Tension/compression heads for CNC tapping

[DavidR8]

Following your thread. I have a T/C head for my Tormach 1100S3 but have never used it. I don't know the inner workings, but mine "behaves" like the driven shaft and tapping chuck are keyed to each other and are spread by a compression spring. I attached Tormach's guide for using the head. Hope this helps a little though someone with actual experience will be the best teacher.

View attachment 516463
View attachment 516464

Thanks Bruce, that's super helpful!

 

[DavidR8]

I have this one from Tormach worked great the few times I've used it (new machine, so don't have a lot of experience with it)

There is a little bit of a trick to it - you have to make sure that the tapping cycle G-code doesn't have any dwell programmed. This can depend on what you are using for CAM and the post.

The gist was that with Fusion 360, if you leave dwell out of the dialog box it wouldn't add a dwell value to the tapping / drill cycle and there was some default. However if you specify a very small dwell .0001 seconds the value gets used and truncated to 3 digits and it spits out a dwell of 0.

The head has enough allowance in tension/compression to accommodate a spindle speed that doesn't exactly match the tap threads in additions to being able to handle the spindle reversing.

I believe there is a NYC CNC video about it.

Thanks, that video was super helpful!

 

[DavidR8]

The problem with my Tormach is that the spindle RPMs on the controller display is not 100% accurate; it doesn't have an encoder that measures actual speed. I've never adjusted it, there is a pot on the VFD of my Tormach where the RPMs can be adjusted. It can be done with a Hall-effect tach on the spindle; adjust the VFD so the Hall-effect tach matches the controller's indicated RPMs.

I'm thinking (scary) that the Z-axis feed should be slightly faster than the spindle speed so the tapping head compresses slightly as the tap advances. If the Z-axis feed is too slow, the spindle would be turning the tap faster than the Z-axis feed; the tap would advance at a rate faster than the head possibly pulling it out the the chuck or snapping the tap (?). The Tormach head has about 1/4" of travel in compression; going too fast in Z "should" result in the head compressing as it's designed to do.

This is a snippet of Tormach's instructions:

View attachment 516497

Using their example, a 1/4-20 tap running at 500 RPM would need a feed rate of 25 IPM (500 / 20); feed rate = spindle RPM / tpi. The concern is that my machine may say the spindle is at 500 RPMs, but it may be 450 or 550 since there's no encoder/tach built into the machine. If my spindle was turning at 550 RPM, the feed rate should be 27.5 IPM (550 / 20). I'm thinking (again, scary) that it'd be prudent to go slightly higher on the Z-axis feed than the calculation to compensate for inaccuracy in the spindle RPM. If I were going to use the head, I'd do the procedure in the Tormach manual for adjusting the VFD pot to get as close as possible to the spindle speed at which I'd be running the tapping head.

If I'm correct in my thinking (all theory, no experience), a slightly high Z-axis feed rate would mean that the head is compressed during tapping. The Tormach head has about 1/4" of compressive travel, so there's a little wiggle room depending on the depth of the tapped hole.

Anyway, don't take anything I said as the gospel; it's my understanding of how it works with no experience.

I can see why accurate spindle speed is necessary, I had a digital tachometer before I pulled all the electronics off of it. I swapped the DC spindle motor for an AC servo that I can run as slow as 1 rpm but given that it's belt drive methinks a tachometer would be a good idea.

 

[dbb-the-bruce]

Thanks, that video was super helpful!

Yeah, I was psyched when I realized I'd be able to do tapping with my 770M.

I went with mist / fog buster cooling. I just don't do enough work or the kind of work that would benefit from flood cooling and the mess and maintenance that comes with it. The machine base is all setup for flood cooling, so I can always add it later if I get to production runs that justify it.

But tapping really needs the lubricant. Most of the tapping that I'd end up doing would be for fixture plate type of stuff. I'll have it drill all the holes, pause and then manually hit all the holes with a dab of Tapmatic cream. Restart and have it do all the tapping. This works well for relatively shallow taps.

I spent some time messing with the post processor for other reasons (and I'm a software engineer) - realized it would be easy to add a delay with an air blast from the mister after each tap cycle. So I added that to my post. The blasts and tapping lube aid does a pretty good job of keeping the taps clean for the next hole.

 

[DavidR8]

Yeah, I was psyched when I realized I'd be able to do tapping with my 770M.

I went with mist / fog buster cooling. I just don't do enough work or the kind of work that would benefit from flood cooling and the mess and maintenance that comes with it. The machine base is all setup for flood cooling, so I can always add it later if I get to production runs that justify it.

But tapping really needs the lubricant. Most of the tapping that I'd end up doing would be for fixture plate type of stuff. I'll have it drill all the holes, pause and then manually hit all the holes with a dab of Tapmatic cream. Restart and have it do all the tapping. This works well for relatively shallow taps.

I spent some time messing with the post processor for other reasons (and I'm a software engineer) - realized it would be easy to add a delay with an air blast from the mister after each tap cycle. So I added that to my post. The blasts and tapping lube aid does a pretty good job of keeping the taps clean for the next hole.

It does look like a simple modification to the post processor is easily done even by mere mortals such as myself

 

[dbb-the-bruce]

It does look like a simple modification

Regarding the "zero" dwell trick....

I re-checked this morning and I'm not sure that the "stock" Tormach post processor used for fusion still requires this. I think the important thing is the PathPilot tapping cycle ADDs the dwell if you don't specify it - check the g-code and if there is no P for the tap cycle you will get a default computed one. So regardless of how you get there, just make sure it has P0.
G98 G84 X-0.8258 Y0. Z-0.715 R0.185 P0. F16.406
X0.8258

That's 2 tap cycles at -/+ .08258 X, P is set to 0.
I set the dwell in fusion to .00005 or some ridiculous small value originally. But when I re-ran it today, with dwell set to just 0 it still had the P0. in the g-code. It may have been fixed.

The post I modified for the tap blast is not the Tormach / Fusion default. It's one modified/developed by David Loomes that was suggested on the Tormach users board. I originally switched to it because it handled mist/flood function correctly - you can use either or both.

/*
Copyright (C) 2012-2020 by Autodesk, Inc.
All rights reserved.
Tormach PathPilot post processor configuration.
$Revision: 2980 $
$Date: 2024-04-06 20:42:23 +0100 (Sat, 06 Apr 2024) $
$Author: david $

Modified by David Loomes to support integrated Fusion 360 probing in PathPilot
24/02/19 Initial probing release
13/06/19 Added post support for plane angle probing
27/10/19 Added support for Tormach extended WCS - 500 WCS max, using G54.1 Pxxx syntax
11/12/19 Added support for electronic tool setter (G37)
21/01/20 Incorporated corrections from Autodesk for smartcool processing.
29/06/20 Added support for I/O boards
25/07/20 Added partial circle probing operations
06/08/20 Added support for inspection reports
28/09/20 Added option to turn on output during probing ops
29/09/20 Added multiple options to control retract operations
09/10/20 Added comments to delimit pre-amble, post-amble and tool table
02/01/21 Added Manual NC 'Action' options to control inspection probing
22/09/21 Don't turn spindle and cooling off when retracting for WCS or 4th axis orientation change
22/09/21 Correct error that caused 'redeclaration of function onParameter' warning from Fusion
17/11/21 Added option to retract on All, Automatic, or ManualNC stop and Optional stop *Modifications by Ian Vivero
07/07/22 Added option to add a delay after turning on flood coolant to allow flow to establish
17/07/22 Added partial support for tapping with chip breaking cycle
20/07/22 [x], [y], [z] substituted in comment field for inspection reports.
22/07/22 Added restart, newpart, newcomponent, newtable options to inspection Manual NC action commands
25/08/22 Added use sub programs option for code generation
10/12/22 Implemented option to have probe fast and slow feeds overriden by values in CAM op
14/12/22 Outputs block delete character "/" before optional sections.
17/01/23 Add post option to make all ETS operations optional
14/02/23 Add support for XoomSpeed smart coolant module
24/02/23 Added independent format for tapping feed format. Adds 2 extra digits for very small tapped threads
24/02/23 Corrected some problems with tool setting applied to optional sections
24/02/23 Postamble is never optional
08/05/23 Add option to use coolant to clear ETS
15/10/24 Add option to output stock size and description to header
*/

description = "Tormach PathPilot with probing and ETS";
vendor = "XoomSpeed";
vendorUrl = "http://xoomspeed.com/CNC/FusionPostProcessor.htm";
legal = "Copyright (C) 2012-2018 by Autodesk, Inc.";
certificationLevel = 2;
minimumRevision = 40783;

I can / should provide my hack for the tap cycle blast if you want.
All of this advice is "Buyer beware" !

And my experience may not match what is currently true with the latest and greatest everything.

-D

 

[BGHansen]

Floating holders . The heads are bottomed out when starting the tapped holes . Feed per rev being just under the pitch allows the head to pull forward at the pitch. Instant reverse . Head reverses and still pulls head out until threads are cleared . Head snaps back to closed position . When reversing ,you can program a lead over the pitch as well as the head would be extending . I never did and never had issues .

That makes sense, my inexperience is showing. . . The process would be to measure the tool length (end of tap in the tapping head chuck) and enter that into the tool table. When tapping, advance the tool to a Z of 0 which would put the tap at the surface (assuming the material being tapped is at Zero). Then advance down in Z without the spindle running (?) to compress the tapping head. Turn the spindle on to run the tap and also advance Z down (per the RPM/tpi feedrate). Shut off the spindle when Z hits depth. Reverse the spindle while advancing Z up to remove the tap. Once I work up the nerve to run a couple of trials, I'll let you know how it goes.

 

[DavidR8]

That makes sense, my inexperience is showing. . . The process would be to measure the tool length (end of tap in the tapping head chuck) and enter that into the tool table. When tapping, advance the tool to a Z of 0 which would put the tap at the surface (assuming the material being tapped is at Zero). Then advance down in Z without the spindle running (?) to compress the tapping head. Turn the spindle on to run the tap and also advance Z down (per the RPM/tpi feedrate). Shut off the spindle when Z hits depth. Reverse the spindle while advancing Z up to remove the tap. Once I work up the nerve to run a couple of trials, I'll let you know how it goes.

Please let us know how it goes. I’m looking for tapping options for my CNC mill conversion. My MASSO controller won’t support rigid tapping so thread milling or a tension/compression head are my only options.