[4]

I Need A CNC Threading for Dummies Book

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!
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.

HardmountRunning.JPG

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.

FirstCutsNewLathe.JPG

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.

FirstSuccessCNCThreading-12-19-18.JPG

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.

10-32-1st-try-12-19-18.JPG

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.
 

Comments

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.
 
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.
 
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]
 
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.
 
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.

View attachment 283133

(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?

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
 
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
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.
 
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.

half-13_first.JPG

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.
 
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.

Best-10-32-122818.JPG

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.
 
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.

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.
 
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.

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.
quadrature.jpg
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.
 
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.
 
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.
 
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 .
 
Last edited:
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.
Sherline_Headstock_base.jpg

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

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

MoreSpringPasses.JPG

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:

GapProblem.JPG

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


Bob
 
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/AccusizeTools-Indexable-Carbide-Turning-2387-2003/dp/B01NH9REZL/ref=sr_1_19?ie=UTF8&qid=1546203334&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.
 
Last edited:
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-Indexable-Carbide-Insert-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.
 
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.
 
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.
 
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!
 
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 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 :)
 
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.
 
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.
 
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

1546367674028.png

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.
 
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

View attachment 283800

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.
1.5-18? :D 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"
 
Last edited:
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.
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.

Success-10-32-02.JPG

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.
 
[5] [7]
Top