New Tapping Head

[dave benson]

The encoders have turned up and I've put the unit together and tested it with files from the old
tapping head, I used one of those usbcnc boards I'd bought years ago.
I've tested it with all the tap types while it was on the bench.

The Gecko had to be tuned.
The usbcnc board just worked.
Mach3 requires it's rotational axes set to rotational.
Mach3 requires rotational axes not to roll over. Important.

One thing to keep in mind when tuning the servo drive for position control tend to overdrive them with a hard tune, often
this results in hunting or dithering around the setpoint this drive has  a softer tune which helps with component lifespan Mach3's
motor tuning is also gentle, in the supplied file if you listen to the motor windings they sound like they are playing music.
In that file the motor is running at 550 rpm, and the gearbox output is 2.25 N\M

I made the adjustment mechanism and have fitted it to the machine, the encoder housing is 3D printed in two parts
that snap together, just out of caution I'll super glue it before running it on the machine.

All I have to do now is 3D print a case for the gecko which will sit backpack style on the motor.

I have some time today, so I'll try to find some motor cabling and give it a run with spiral point and hand taps, I don't expect
any trouble with taps down to m2 and up to m8 in steel but will slowly work up the thread diameter and pitch towards M12x1.5 in al and M8x1.25
to determine an upper limit for safe usage.
 
Dave

[Bob La Londe]

Mach3 requires it's rotational axes set to rotational.
Mach3 requires rotational axes not to roll over. Important.

I'm not sure I understand why this is the case?  Mach 3 will accept a command of G01 A3600.  (Ten threads.)  Is it a function of how your threading routine is written?  Mach 3 will also accept incremental mode, and resetting the working offset of a coordinate inline in the code.    I took advantage of those things when machining Barley Twists with a conventional 4th axis. 

[dh42]

Hello Dave

Just for info ; If you need a working macro for the G83 for lathe, I've one. The original one is bugged, it do not works properly if the code use negative coordinate (ex, if the Z=0 is at the surface of the workpiece)

With the lathe, the G83 is not hard coded like with milling but is a macro called M1083.m1s that is called when a G83 is encountered in the GCode. (same for G77 and G78 that call M1077 and M1078)

Note: This way of using a macro = 1000 + the Gcode value can be used to replace any other Gcode/Mcode that is hard coded, even with milling. Ex, if you create a M1030.m1s macro, it will be used in place of the M30.

++
David

[dave benson]

I'm not sure I understand why this is the case?

10.1.2 Rotational Axes The rotational axes are measured in degrees as wrapped linear axes in which the direction
of positive rotation is counterclockwise when viewed from the positive end of the corresponding X, Y, or Z-axis.
By "wrapped linear axis," we mean one on which the angular position increases without limit (goes towards plus infinity) as the axis turns
counterclockwise and decreases without limit (goes towards minus infinity) as the axis turns clockwise. Wrapped linear axes are used
regardless of whether or not there is a mechanical limit on rotation.

So in short : 
rollover on      DRO  reads 358,359,360,0,1,2
rollover off      DRO  reads 358,359,360,361,362

Thanks David I'll keep that in mind, I took some of my conceptional inspiration from in part the lathe G32.
I have used fusion for the lathe (nice) and now use Ezilathe, sometimes I do the drawing in CB and export a .dxf.

For the most part I use my lathe like this:
Sometimes I just want to clean up a shaft with emery tape so I don't even turn the controller on.

For mostly simple to medium complexity jobs I use the Mach3 built in wizards. This is most of the time.
For threading I use Ezilate (I would not use anything else).
For complex\tricky jobs still use the same procedure but turn the AI in the turrets on.

Standing back and looking at the big picture, the plugin lets everyone from those with a small al based machine
running grbl to a modern industrial controller because the Gcode is simple Gcode commands and not macros
which have incompatibilities in their implementation across controllers.

The other thing is that you get to make a drilling cycle which is identical to say a standard G83
and then customise it to suit the exact needs of a particular task at hand.

I read in a paper somewhere that 90% of the wear on a drill is when it starts to cut so pecking
would shorten the life of the drill but there's cases where clearly because of the nature of the material, you have too, the other day
I started using pauses instead of pecks 'to break the chips really, rather than it being a deep hole or gummy material, so that the
swarf would not curl up around the spindle, this worked well as I could set the length of the swarf (about 50mm) so it was very easy
to clean up later and I had a clear view of the cut during cutting so that I could give it a spritz of cutting fluid.

Would this be better than pecking where you can set the length of the swarf also, I don't know
I guess not, but my machine has really fast rapids so bangs about while pecking where with pausing
I could not hear anything other than the spindle and the swarf length was programmable too.
It was a much more pleasant experience stood next to the mill.

Just as an aside I got my son to hold the motor end of the unit and I grabbed the business end with a rag just to get a
human sense of how much torque was available and it's going to be more than adequate when I did the calc's I rounded
down and used conservative numbers.
The optimistic numbers made it a little under 5 N\m so I went a got a new harder spider for the jaw coupling.
Dave

[dave benson]

I got a chance to 3D print the Gecko Backpack and give it a test fit for alignment on the machine, you undo
one M6 SDHCS to engage and disengage the unit and one M6 SHCS to clamp the spindle.

It weighs 3.5 kg so Ill leave it disengaged but on the machine rather than remove it and store it.
I wired up the servo except for the signal wires as I don't have any on hand and have to get some.

I have managed not to modify the machine and keep inside the guards boundary so I don't have to modify the guard to much.

A nice thing to have when tapping is some indication of the load on the tapping head .
I like Analogue meters and had kept this one for some project or other and forgotten about.
I've connected it a current measuring sensor and it's working. Just as a side project I'll see if I can make a
case for the meter, the idea being to bluetooth it.

Dave

[dave benson]

I got a chance to test the tapping head out with a couple of threads, M6 x 1.0 and M3 x 0.5.
The M6 was a through hole for a M6x1 spiral point tap.

The M3 was a blind hole 10 mm deep and tapped using a Hand Tap to 8 mm deep using an
intermediate tap with the point ground down to make an approximation of a plug tap.

I tested the unit on the bench with a usbcnc card (100khz), and on the machine with a parallel port
with Mach3 running the standard kernal speed of 25khz.
It'll also run GRBL.

I didn't test it to max speed with the bench tests as I would not be able to feed that many pulses to the axis, just to 20000 degrees per minute.
This is what was the default value for the other old one.
This new one can tap twice as fast @ 40000 degrees per minute But I'm not going to change the default setting as it is a good safe setting.
With this gearbox, the input bearing safe speed is up to 1000 rpm with periodic excursions to 2000 rpm so @40000 deg\min is
equal to about 1111 rpm at the input shaft bearing, which is close enough.
It's very quiet in operation, my mill has a geared head so to use the tapping head the
procedure is:
The gcode file has run to the point where the drilling ops are done and the tapping ops start.
The machine is waiting for the tool change for a tap.
I change the tool (tap). And indicate zero. I put a mark on the tap (indicating a master flute)
for clocking threads.

Then:
Turn off spindle at wall.
Place mill head in neutral.
Slide the jaw couplings of the tapping head together and tighten.
Start Mach3 to run tapping ops.

Overall, I'm happy at this point, I've tested with m6 and smaller threads and these will be
mostly what I use, and these can be done at full speed if your game enough.
I'm going to test to M12 x 1.5 in al and M8 x 1.25 in steel later on tonight.

Dave

[dave benson]

Another small update.
I've done more testing in Al up to M10 x 1.5 but got side tracked with the torque meter project
As of today, I've written the firmware for two esp32's, one measures the current to the motor and transmits it via ESPNOW to
the other, which displays it on a portable meter. This is an auto connecting link so after a power loss it will search for and connect to the receiver.

I 3d printed a case and on the weekend assembled it and tested it (I did calibrate it on the bench) so hopefully won't have to do any more to it.

I wanted to have the dial illuminated with different colours from green through yellow to red   according to how close you are to the maximum current draw.
I did try a red, green and yellow leds but they are not bright enough so I might look into a led strip.
I have some time now so will test the meter on the machine and try a few larger threads that I have tapping sized drills for.
Dave

[dave benson]

I connected the torque meter and set the drive trip current 6 amp for this motor.
The other head had a 150  watt motor and a 16\1 gearbox and could do M16 x 2
This one has a 100-watt motor and a 10\1 gearbox ratio so is less capable, and I've found the limit
for this tapping head using the torque gauge.
In aluminum 6060 It can do up to M10x1.5 with some head room left, M12x1.5 requires
more torque than this motor can deliver.
Using an analog meter worked out well and I much prefer using them over digital displays.

Dave

[dave benson]

Earlier in the thread I mentioned that you can clock the threads, so that you can clean them up
so time later if they get damaged.

I got the opportunity to do this today as I found while rummaging through some turret plates, the test plate I did for the last tapping head.
I put it the electrolysis bath, which didn't clean up the threads and left a dark hard to remove
coating.

I did clock the threads on this plate, so copy and pasted the tapping code into a file and ran it through.
To clock the threads you mark the tap (I grind a very small nick into the shank and sharpie it)
 the master flute is the one that starts cutting first, when stood at the mill, the master in this case
faces toward you, this is zero degrees, once you have set the Z axis to the top of the stock you are good to go and run the tapping file.

This works fine IF you are using the same tap, that tapped the holes, in this case I lost the machine and tap that I used.
Luckily in this case I used a Sutton brand tap and they haven't changed the geometry since I was a apprentice.
Unluckily for me I didn't have that tap anymore so I had to manually find the clocking point, To do this I found
and marked the master flute (the one that starts cutting first), I then
inserted the tap into the hole with my fingers and then rotated the tap backwards until it came free from the hole
and noted the face the master flute was pointing to.

I then turned the work in the vice so that face was facing the operator went stood at the machine.
I navigated to the first hole and then loosened the tap a little and wound it into the thread 10 mm
ten threads and then nipped up the tap and went to the MDI screen and reversed out of the hole
This is a 1mm thread pitch, so I issued a F5000 Z0.05 A0 (the start of the hole) in the Gcode.


I'm happy to report that the job went ok, I placed a section of cardboard under the workpeice to
catch any chips which would mean that I muppeted the indicating in, and was making a new but not improved thread.

I used the torque meter, and it read 750ma while cleaning the thread, and 1100ma while rapid retracting. Idle current 750ma - 637ma = 113 ma to clean hole.

I let the file run for an hour or so then ran the rest of the file at full speed 40000 deg\min.
I'm still waiting on the led strips to be used for the colour change indicator, I have written code
so the first thing the meter does on start up is do the Cylon thing (Don't judge me) then show a conventional led VU type meter that
changes colour according to how close you are to the torque limit. The Idea being that the Leds show gradients from green through to red for forward motion
cutting moves, and a set of different colours for retracting.
I'd also like to have a few different modes like a peak meter mode, which would be handy.
I've wired this Axis the simplest way possible, you could for example run the reset line from the Drive to a limit switch input and stop the machine on overload. 
To recover from this error simply reset the controller and type in the Gcode line at the start of the mop.  In this case G0 Z 0.520 A0

I've included the tapping file without the drilling mops as in the case I don't need them.
To set the clocking angle to any desired degree, indicate the tap in master flute facing you when stood in front of the machine, At this point the master flute
should be facing you and the tap is at Z zero, A 0, now using the MDI rotate the Axis to the desired clocking angle and then set the axis to zero.
I have made some adjustments to the plugin (the parser didn't like hanging white spaces in a mop name or duplicate mop names in the file) and will post it in that thread.

Dave

[dave benson]

more pics

[dave benson]

I got a chance to do some more testing with steel.
In the first pic you can see a spreadsheet with my motors specs\gb ratio and coupler torque
capacity.
I've uploaded the spreadsheet so if you are thinking of making one it may help inform some of your design choices.

Red means that you can't thread this hole.
Green means that you can thread this hole.
Purple means that the coupler capacity has been exceeded.

In the second pic are the data for the old tapping head, which could do a lot more threads, originally when I
made the first one I used a love Joy 4 NM coupler; this is the one that's on the machine now.

As I tested up towards M12 (in mild steel) the spider in the coupling was compressing more and more, and I
became concerned about stalling the Axis out and stopped at around M12 and looked up the torque
rating of the coupler and got a larger one.

In the meantime, while waiting for the coupler to arrive I revisited the M12's to see what would happen
increasing the coarseness of the thread each step and noting the compression in the spider.

At M12x1.75 the spider was compressing to what looked like 80% of its original size.
 If I had been closer to the panic button when doing this thread, I would have hit it.
However, I was distracted when the hole started and so saw the last half being completed, the hole ran through ok
so, I let the machine do the other few.

I thought that I may have lost steps on the Z Axis but no, so the takeaway is that there's a little
give in the system regarding backlash, nevertheless at the time added a pirouette
to the hand tapping code to compensate for the free backlash in the system, it won't compensate
for the backlash caused by the spider compressing though.

Dave

[dave benson]

I finished the tests up to M8 x 1.0 in hrs mild steel.
The first hole I tried to tap stalled the axis immediately.
It should have been able to do this hole with a little reserve and after double checking everything which seemed ok?
I took the workpeice to the bench vice and tapped the hole It was indeed very tight to tap as if the tap was blunt so I
inspected the tap with a magnifier  and the grind on the tap looked ok and not deformed.

 At his point I wasn't sure what was wrong, so I waited to the next day and got a branded tap and drill from the
 local industrial supplies place, and I got some cutting compound.

I did the test again and it went fine the spider wasn't getting a hot supper and I could see on the torque meter the that I wasn't close to the drive re-setting.
It turns out that the root dia on the tap from the set I bought of ebay is too big and this is why I thought that the hole was too small.

Dave