# I Need A CNC Threading for Dummies Book



## MontanaAardvark (Dec 20, 2018)

For the last couple of months, my main project around the shop has been moving threading onto a CNC Sherline lathe.  Sort of by definition, anything that gets a small thread on it (say anything from 4-40 up to the biggest threads I've ever used) is going to be small enough for the Sherline's envelope.  I have a Sherline long bed lathe that I bought back around '07 and converted to CNC.  I threaded a couple of things back around 2008 or '09 but other than proving I could do it, I hardly ever touched that lathe.  

This can be long a story and I don't know quite how long to make it.   Not sure how much background is needed.

I'm running Mach3 and Windows 7 on the PC.  Because I have three machines on the same PC and for the generally better performance you get this way, I'm running an Ethernet Smooth Stepper.   Because the shop has moved around a bunch of times in the intervening 10 years, the lathe has been moved.  The last time I tried to just move the axes on the lathe, it didn't respond at all and I had to resurrect all the hardware.  When I went to hook up my home made optical sensor, it blew up.  I had grabbed the wrong power pin.  

I rebuilt it based on an optical interrupter (instead of reflective) from CNC4PC C3 card and made the hardware to mount it.  




I have an oscilloscope and can watch the voltage pulses out of this.  When I look at them, I see that the pulse is about 2-1/2 milliseconds long (2500 microseconds) but jitter about 200 microseconds.  Call it +/- 100 usec.  That's +/- 4%.  Is that a problem?  Don't know.  Nothing to compare to. 

I tried the scratch test and the first time it came out messy.




The threads look less like a"V" and more like a "W".  Like it's missing the index or calculating something wrong.  Plus the threads on the left look different.  The peak of their W isn't as pronounced.  I don't think it's a lighting trick or other photographic thing.

After Jim posted this update: https://www.hobby-machinist.com/threads/fanuc-ot-to-dc_cnc-conversion.66432/page-4#post-630786  One of the things it got me thinking of was just to run the motor faster.  Plus I was suspicious the chuck might be loose.  

Yesterday, I increased the motor speed from 200 to 300 and scratched a blank again.  To be honest, I wasted a couple of days to get a successful scratch to this because I had Mach3 set in diameter mode and was entering the cutter positions in radius mode.   Took me a while to realize the scratches weren't deep enough.  Anyway, yesterday the overlapping 10 scratches looked like single scratch, so I decided to go for it and thread a test piece.  1/4-20. 




It was a little tight - I had to thread on that nut with a wrench, but it worked fine after that.   This is a 1/2" long stretch of 1/4-20 threads.

Figuring that with CNC, if I can thread 1/4-20, I should be able to thread anything, I went for 10-32 in aluminum.  Did the prep work on the manual lathe, and then set it up.  First pass success.  Again, I had to tighten the nut with a wrench, but aluminum would surely shear off if the threading was too far wrong.  




Although the nut screws on well, if you look closely at the left end of the thread, the shape isn't good.  It looks like the cut varying from the right end to the left end is still there.  It doesn't cut exactly the same path every time.  

So I'm not quite done, but these threads are usable in a pinch.  I want to make it better.  My questions of the day are why the threads don't cut the same from end to end, and why do they seem to have more variation the farther into the cut I'm getting.  

Can anyone tell me if the 4% variation in the pulse width/timing is normal?  I see the RPM counter on the Mach3 Turn screen wobble around, too.  Maybe from 295 to 302 when doing the 1/4-20 at 300 RPM and maybe a bit more variation when at 450 RPM for the 10-32.  They don't seem to vary the full +/-4%, but maybe the display doesn't update quickly enough to see that.  Could this variation all be from not using a tailstock?  I didn't think so because I thought the right end would be worse.


----------



## JimDawson (Dec 20, 2018)

First let me say that I'm no expert in Mach3.  But as I understand it, Mach3 reads the RPM before the start of the cut then calculates the feed speed based on that RPM.  Once the cut starts, if the RPM varies then so will the threads because the feed rate is constant.  The spindle/axis are not really geared together.

I wouldn't think a 100 microsecond variation would make a lot of difference in the start position at 300 RPM.  You might try adding a low pass filter (maybe 0.01 mF?) to the pulse output to reduce the spike and smooth out the pulse timing.  I don't know what the input scan timing is in Mach3, but there might be some variation there.


----------



## mmcmdl (Dec 20, 2018)

Try starting your thread cycle at least 4Xs the pitch minimum in the z axis .  For a 1/4-20 thread in aluminum . you should be pushing 1500 rpm minimum . At the rpm you're running , you are tearing the material off .


----------



## jumps4 (Dec 20, 2018)

Hi aardvark
 I fought mach3 for years with this issue and I can give you a few tips
  the latest version of mach3 ending in 66 won't work for threading and that is the reason they made mach4
066 is junk so no matter what you should start there.
I'm using Version R3.043.057 without issue.
I'm in a rush to leave but if you search this site for mach3 and my name "jumps4" you should find the website to download the older versions.
the Sherline is not really ridged enough for most carbide and a nice sharp high speed steel tool will greatly improve the results.
you will probably find your depth of cut cannot exceed .001 or .002  after the first pass  of maybe .010 or less and a lot of spring passes.
the metal rod your threading makes a big difference. I purchased rod from home-depot that will not thread it pulls like bubblegum.
hot roll and a lot of cold rolls are fussy so before blaming the lathe try brass it is the best for minimizing the issues with material.
 This in my 9x20 making threaded inserts in cold roll with HSS tool...   
https://www.hobby-machinist.com/threads/9x20-lathe-cnc-conversion.8692/page-4#post-288577
good luck
Steve


----------



## RJSakowski (Dec 20, 2018)

If what Jim said is about Mach 3 setting the feed rate based on an initial value is true, then there would be no reason to expect consistency in your threads.  The instantaneous spindle speed on a small lathe will vary with the cutting load.  Almost certainly, there will be some slow down from no load speed.  The fact that you are seeing jitter would indicate to me that your spindle speed is varying slightly from one rotation to the next.  On a large lathe, I would expect spindle speed to be much more uniform.  The motor would be fully capable of dealing with any threading load and the mass of the spindle and chuck would tend to smooth out any variations

To accurately thread, the spindle speed should be constantly monitored preferably with multiple pickup points encoder wheel and that information fed into the controller which would change the feed rate accordingly.  

My experience with Mach 3 was on a mill.  Mach 3 would be sending information to the driver motors to synchronize their speed to each other. I am not aware that it would be able to adjust a G code program being executed to compensate for a change spindle speed.


----------



## MontanaAardvark (Dec 20, 2018)

mmcmdl said:


> Try starting your thread cycle at least 4Xs the pitch minimum in the z axis .  For a 1/4-20 thread in aluminum . you should be pushing 1500 rpm minimum . At the rpm you're running , you are tearing the material off .



Mach3 said it couldn't go faster than 300 RPM on 1/4-20 (I'm not sure I remember that right - it might have been 200 RPM)  I got up to 450 RPM on the 10-32 thread.  I may have the axes constrained too slowly - rapids are set to 15 IPM with the standard leadscrews - but I don't think the machine would be capable of threading at 1500 RPM under any circumstances.  

The Sherline headstock is about 1/8 HP and the machine isn't terribly rigid.  In general, the whole system has to balance; speed of rapids, RPMs of motor, horsepower (torque) in the cut, everything.  There are certainly tradeoffs in using the Sherline instead of a more powerful machine, but I'm working with what I have.


----------



## MontanaAardvark (Dec 20, 2018)

jumps4 said:


> Hi aardvark
> I fought mach3 for years with this issue and I can give you a few tips
> the latest version of mach3 ending in 66 won't work for threading and that is the reason they made mach4
> 066 is junk so no matter what you should start there.
> ...



Thanks, Steve.  In real life, I'm Bob.  I keep thinking it says that in my profile, but that's another forum, I guess.  

I will check the version.  This sounds vaguely familiar and I think I might have changed back to 57, but that's easy to check.  

I don't see how I control the depth of cut in the threading wizard.  When I threaded by hand on the Sherline, I never advanced the cutter more than .002 - but that's in radius so .004 in diameter.  Maybe a better CAM program than the easy one that came with Mach3 Turn is called for.


----------



## Liljoebrshooter (Dec 20, 2018)

No ideas on the cnc stuff but that isn't a threading tool.


----------



## MontanaAardvark (Dec 20, 2018)

Liljoebrshooter said:


> No ideas on the cnc stuff but that isn't a threading tool.



It's not?  That's what they're sold as in carbide tool sets.


----------



## JimDawson (Dec 20, 2018)

While that insert is a 60° cutter, the nose radius is way too large, looks like about 0.016 radius, threading inserts for small threads come to a pretty sharp point




or


----------



## MontanaAardvark (Dec 20, 2018)

I don't have a good way to measure that.  To the eye, it looks like a point, unlike my carbide insert threading tool, which has a very rounded tip to my naked eye.  In the full size crop from my original I can see a radius, but I don't see how to measure that.


----------



## JimDawson (Dec 20, 2018)

Ahhh, OK, I looked at the wrong picture.  Yes, the brazed carbide tool will work for threading.


----------



## MontanaAardvark (Dec 20, 2018)

JimDawson said:


> Ahhh, OK, I looked at the wrong picture.  Yes, the brazed carbide tool will work for threading.



D'oh!  I forgot I had that other picture in the mix.  I used that for the scratch piece that it was in the picture with.  At best, the threads would have been U shaped.  Maybe OK for 3/8-16 or bigger, but I don't know why they sell those things.   

I need to order some more of those sharp point tools.


----------



## MontanaAardvark (Dec 20, 2018)

jumps4 said:


> the latest version of mach3 ending in 66 won't work for threading and that is the reason they made mach4
> 066 is junk so no matter what you should start there.
> I'm using Version R3.043.057 without issue.



I'm using R3.043.062.  I think that was because .066 didn't play nice with the smooth stepper.  

Is there any reason to suspect this version?


----------



## jumps4 (Dec 20, 2018)

Hi Bob
I asked about the threading problem in the Yahoo mach2/3 user group where the original beta testers hang out and they sent me to the 57 version I did try others but I don't remember what versions. I fought this for months blaming my machine and breakout boards.
This pdf may help if you don't have it and there may be a rev:3
As far as the tool the less hp you have the sharper that tool better be.
I thread from 300 to 600 rpm on a standard breakout board a smooth stepper may work better but 600 works pretty good on aluminum
I do all threading with coolant.
check the pdf file, your window in the disk may need to be longer to see a defined pulse. my pulse width is optical but had to be wider
here are all the mach3 versions

ftp://ftp.machsupport.com/Mach3/

here are all files related to mach3/4 from their ftp site at Newfangled solutions

ftp://ftp.machsupport.com/../

there are more threading wizards on the mach3 forum and from newfangled solutions there is a conversational lathe program the will do most everything plus threading (purchase item)
Good luck
Steve


----------



## mmcmdl (Dec 21, 2018)

Ah , yep . After seeing what your machine was , I was way off on my info . I figured it was a full blown cnc  . One other idea if needed would be a geometric diehead which would work in your toolholder . Either way , Go with a dead sharp point .


----------



## MontanaAardvark (Dec 21, 2018)

jumps4 said:


> Hi Bob
> I asked about the threading problem in the Yahoo mach2/3 user group where the original beta testers hang out and they sent me to the 57 version I did try others but I don't remember what versions. I fought this for months blaming my machine and breakout boards.
> This pdf may help if you don't have it and there may be a rev:3
> As far as the tool the less hp you have the sharper that tool better be.
> ...



Thanks much for that pdf.  Started reading it already.  

I'm wondering if it's time to switch over the Mach4.  I bought Mach3 around 2005, so I've certainly gotten my money's worth out of it.  I'm running my Grizzly G0704, my Sherline 4-axis mill and lathe on it.


----------



## MontanaAardvark (Dec 21, 2018)

Interesting day.  I've been running maximum rapids on my Sherline motors limited to 15 IPM.  Why?  I honestly didn't remember.  So I put my 1" by .001" indicator on a stand and moved Z back and forth for an inch to see if I'd loose any steps by doing faster moves.  I went from 15 to 40 IPM by fives and only after several minutes of back and forth tests at 40 IPM did it drop some steps and lose position.  I backed off to 30 IPM for rapids.  Then I did the cross slide at 30 IPM (same size motor) and ran it for several minutes (at least 10, maybe 15) and it never dropped steps either.   

That means I doubled the speed on both axes, which will allow more ability to pick proper feed rates.

Then I tried to re-create a piece I had done by hand for my last engine model, about 5 turns of 4-40 on the end of a quarter inch diameter rod.  On this one, I ran the speed up to 1000 RPMs and it went very well.  Probably overcut it a little as the nut wobbles a bit too much.  Most everything else I've done I've undercut. 




I did another 10-32 thread before this, only longer than yesterday's and it looked like the other one above.  The threads look worse the farther to the left they extend.


----------



## P. Waller (Dec 22, 2018)

Does this machine not have a canned thread cycle?


----------



## MontanaAardvark (Dec 22, 2018)

P. Waller said:


> Does this machine not have a canned thread cycle?



*Edit to add:  *I think the answer is yes. 

In the sense that Mach3 has a "threading wizard" that writes a GCode snippet that cuts the thread using a G84 canned cycle.  It doesn't do something like let me say, "4-40 external threads 0.150 long", but I enter starting and stopping diameters, thread pitch, end point, and a few other things.


----------



## mmcmdl (Dec 22, 2018)

That sounds like a canned cycle , although threading used to be G76 . That's inflation for ya .


----------



## P. Waller (Dec 22, 2018)

MontanaAardvark said:


> *Edit to add:  *I think the answer is yes.
> 
> In the sense that Mach3 has a "threading wizard" that writes a GCode snippet that cuts the thread using a G84 canned cycle.  It doesn't do something like let me say, "4-40 external threads 0.150 long", but I enter starting and stopping diameters, thread pitch, end point, and a few other things.


Excellent, this is pretty much what most conversational controls do, this is a Bridgeport control from the 90's.
Easy as could be, fill in the blanks. 
It has a good deal of safeguards that will not allow certain moves in conversational mode but will do whatever you program in G code manually.
Anyone that knows how to run a manual lathe could be running this machine in hours.


----------



## mmcmdl (Dec 22, 2018)

P . To me , that looks confusing . I used a Funuc 6mb ( conversational programming ) on a Makino Count 15 back in the 90s . My codes were something like this .

G76 P1020060 X Z F
G76 P Q U W R

Been a long while ago , so I know this is not perfect  

I miss that lathe .


----------



## P. Waller (Dec 22, 2018)

G76 P1020060 X Z F
G76 P Q U W R 

What could be less confusing then that (-:
1=External thread
2= Internal thread
Lead/TPI
Thread height/Full depth of finished cut
First pass DOC
Following passes DOC
Finish pass DOC
Spring cuts, just as one does on a manual machine, same finish diameter just dusting it off.
Withdraw is the distance that the tool will retract in order to clear chips
Engage Angle is like using the compound on a manual lathe, in the case of this thread it is a  1 1/4-4 Acme thread or 29 Deg. included
Start Z (.200") from the beginning of the part, same as a manual machine
End Z (13 3/8") from zero, same as a manual machine
Start diameter and end diameter are the same unless you are making a tapered thread, same as a manual machine

Anyone with a small amount of experience with a manual machine can run this.

It is fill in the blanks, no code and no math.
Simple manual operation done for you simply by filling in the empty text fields.
If one can not operate a keypad all bets are off


----------



## mmcmdl (Dec 22, 2018)

Yep , similar to the Fanuc , just fill in the blanks .


----------



## MontanaAardvark (Dec 22, 2018)

If I can ask, then, what puzzles me is that my cuts look worse the closer I get to the chuck.  I'm trying to figure out how to fix that. 

It's not like they're the wrong pitch, it's like sometimes the cutter ends up in the wrong place.   Look at the left end of this picture. 




(the bad focus will hurt your eyes if you look to the right - sorry)
See how there appears to be two different cuts?  There's like a wrong number of peaks and they're shaped wrong.  This is about a 3/4" long piece of 10-32 thread.  It gets about the first half of the threads right, but the farther it advances to the left, the worse it does.  I did this after I fixed the backlash but before I adjusted the G00 rapid moves to go faster

This seems like it could only be that it's calculating really wrong values for Z.  I can't see how it could be the index pulse because they don't booger up the threads on the right and if they were wrong by a half or a quarter turn, I'd guess they'd mess up those threads but it would stay the same end to end. 

Any ideas of what to look for?


----------



## mmcmdl (Dec 22, 2018)

Have you tried cutting a larger thread , say a 1/2-13 or so ? If so , same results ? I would put an undercut in the back btw . I think I said it in an above post also , sometimes these small threads can be a PITA and end up looking like a plowed field . You get down to where the material can't support itself and trouble arises . 10s ? Should be no problem , but I did have to use dieheads on alot of projects just because of problems like this . 

Try that 1/2" with an undercut and see what you come up with .


----------



## MontanaAardvark (Dec 22, 2018)

mmcmdl said:


> Have you tried cutting a larger thread , say a 1/2-13 or so ? If so , same results ? I would put an undercut in the back btw .



I haven't cut a 1/2-13, but I've cut 1/4-20.  Not as long, just half an inch.  I think it would have showed up though. 




I can try the 1/2-13 tomorrow morning.


----------



## mmcmdl (Dec 22, 2018)

The 1/4 looks better than the 10 . You have alot of excess stock sticking out of that chuck which multiplies your problems .


----------



## P. Waller (Dec 22, 2018)

MontanaAardvark said:


> If I can ask, then, what puzzles me is that my cuts look worse the closer I get to the chuck.  I'm trying to figure out how to fix that.
> 
> It's not like they're the wrong pitch, it's like sometimes the cutter ends up in the wrong place.   Look at the left end of this picture.
> 
> ...


I can only make some observations on this.
Whenever a machining process develops a change over a short distance such as above there are machine issues at play, otherwise the thread would be awful the entire length and not just at one position, speed an feed must remain constant in order to single point thread as opposed to facing a large part without CSS, the cut speed changes drastically in this case.
That being said there may well be a problem near the chuck where most of the work has been done in the past.


----------



## JimDawson (Dec 22, 2018)

MontanaAardvark said:


> what puzzles me is that my cuts look worse the closer I get to the chuck.



It appears that the Z is losing position as the cut progresses.  But I can't tell if it's over feeding (pitch getting longer) or under feeding (pitch getting shorter) or just variable.  By the end of the thread, the peaks have moved about 1/2 thread pitch.

Let's assume, for the moment, that the Z feed speed is constant.  Then the only possibility is that there is variation in the spindle speed.


----------



## MontanaAardvark (Dec 22, 2018)

JimDawson said:


> Let's assume, for the moment, that the Z feed speed is constant. Then the only possibility is that there is variation in the spindle speed.



I have the luxury of being able to swap out the entire headstock, since I have three Sherline systems.  This one is actually the oldest one and when I did the CNC conversion, I set it up to allow me to pull the headstock just by undoing the one screw Sherline uses.  

Maybe that's the first experiment tomorrow.


----------



## Boswell (Dec 23, 2018)

I wonder if you are loosing steps with your stepper motors.   Does the issue show on every pass? If you just do a few scratch passes do you get the same issue?  You can clearly see an out of sync cutting starting about half way down the threads. running a minimum depth scratch pass would help isolate the issue between hardware and software. If you run several scatch passes with no issue then I would think there is likely a hardware issue when the cutter is under load. If you do get the issue with a scratch pass then more likely it is a software (computer) issue.   

[Edit: I wrote this several hours ago, so a little out of date, not sure why it did not show up right away. most likely the Keyboard to Floor Interface]


----------



## MontanaAardvark (Dec 23, 2018)

Boswell said:


> I wonder if you are loosing steps with your stepper motors.



That's one of the few things I'm pretty sure is good.   While I was testing to see if my speeding up the rapid movements worked I put a 1" DTI indicator on the bench (.001" resolution) and ran both axes back and forth the full inch (one axis at a time).  I wrote a simple Gcode file that ran it 15 full cycles - 15 times in each direction - and then ran that file 10 times.  150 cycles.  Actually I did that more times on the Z axis than the X.    

I have had electrical noise problems with the Xylotex hardware (stepper drivers) before.  I need to take a look at that.  First, though, I'm going to try to thread a half inch rod at 1/2-13.


----------



## jumps4 (Dec 23, 2018)

MontanaAardvark said:


> If I can ask, then, what puzzles me is that my cuts look worse the closer I get to the chuck.  I'm trying to figure out how to fix that.
> 
> It's not like they're the wrong pitch, it's like sometimes the cutter ends up in the wrong place.   Look at the left end of this picture.
> 
> ...




That is the same problem I chased for months.
It is probably the mach3 version....
locate your mach3 directory and make copies of all of the files with the xml extension (so you don't loose all of your settings, pin numbers, motor tuning  )
download Mach3Version3.043.057.exe and run from the site I gave you above
recopy the xml files you saved to the mach3 direcrory if your xml files were replaced.
and that is all there is to changing versions, (you may have to reinstall smooth stepper i'm not sure ) as long as you make copies of the xml files there is no setup. just install and retest
there are better threading wizards in the mach3 forum
good purchase for lathe: http://forum.machsupport.com/forum/index.php/topic,20001.0.html
Steve
Steve


----------



## MontanaAardvark (Dec 23, 2018)

jumps4 said:


> That is the same problem I chased for months.
> It is probably the mach3 version....
> locate your mach3 directory and make copies of all of the files with the xml extension (so you don't loose all of your settings, pin numbers, motor tuning  )
> download Mach3Version3.043.057.exe and run from the site I gave you above
> ...



Thanks for the tips.  Downloaded the new wizard, and was going to look for one anyway. 

One thing I'm concerned about is that Mach makes a lot of decisions on how many passes to make, and other parameters.  Since the Sherline is a light duty lathe, I'd prefer to make gentle cuts.  In the Wizard I'm using, there's no way to limit the cuts.  I'm not doing this for business, so it's fine by me if it takes a bit longer because it makes more passes.


----------



## MontanaAardvark (Dec 23, 2018)

I swapped the lathe headstock.  Long story, but I believe this is the headstock that came with the lathe when I bought it.  

The jitter in the RPMs dropped in half, or more.  At 300 RPM, I see 299 to 301 on the RPM indicator on Mach 3.  

Then I tried the 1/2-13 thread in aluminum.  This is slightly undercut - the valleys aren't deep enough.  I recut it and it was still a little tough to get a nut on, but I eventually did without using a tap.  




There's about .70 to .75 sticking out of the chuck and it's threaded 0.60".  

I didn't try the new threading wizard or "downgrade" to the older Mach3.  Just limits on time available.


----------



## MontanaAardvark (Dec 29, 2018)

I started a thread about this on the Yahoo! Sherline CNC group because it eventually might become a Sherline Chucker lathe and wanted to talk with anyone who has been down that road.  As luck would have it, Ron Ginger, the guy who wrote the Mach3 threading wizard is on that group and gave me some advice.  Ron advocates for Mach4, primarily because threading works much, much better and secondarily because it's the only mach version being supported now.  

I rearranged the shop a bit so that I can see the RPM display while threading.  I setup to cut another 10-32 screw about 3/4" long and did all of that to keep an eye on the spindle RPMs when it's cutting a pass.  The speed didn't change - which seems like the display stopped updating.  While retracting the cutter and getting ready for the next pass, it shows a + 1 (no more than + 2 for sure) RPM difference.  

When I cut the 1/2-13 test piece last Sunday, I could hear the spindle motor bogging down a bit.  Yesterday, when I cut the 10-32 test piece (in brass; 360, I think) I didn't hear the motor bogging down at all.  It's the best 10-32 I've cut but still has an issue.  




The issue in this 10-32 screw has moved from the end closest to the chuck to the end farthest from it.  On the far end, the tops of the threads appear wider - and flatter - and the cuts don't look as deep.  On the chuck end, they look more properly formed.  A nut will thread onto the wider looking end, but requires either a wrench or nut driver.  Once it goes on past that first quarter inch or so, then it's easy enough to thread it on by hand.

I have not downloaded and started working with Mach4 yet.  That will mean redoing my pulse generator and (I guess) going over to a quadrature encoder.  I don't understand what quad encoding does for you; AFAIK, the only advantage is that it tells you the direction.  From the standpoint of measuring speed, they don't do more for you than the same number of pulses/rev that a single pulse would give.  At least, that's what I've been told over the years.


----------



## JimDawson (Dec 29, 2018)

It really looks like the part might be springing away from the tool on the start of the thread.  Just by eyeball it looks like the pitch is consistent.  Maybe program in a few spring passes and see how it looks.



MontanaAardvark said:


> From the standpoint of measuring speed, they don't do more for you than the same number of pulses/rev that a single pulse would give. At least, that's what I've been told over the years.



It depends on the encoder as to how many pulses/rev you get.  In quadrature, you get 4x pulses as the number of lines.  So a 1000 line encoder would give you 4000 pulses/rev.  Your electronic hardware would have to allow for quadrature input to take advantage of that.

If you are only reading the index pulse, then yes, you would only see 1 pulse/rev.


----------



## MontanaAardvark (Dec 29, 2018)

I'm pretty sure I bumped up the number of spring passes from 1 to 2, so still not "several".  That's an easy fix, though.  



JimDawson said:


> It depends on the encoder as to how many pulses/rev you get. In quadrature, you get 4x pulses as the number of lines. So a 1000 line encoder would give you 4000 pulses/rev. Your electronic hardware would have to allow for quadrature input to take advantage of that.
> 
> If you are only reading the index pulse, then yes, you would only see 1 pulse/rev.



I wrote that poorly.  A quadrature encoder gives pulses that are 90 degrees to each other (think sine and cosine).  The timing between those two wires tells you the direction the shaft is going and the period of either signal, either sine or cosine, can give RPMs.  


If you have 1000 pulses per rev, it's possible to sense the speed every third of a degree (0.36 degree) from either wire, but the only information quadrature pulses give that you don't get from either sine or cosine is direction.   Except for the direction information, you're getting nothing out of the two wires that you wouldn't get out of one wire.  I think it's always safe to assume our motors are running in the right direction.  Or look at the quadrature information before starting to cut to make sure the spindle isn't running backwards, if it can.

I don't believe our systems are fast enough to tweak the feed rates thousands of times per spindle rotation and have the mechanical parts respond.  Mach3 apparently only makes the feed rate calculation once between passes.  In my 10-32 example, it used the same Z-axis feed rate for 24 turns.  

Some interval between adjusting Z-axis feed once in 24 turns and "several times per turn" seems like a better thing.  Your encoder may be giving your 4000 PPR, but you're very likely using very little of that.


----------



## JimDawson (Dec 29, 2018)

MontanaAardvark said:


> I don't believe our systems are fast enough to tweak the feed rates thousands of times per spindle rotation and have the mechanical parts respond. Mach3 apparently only makes the feed rate calculation once between passes. In my 10-32 example, it used the same Z-axis feed rate for 24 turns.
> 
> Some interval between adjusting Z-axis feed once in 24 turns and "several times per turn" seems like a better thing. Your encoder may be giving your 4000 PPR, but you're very likely using very little of that.



Mach3 is probably the worst case in that it grabs a sample prior to the start of the cut and as far as I know does not make any adjustments while cutting.  Not sure if Mach4 has the capability of adjusting things on the fly.

My system is a bit different in that it tries to adjust the RPM every 10ms or so, but I know the system can't react that fast. The primary difference is that I'm using electronic gearing so the Z and A axes are tightly coupled with a position update every 62us, so absolutely constant RPM is not a critical factor, Z just tightly tracks A at the set ratio.


----------



## MontanaAardvark (Dec 29, 2018)

JimDawson said:


> My system is a bit different in that it tries to adjust the RPM every 10ms or so, but I know the system can't react that fast. The primary difference is that I'm using electronic gearing so the Z and A axes are tightly coupled with a position update every 62us, so absolutely constant RPM is not a critical factor, Z just tightly tracks A at the set ratio.



That's the way it should be done, and the whole reason I'm going down this road of trying to get my Sherline to make all of my threaded parts is to avoid hard gears.  The gear change system on a manual Sherline is inconvenient and the gear arrangements for some threads (finer than about 28 TPI) go beyond inconvenient to dangerous on my SC4 lathe.   The gears don't fit inside the cover, so that you're standing at the controls to stop the motor with your hand a few inches from a moving gear.  

This is Florida, so I don't wear long sleeves in the shop (not regularly) that would be a bad combination.


----------



## mmcmdl (Dec 29, 2018)

JimDawson said:


> It really looks like the part might be springing away from the tool on the start of the thread.



That's what it looks like to me also , and if it is , you could program a tapered thread to compensate for the spring . I don't believe multiple spring cuts would make much difference .

Or just run a die up on it for finishing .


----------



## MontanaAardvark (Dec 30, 2018)

mmcmdl said:


> That's what it looks like to me also , and if it is , you could program a tapered thread to compensate for the spring . I don't believe multiple spring cuts would make much difference .
> 
> Or just run a die up on it for finishing .



I've run a nut up the last couple of threaded pieces and it works well as a "sorta die".  It doesn't have slots for chip relief and doesn't produce visible chips but after running it back and forth up the threaded rods, they get smoother.  

This makes me wonder if perhaps the headstock isn't exactly parallel with the Z-axis.  How Sherline does that is they used about a 4" long square key to line it up and then single screw to lock everything in place on a tapered shaft.  I should try to check that with my sensitive DTI.  



For illustration, this is an accessory riser that raises the headstock to allow bigger work pieces, but shows the square alignment key and the tapered pin with the large screw that holds the headstock in place.  If that was sitting slightly out of a perfect position, I could see the headstock axis not being exactly parallel to the Z-axis.


----------



## MontanaAardvark (Dec 30, 2018)

For posterity - and those who might be reading and not commenting.  

I tried more spring passes and it's definitely better.  Much better.  




Now it's just the first couple of threads and not the first quarter inch.  I think I can see the brass deflect at the end as its cutting, and then the spring passes taking more at the right end.  I did 8 because I had no idea what number is needed.  I might retry this with a LOT of them.  Like 20 or something.  But - why is the end moving?  

I wanted to try a lathe center or some way of supporting the end to keep the blank from moving.  I don't have a follower rest and don't know if that's the answer either.  My live center is long enough, but wide enough that the cutter crashes into it, and my dead center seems narrow enough but is too short.  I get this: 




I need a longer dead center.  Maybe I need to make something - I've never seen any mention of this before. 


Bob


----------



## JimDawson (Dec 30, 2018)

MontanaAardvark said:


> But - why is the end moving?



Looking much better!

Material springs from the cutting forces, that is just a fact of life.  But you can minimize that with really sharp tools with the proper geometry.  The tool that you are using is not very sharp, and has no rake on the cutting edges (just flat on top).  You need some positive rake to have a more knife like edge presented to the work.  What you have there now is more like a scraper rather than a cutter.  Works fine for roughing cuts with a lot of cutting pressure.

I'm not recommending that you purchase an insert type tool, but here is a pretty good illustration of what it needs to look like.
https://www.sandvik.coromant.com/en-us/products/threading-inserts-grades/pages/default.aspx

You might take a look at these also, they seem to be good tools.  I use them on both my CNC and manual lathe.  But I do tailor the inserts for the specific material and job.  The inserts that come with the set are pretty good general use inserts.
https://www.amazon.com/AccusizeTool...6203334&sr=8-19&keywords=accusize+tool+holder

Hanging your tool out a bit farther from the holder might get you clearance for the tailstock.  Also, most of the right hand side of that tool is doing nothing except getting in the way, grinding as much clearance as you need on that side wouldn't hurt a thing.


----------



## MontanaAardvark (Dec 30, 2018)

No problems on the tool recommendations - thanks.  I don't know enough about them.  I have some replaceable insert tools with triangular flat carbide cutters, but no experience with threading inserts like you link to.   What I have looks like this, only not the name brand:
https://www.amazon.com/Accusize-Ind...-2380-5022/dp/B00I4AW722/ref=lp_257517011_1_3 

I'm using this brazed carbide cutter because it's the best thing I've got, but shopping for replacements is high on my priority list.  Over the years, I've had better results with brazed carbide cutters than the replaceable insert carbides, but never used one like that AccuSize kit.

At some point, I want to try internal threading, which I've never done with single point cutting.

Unfortunately, hanging the tool out farther isn't the axis I need more room on.  The tailstock is hitting the right edge of the cross slide so it can't get any closer.   If the tool were about 0.2 or .25 to the right that might get me there, because the slide would be farther to the left.  The danger there is crashing the cross slide into the chuck.  I don't believe I have a tool holder that would get me there.


----------



## JimDawson (Dec 30, 2018)

You could always grind up a HSS tool bit for threading, I keep a few around for those non-standard jobs that require odd shapes for clearance.  The cutting area on the tool doesn't have to be any deeper than the thread depth plus a little clearance.


----------



## Glenn Goodlett (Dec 31, 2018)

I finally won a three day fight with my Shopmaster CNC trying to cut threads. The ultimate take away was that my machine, for whatever reason, will not reliably cut threads using a G76 cycle. If I use a wizard or write the G code manually that describes each pass on a separate line, the threads are cut perfectly. Go figure.


----------



## MontanaAardvark (Dec 31, 2018)

Glenn Goodlett said:


> I finally won a three day fight with my Shopmaster CNC trying to cut threads. The ultimate take away was that my machine, for whatever reason, will not reliably cut threads using a G76 cycle. If I use a wizard or write the G code manually that describes each pass on a separate line, the threads are cut perfectly. Go figure.



Good to know.  That's a hard won insider secret, so thanks for sharing!


----------



## Glenn Goodlett (Dec 31, 2018)

I wish I knew why G76 would not work reliably. Also if I try to use the NFS wizard, which I like for most things, to cut threads, it tries to cut threads all the way through the stock and beyond. I just don't get it. And I'm certainly not above operator error or lack of understanding.


----------



## JimDawson (Dec 31, 2018)

Glenn Goodlett said:


> I wish I knew why G76 would not work reliably. Also if I try to use the NFS wizard, which I like for most things, to cut threads, it tries to cut threads all the way through the stock and beyond. I just don't get it. And I'm certainly not above operator error or lack of understanding.



I use G32 for single point threading and let the CAM program assign the passes and cut depths.  Saves me from having to think


----------



## MontanaAardvark (Dec 31, 2018)

JimDawson said:


> I use G32 for single point threading and let the CAM program assign the passes and cut depths.  Saves me from having to think



What CAM do you use?  Among the things I'm looking for is CAM.  Screw cutting in particular, but general lathe work would be useful, too.


----------



## JimDawson (Dec 31, 2018)

Fusion 360


----------



## JimDawson (Dec 31, 2018)

I have been using the Haas-turning post.  Seems to work well.  My son does most of the design work, then I take it from there.


----------



## MontanaAardvark (Jan 1, 2019)

JimDawson said:


> I have been using the Haas-turning post.  Seems to work well.  My son does most of the design work, then I take it from there.



Jim, have you ever tried a follower rest?  A well set follower would keep the work from deflecting away from the cutter all along the cut.  Seems better than my dead rest idea.  With a dead rest, even if it keeps the end from moving, the center of the part could deflect away from the cutter.  The longer the part, the more that ought to be a concern.  

It seems conceptually like trying to turn something more than "a few" times L/D ratio.  You know the work is going to deflect too much without one.


----------



## JimDawson (Jan 1, 2019)

MontanaAardvark said:


> Jim, have you ever tried a follower rest?  A well set follower would keep the work from deflecting away from the cutter all along the cut.  Seems better than my dead rest idea.  With a dead rest, even if it keeps the end from moving, the center of the part could deflect away from the cutter.  The longer the part, the more that ought to be a concern.
> 
> It seems conceptually like trying to turn something more than "a few" times L/D ratio.  You know the work is going to deflect too much without one.




No, I don't own one.  If I need to support the work with a tailstock and don't have tool clearance to get in there, then I grind away tool bit or do something else to get clearance.  This could mean making a special center to do the work.  I think the smallest piece I have manually threaded on my lathe is 10-32 with with about 3 inches of stick out.  I supported this with a center and stuck the tool out a long ways to get clearance.

I don't have a picture of the setup but here is the part




I don't have a tailstock on my CNC lathe so everything has to be close to the chuck.  But I don't have much experience yet threading on the CNC, in fact I cut the first actual threads on it yesterday.   It was pretty easy because it was 1.5''-18 thread about 2 inches from the chuck.  Not a lot of spring there.


----------



## MontanaAardvark (Jan 1, 2019)

JimDawson said:


> No, I don't own one.  If I need to support the work with a tailstock and don't have tool clearance to get in there, then I grind away tool bit or do something else to get clearance.  This could mean making a special center to do the work.  I think the smallest piece I have manually threaded on my lathe is 10-32 with with about 3 inches of stick out.  I supported this with a center and stuck the tool out a long ways to get clearance.
> 
> I don't have a picture of the setup but here is the part
> 
> ...



1.5-18?     I'll bet there wasn't much spring there.

Thanks for the info. 

An easy experiment would be to put something in the tailstock to act like a dead center.  A piece of 1/8" diameter steel rod just long enough to clear the tools and with a point on its end ought to work OK.

Edit to clarify that to "... with a point on its end and held in a drill bit chuck"


----------



## MontanaAardvark (Jan 4, 2019)

I think I've finally got it.  Back in post #45, I talked about needing some sort of lathe center to keep the far end from deflecting too far away. 


MontanaAardvark said:


> My live center is long enough, but wide enough that the cutter crashes into it, and my dead center seems narrow enough but is too short.



I was chatting with a friend by email and he suggested I take a broken drill bit, grind a point onto it, and put it in my tailstock chuck.  I didn't have a broken bit handy, but I had a broken #1 center drill (1/8" dia. drilling portion).  One end was broken off, so I ground the good end to reduce its ability to cut.  It took me a couple of days to get around to doing everything, but I tried it today. 

Bingo. After I pulled the cutter and dead center out of the way, a nut threaded on easily and felt the same all along the length. Unlike the others, not different along the length - too tight at the far end and too loose at the near end.




I still preform the brass on the manual lathe, cut it to major diameter, and I drilled the center to put the broken center drill in it..  Transferred everything to the CNC lathe, set my Z dimension, then started the cycle.  First pass success. 

Sharp eyed viewers will see that the my brazed carbide cutter's tip broke off, so the search for new threading bits stopped being academic and I need to get some good cutters, before I try other experiments.


----------

