotted the hole, drilled it with .201 drill all the way through + .070", then tried to run the tap cycle. The first
hole the tension/compression holder seemed to work fine, no issues but when I tried a 1/4x20 bolt, it would not thread all the way down, through the
material. I looked at my Fusion 360 setup for this op and realized I needed the tapered tap to go more than the +.070" to get beyond the tapered part
of the thread tap.

So on my second test, I set the below hole height to .50" after measuring the tap. This time the tension/compression holder seemed to bottomed out and caused the Z axis to move off its normal top of travel stop position at the end of the tap cycle. I got a yellow flag notice. I then had to reset the X,Y, Z axis stops. So I decided to stop while I was ahead... and seek some help. I am attaching the code for the tap cycle to this post. If anyone has some advice, I would appreciate it. Thanks. Cismontguy

%
(1001)
(Machine)
( vendor Tormach)
( model Tormach PCNC 1100 Series 3)
( description Tormach PCNC 1100 Series 3)
(T79 D=0.25 CR=0. - ZMIN=-1. - right hand tap)
G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G20 (Inch)
G30

N10(Drill2 2)
T79 G43 H79 M6
S458 M3 M8
G54
G0 X0.75 Y2.25
G0 Z0.6
G0 Z0.2
G98 G84 X0.75 Y2.25 Z-1. R0.2 F22.9
Y0.75
G80
G0 Z0.6
M5 M9

G30
M30
%

Tapping with the Tension/Compression heads can be a struggle.
Sometimes the spring compresses on entry and you won't achieve accurate depths.
For thru-holes, I always go an extra 2-3 threads deep to compensate.

Also, G84 doesn't work so great on Tormach's without an encoder.
It's better to do long-hand programming for tapping instead of using G84.
Feed in... PAUSE (one second for the spring to relax)... Reverse Spindle... Feed out
On Tormach's website (and in the manual), there's instructions for long-hand programming for tapping.

For these reasons I prefer Threadmilling.

Hello Russ Machine,

Thank you for your help. Yes, I prefer thread milling too, but do not have a thread mill that small for 1/4" x 20 threads. Plus I have this Tension/Compression head and
I was hoping I could get some use out of it. I have only used it with PathPilot and conversational threading. But I had multiple holes to thread and this was an opportunity
to try again... Good to know about the G84 not working so great on the Tormach. I had looked at the Tormach YouTube and NYCCNC but did not get any real insight into
how they were doing their tapping. Plus neither were in .500" 1144 steel.

When its not a work job I will have to play around with the long hand coding, like you suggest. I do know that you can program Fusion 360 for a Dwell time at the end of the hole.
I wonder if it would be worth investing in a CNC thread mill rather than using a standard hand tap, like I was using? I have seen they are more compact with their thread cutting
area. Thanks! Cismontguy

Hello Forum,

So after reading RussMachine's comments I explored this issue some more. One of the things I found is that the Tormach's slowest RPM is 525. I had programmed my code in Fusion 360 to use 458 RPM because that is what G-Wizard had suggested. I did not know or remember that this was BELOW the minimum RPM the Tormach. This effects the surface feed rate 458 RPM SFR = 30 Ft/min 525 RPM SFR = 34.3 So there is a difference. Also there is no dwell in Fusion 360 but you can add one if you want. PathPilot automatically adds one if you use it for your thread cycle G84.

Here are some other useful links and info I found. YouTube channel for John Saunder's NYC CNC just made a video (10/2020) on the Tormach threading with the Tension/Compression holder. Learned some things there, too. And Tormach has suggestions, like RussMachine said for download on their page for selling their Tension/Compression head. See below. Hope this helps someone else. Would like to hear if anyone else has good or bad results with this Tension/Compression holder? Please post to this thread. Thanks, Cismontguy

https://tormach.com/tts-er20-collet-...der-32021.html

https://www.youtube.com/watch?v=Rwpfj9g278Q&t=359s


Tormach instructions for tapping-------------------

Programming Examples, Tension/Compression Tapping Head
Long-hand Code
This is the preferred method for general tapping.
(Tap: 1/4 20)
N10 G90 G80 G40 G54 G20 G17 G50 G94 G64 (Safety block)
N20 M3 S400 (Spindle on CW)
N30 G0 X2 Y2 Z.1 (Rapid to Above 1st Hole)
N40 G1 Z-.5 F20 (Begin Tapping 1st Hole)
N50 M4 S400 (Reverse Spindle Direction)
N60 G4 P.5 (Dwell, 0.5 Second)
N70 Z.1 F20 (Retract)
N80 M3 S400 (spindle on CW)
N90 G4 P.5 (Dwell, 0.5 Second)
N100 G0 X3 Y2 (Rapid to Above 2nd Hole)
N110 G1 Z-.5 F20 (Begin Tapping 2nd Hole)
N120 M4 S400 (Reverse Spindle Direction)
N130 G4 P.5 (Dwell, 0.5 Second)
N140 Z.1 F20 (Retract)
N150 M30 (Program End)



G84 Tapping Cycle
G84 is designed for use with rigid tapping; however, it can also be used with success when

utilizing a tension/
compression head. A dwell time is automatically calculated when using.
(Tap: 1/4 20)
N10 G90 G80 G40 G54 G20 G17 G50 G94 G64 (Safety block)
N20 M3 S400 (Spindle on CW)
N30 G0 X2 Y2 Z.1 (Rapid to Above 1st Hole)
N40 G84 Z-.5 R.1 F20 (Tapping 1st Hole)
N50 X3 Y2 (Tapping 2nd Hole)
N60 M30 (Program End)
G84 in PathPilot™
Automatic dwell can be overridden by using a P word on the G84 line (e.g., G84 on P2) where

the P value is
the dwell in seconds.
General Tapping Tips
The following tips are applicable to all machine tapping applications.
Calculating Feed Rate
It is very important to use the correct feed rate. The feed rate for a specific tap is

calculated as follows:
For Inch Taps: Feed Rate (IPM) = Spindle Speed (RPM)/Threads Per Inch (TPI)
• For Example, 1/4×20 tap programmed for 500 RPM will need to be feed at 25 IPM
For Metric Taps: Feed Rate (mm/min) = Spindle Speed (RPM) × Metric Pitch
• For Example, M5×0.8 tap programmed for 500 RPM will need to be fed at 400 mm/min

Quote:

---

Originally Posted by cismontguy

I wonder if it would be worth investing in a CNC thread mill rather than using a standard hand tap, like I was using?

---

You'll almost certainly run into problems using a standard hand tap - they aren't able to clear the chips. I think you're probably thinking in the direction of a machine tap. I suspect that, and running the spindle at the correct speed would solve your issue.
I don't use taps myself so i can't comment on G84. I would expect it to work ok if it's documented by Tormach. Also be careful of anything you pick up from NYCCNC !
Step

For my money, thread mill, every time, simply because there is zero risk that a tap breaks and gets stuck in the hole.
Given that tapping is among the last operations, it's SO ANNOYING to break a tap and scrap the part because it doesn't come out.

Micro-100 has some nice single-tooth thread mills at reasonable cost; Brazed carbide on steel shanks I think.

Quote:

---

Originally Posted by jwatte

For my money, thread mill, every time,

---

1/4-20 tap impossible

Quote:

---

Originally Posted by jwatte

Micro-100 has some nice single-tooth thread mills at reasonable cost; Brazed carbide on steel shanks I think.

---

I can't find any Micro-100 thread mills that are cheaper than monthly charges for Fusion. Could you please provide a link?

Quote:

---

Originally Posted by kstrauss

I can't find any Micro-100 thread mills that are cheaper than monthly charges for Fusion. Could you please provide a link?

---

:)
Step

I’ve Tapped 100’s of 1/4-20 with this $30 threadmill, nice tool, though it’s only necked to go .5, might have to finish last few threads with tap.
https://onlinecarbide.com/142056tpi.html

Ha! Yeah, they've gone up slightly on Amazon, but are still reasonable, given that they don't break or even wear out. (I mean, I suppose they eventually will, but ... not there yet!)

https://amzn.to/3jMDkkA

By comparison, the list prices for the Sandvik ones are $200, but they sometimes go for $75 if you can find the right seller at the right time.

Quote:

---

Originally Posted by Dozer56

I’ve Tapped 100’s of 1/4-20 with this $30 threadmill, nice tool, though it’s only necked to go .5, might have to finish last few threads with tap.
https://onlinecarbide.com/142056tpi.html

---

A user on another mailing list suggested https://www.carbidetoolsource.com/si...m-thread-mills They are USA made, good prices, have small sizes and reasonable shipping charges to Canada. Has anyone had good/bad/indifferent experiences with their products and service?