Hello Guest it is October 14, 2019, 07:53:26 PM

Author Topic: Questions on Threading With Turn on Sherline - From Yahoo SherlineCNC Group  (Read 28347 times)

0 Members and 1 Guest are viewing this topic.


This is an attempt to move some discussions from the SherlineCNC group over here, where I hope to find some information I need.  Over the last several days, we had a long discussion on what it takes to thread successfully on a CNC lathe. 

I have tried threading several times with Mach3 on my Sherline CNC Lathe.  It has almost never worked (I did get one usable 8-32 screw).  Guys on the SherlineCNC list recommended a few things.  First off, stronger steppers than the 70 in-oz motors I'm currently using.  No problem. 

Here's where the Mach questions start: can Mach3 drive a stepper at a fixed RPM to replace the Sherline spindle motor?  I don't see a specific place where I can set this up. 

Next question: I currently have an opto-coupled feedback sensor that appears to give me stable RPM numbers.  They might even be correct.  ;)  But Mach3 doesn't seem to use that information to adjust the Z axis.  Am I missing a configuration issue?  I have just read other folks saying they're sure it does use it, but I'm not sure it works with parallel port drive. 

Is threading addressed in an article or app note or something?  I see the Turn pdf book is the same one I have that goes back many versions.  I've read threading was recently improved, and I have the R3.042.020 Lockdown version, so that won't be documented in that pdf file.   

If Turn can control a stepper on the spindle, I will order 3 new higher torque motors and the spindle stepper mount.  If not, I'll just get 2.  So far, one usable brass 8-32 screw (for $1200) isn't terribly worthwhile.  I'd like to set up my lathe to be more useful.  I am probably more interested in finer pitches, but recently had to cut a 2mm pitch M16 screw in steel (manual cranking the lathe) so I'd like to be ready for anything.


Thanks,
Bob

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Here's where the Mach questions start: can Mach3 drive a stepper at a fixed RPM to replace the Sherline spindle motor?  I don't see a specific place where I can set this up. 

Yes you can set up a spindle motor as Step/Dir, you just asign the pins for Spindle in Ports and Pins, Motor Outputs and then once you have that enabled you can then tune it as you would an axis. You need to calculate the Velocity as revs per second rather than per minute.

Next question: I currently have an opto-coupled feedback sensor that appears to give me stable RPM numbers.  They might even be correct.  ;)  But Mach3 doesn't seem to use that information to adjust the Z axis.  Am I missing a configuration issue?  I have just read other folks saying they're sure it does use it, but I'm not sure it works with parallel port drive. 

I am not sure how well the axis is controlled with the parallel port when threading, there were reports that it was slowing the Z if the spindle slowed down but how well it tracks I dont know. I cant test for two reasons, firstly I use the SmoothStepper and dont have a parallel port on the Pico motherboard and secondly even if I did my spindle has far too much power to let a mere threading tool slow it down ;D
 I can however confirm that the SmoothStepper controls the Z axis well when threading as a recent sheared key in the headstock saw my lathe slowing from 1000rpm at the start of each pass down to around 200rpm by the end and this was the same for each of the 10 passes and the thread was perfect, so might be worth considering?

Is threading addressed in an article or app note or something?  I see the Turn pdf book is the same one I have that goes back many versions.  I've read threading was recently improved, and I have the R3.042.020 Lockdown version, so that won't be documented in that pdf file.   

Threading has been improved but the basic way of threading is the same as it always was, its the way Mach deals with things internally that have changed.

If Turn can control a stepper on the spindle, I will order 3 new higher torque motors and the spindle stepper mount.  If not, I'll just get 2. 


You dont actually need Mach controlling the spindle at all to be able to do threading, all you need is an index pulse but possibly your present motor is not capable of holding a reasonable speed under load.

So far, one usable brass 8-32 screw (for $1200) isn't terribly worthwhile.  I'd like to set up my lathe to be more useful.  I am probably more interested in finer pitches, but recently had to cut a 2mm pitch M16 screw in steel (manual cranking the lathe) so I'd like to be ready for anything.

Think you may be pushing a sherline trying to do m16 threads, in steel especially, make sure you do plenty passes :)

Hood

[/quote]

Offline RICH

*
  • *
  •  7,367 7,367
    • View Profile
Bob,
I have a Sherline lathe and do threading / turning on it. It was a giift, has the x axis extended table, steppers
are around 125 in/oz, microscope attached to it, uses a single index for the pulse to do threading, motor is the newer more powerfull version, and use ean MPG with it. I use it for making small model parts as it fits the need. If you look at what I made thread you can find some postings from me.

I plan on doing some modifications to it. Just struggling with what i really want to do to it, make my owne lathe,
 or modify a mint 6" Atlas i rebuilt and that is laying around, finish a add on attachment for the larger lathe for doing fine work ( basicaly a put in place, very accurate ball screwed x / z ).Too manny options, maybe i will do them all.

The "punny" lathe, no knocks on Sherline, but it could easily take a ride on Hood's lathe carriage.
Just want to keep things in perspective.

Since your interested in turning, you may want to start following the LazyTurn ( currently being developed ) thread and take a peek at LazyCam Turn ( Lazyturn will replace it ). There are manuals in the Members Doc's about both which could be of value to you. I am not going to update / or enhance the LazyCam Turn manual and the LazyTurn manual is constantly being updated to reflect some 250 plus pages of posted text. Feel free to comment as i am open to constructive comments.There is the Mach III Turn manual  but there is no Sherline specific manual.
As far as threading, there are numerous posts about it but nothing captures it concisely for a punny lathe.

Now on to your questions:
Yes you can do threading with it and we have done down to 1/80's. The threading really works well for the
punny lathe users as Art made provision to address issues associated with punny lathes in Mach.
Sorry but it's my lathe and i can call it anything i want! A major problem that someone will have with threading
is accuracy. It dosn't take much to screw up a thread.

I would recomend larger steppers. Tools should be razor sharp and cuts need to be very small / and plenty of passes.
Spindle speed, steppers used, accuracy of the lathe all act as a system. Each can affect how you need to run
the punny lathe for threading and will define what the outcome is. You can use the PP with backlash compensation,
the SS ( backlash is coming ) and modify the threading wizard  for g32 output instead of g76.

I got to go and will post more later. You can write a book on all of the above. I get a chance I'll put something together on this  if time allows. Feel free to ask questions.
RICH

MODIFIED: mACH VERSION 3.042.12 AND ABOVE IS FINE ( if memory serves me) , LOCKDOWN X.*********.20 IS GOOD FOR THREADING.
HAND CRANKING A LATHE HAS IT'S PLACE BUT CNC IS SO MUCH BETTER. NO YOU CAN'T SLAVE THE Z AND MECHANICALY HAND CRANK IT LIKE IN DESK CNC. NO I DON'T WANT TO COMPARE APPLES AND ORANGES.  ;)

    


 





 
« Last Edit: January 20, 2009, 07:00:08 AM by RICH »
Rich, and Hood,


Thanks much for the answers.  Looks like I'll be ordering three higher power steppers soon. They are currently 70 in-oz, and that is very old tech.  They get hot to the touch when just sitting there, my newer 269 in-oz motors don't get hot at all.  I put this system together from junk I had lying around the house, except for the new CNC-ready lathe I bought for the task., so it wasn't really "designed".  I just know I had seen CNC lathes with 70 in-oz on the two axes.  I had them, so I used them.   

"Puny lathe".   I like that name.  I would love bigger iron, but don't really have a pressing need, so I watch the classifieds.  You always want something a bit bigger than you have, right?, so I would like a 9x20 to 9x30 lathe, but not the several hundred lbs. that comes with the size. 

I don't really know where my problem is coming from.  My guess is that the Sherline DC motor does not have the torque at 200 RPM to cut properly, and the motor slows down erratically.  I have to run the motor that slowly because my 70 in-oz motors don't want to go over about 10-11 IPM.  Still, I would think the Z axis would compensate if the speed went down.  What seems to happen is that threads get cut with different pitch farther down the screw, some threads are split in two, with a tool pass down the center.  As an experiment, I tried to cut a a 1/4-20 screw last night, with the parameters in the wizard set for a 200 RPM spindle, but set the motor to about 185.  The thread does not match any other 1/4-20 bolt. 

I will try to find the Lazy Turn thread. 



Thanks,
Bob


Offline RICH

*
  • *
  •  7,367 7,367
    • View Profile
Bob,
1. Assume your using an index for the pulse sink. When you set the rpm at 200 does the Spindle  "Strue" box  change much in the MACH turn window?  
2.How much backlash do you have?
   - are you using backlash compensation?
3.Have you checked the x and z  for repeatability?
4.What kind of stepper drives are you using?
   - what voltage is coming out of your power supply?
5.What kind / size chuck are your using ie; Sherlines?
   - what motor and spindle pulley are you using?

Don't let my questions seem like a PITA, stay with me.
RICH
Bob,
1. Assume your using an index for the pulse sink. When you set the rpm at 200 does the Spindle  "Strue" box  change much in the MACH turn window?  

You mean the value in the Strue box for the speed in RPMs?  I do see it go down under load.  I think it changed "a few" RPM last night when I had it set to 185.

My circuit is an opto sensor that points an IR LED at the spindle and the reflection is broken up by a piece of black tape.  It's a copy of Dave Hyland's design
http://davehylands.com/Machinist/CNC/CNC-Spindle-Encoder/  and gives a good solid logic output, at least, the last time I looked it did. 

Quote
2.How much backlash do you have?
   - are you using backlash compensation?

Yes, I currently have been messing with things and made the backlash worse.  Currently, I have .005", but with backlash compensation, I can go back and forth .100" on my dial indicator and not see any difference. 

Quote
3.Have you checked the x and z  for repeatability?

I have checked them.  They seem to be repeatable, but I don't recall numbers. 

Quote
4.What kind of stepper drives are you using?
  - what voltage is coming out of your power supply?

It is a 24V switcher, so it's a regulated PS, and I believe it's 24V 5A. 

My controller is a Xylotex board.  I had bought a four axis controller from them and couldn't try it out for a few months.  When I did, I had trouble that I eventually determined was its A axis.  Jeff was not willing to swap it out, since it was out of the warranty by the time I first turned it on, and I tried to replace the Allegro chip, ruining that channel in the process.  So I bought a replacement for my mill and had this one sitting around. 

The motors are some 6 wire motors that I am using as 4 wire.  The label says they are "Japan Servo" (brand), 6V, part KP56LM2-097.

When I try to go faster than about 12 IPM, I get awful sounds and the shaft stops turning.  I guess this is the mid-band resonance people talk about.  But I can't overcome it by going faster. 

Quote
5.What kind / size chuck are your using ie; Sherlines?
   - what motor and spindle pulley are you using?
It is a Sherline 3 jaw.  I have a 4 jaw scroll chuck and 4 jaw independent jaw chuck, all Sherline.  The motor is the stock Sherline DC variable speed motor and pulley assembly.  The lathe itself was purchased new last December ('07). 

Quote
Don't let my questions seem like a PITA, stay with me.
RICH

Not at all.  I appreciate the help.  I would not like to drop another few hundred and have it turn out to be something silly I could have fixed. 


Thanks,
Bob

Offline RICH

*
  • *
  •  7,367 7,367
    • View Profile
BOB,
Ii just needed some info to know where your coming form before i take this few more steps forward.
1. good on the rpm it should be steady before actualy doing the threading. The Z feed rate will change
should you spindle slow down and mach will account for it. It reacts rather quickly and compemsates within reason.

2&3. the backlash works very well. Mach starts the z motion and is timed such that idealy you hit the thread right.
    one test recomended is to have very small cuts say 50 / .0001" such that you are cutting but it follows the
threadiing repeatedly  and can be used as a visual of how good things are. i will look around for info on threadiing and post Art's explaination of how it works.

4. 295 in/oz steppers will be more than enough. but....  you only have 24 volts and 5a available so.....
   as you decrease the amps the stepper torque will decrease and as you increase the voltage the speed can be
be improved. so........ because you are both voltage and current limited , lets say 2.5  and 24 volts that the stepper
may be only 150 in/oz and around 20 ipm ( excuse as just quessing ) . now you can run two power supplies and get ( hmm......48 volts and 5a  or 10a and 24 volts i am not realy sure on this read your power supply manual PLEASE) but you may still be limited by the drive max current setting

The current steppers on mine are only 125 oz/in and if got off my duff ii would change them out with the 250's i have.

 Look up the T/S curves for those steppers and see what the graph shows for differenet wiring at 24 volts. 

I am guessing that you are loosing steps at 12 ipm so  change your velocity to 8 or 9. Speed of the stepper will limit  spindle speed used for threading. go into one of the threading wizards and use 100 rpm for the spindle speed and then try different threads and it will tell you if your velocity is ok . If not you need to change your spindle speed. you stepper needs enough torque / speed  to go from stand still and accelerate to required speed to index correctly without missing steps.

5.the old sherline motors sucked ( my opinion ) and don't have the torque of the newer ones. now you can increase the deliver torque if you have and can switch the belting.  I you had a heavier chuck you increase inertia
thus both can have an effect on the motor slowing down during threading.  hey,  ever little bit helps. no i wouldn't
get a new chuck.

Just some thoughts on the punny lathe and hope it makes sense, 
RICH
   
BOB,
Ii just needed some info to know where your coming form before i take this few more steps forward.
1. good on the rpm it should be steady before actualy doing the threading. The Z feed rate will change
should you spindle slow down and mach will account for it. It reacts rather quickly and compensates within reason.
I ruined another piece of brass last night.  Maybe brass isn't the best stuff to try and cut a screw in, but I don't have any conveniently sized pieces of anything else and I have a pound of short pieces of 1/4" brass rod.  Last night, I think the piece moved in the chuck.  There was nothing remotely resembling a screw thread. 
Quote
2&3. the backlash works very well. Mach starts the z motion and is timed such that idealy you hit the thread right.
    one test recomended is to have very small cuts say 50 / .0001" such that you are cutting but it follows the
threadiing repeatedly  and can be used as a visual of how good things are. i will look around for info on threadiing and post Art's explaination of how it works.
That would be good.  I don't have any Gcode for tests to run, and I'm not sure I can come up with any. 

Quote
4. 295 in/oz steppers will be more than enough. but....  you only have 24 volts and 5a available so.....
   as you decrease the amps the stepper torque will decrease and as you increase the voltage the speed can be
be improved. so........ because you are both voltage and current limited , lets say 2.5  and 24 volts that the stepper
may be only 150 in/oz and around 20 ipm ( excuse as just quessing ) . now you can run two power supplies and get ( hmm......48 volts and 5a  or 10a and 24 volts i am not realy sure on this read your power supply manual PLEASE) but you may still be limited by the drive max current setting

The current steppers on mine are only 125 oz/in and if got off my duff ii would change them out with the 250's i have.

 Look up the T/S curves for those steppers and see what the graph shows for differenet wiring at 24 volts. 

I am guessing that you are loosing steps at 12 ipm so  change your velocity to 8 or 9. Speed of the stepper will limit  spindle speed used for threading. go into one of the threading wizards and use 100 rpm for the spindle speed and then try different threads and it will tell you if your velocity is ok . If not you need to change your spindle speed. you stepper needs enough torque / speed  to go from stand still and accelerate to required speed to index correctly without missing steps.

I had not thought of slowing down the feed, so maybe I'll try that. 

My choice seems to be to just replace my Z axis stepper, or replace the spindle motor with a stepper and the Z axis.  I think 70 in oz on the X axis is probably ok, but I'll replace that too.  So one new stepper or three, and if it's all three, maybe I ought to do everything over again.  I like what I've read about the Gecko stepper drives - they seem to have a lot of advantages over the Xylotex drives like I'm using.  Sounds like a 3-axis set of Geckos, a 50V supply, three motors, a mess of wire, and all that junk. 

Quote

5.the old sherline motors sucked ( my opinion ) and don't have the torque of the newer ones. now you can increase the deliver torque if you have and can switch the belting.  I you had a heavier chuck you increase inertia
thus both can have an effect on the motor slowing down during threading.  hey,  ever little bit helps. no i wouldn't
get a new chuck.

Just some thoughts on the punny lathe and hope it makes sense, 
RICH
   

And the thought that never occurred to me until now - find the torque vs. speed curve for that Sherline motor!  I think it's supposed to be good.  Aren't all DC motors supposed to be good at slow speed? 


Thanks again,
Bob

Hate to quote myself, but for context....


And the thought that never occurred to me until now - find the torque vs. speed curve for that Sherline motor!  I think it's supposed to be good.  Aren't all DC motors supposed to be good at slow speed? 


Thanks again,
Bob


According to Sherline, at http://www.sherline.com/dimen.htm - the motor should have its maximum torque at slowest speeds - where I'm using it.  Rough numbers, at 200 RPM, it should have around 450 oz-in of torque.  Way beyond the 270 oz-in stepper I'm considering.  I have my motor pulleys in the "higher torque, lower RPM" setting.

Now maybe the belt is slipping or something like that, but that's plenty of torque. 


Bob

Offline RICH

*
  • *
  •  7,367 7,367
    • View Profile
Bob,
You have the newer motor. The T/S curve I was refering to was for the steppers you currently have.
It's your decision on the purchase of new drives. My point was, that with your current controller you will be limited
on what can be deliver to the new steppers should you purchase them.

Suggest you try cutting 40tpi on the 1/4" stock at a slower speed and say .003" pass depths. Brass is fine, but you can also buy some of that cheap 1/4" gummy Al from the hardware store and save the brass for a later project.
This way you will able to tell how all is working.  While in Turn try  the thread wizard to generate the code.
RICH