Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: BobW4ATM on January 19, 2009, 10:32:16 PM
-
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
-
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]
-
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. ;)
-
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
-
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.
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.
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.
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.
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).
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
-
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.
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.
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.
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
-
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
-
This is what I got tonight. I set the motor speed down to 100 RPM and used the threading wizard (as usual). The threading seemed to go alright for a few passes out of the 12 it was going to take, but afterwards, I could not get a nut to thread onto this.
Then I did something really unusual. Without having changed anything, I started the cycle over again. If Mach always picks up at the start, times and does all the calculations, it should start right again, only this time, it shouldn't cut anything. I've done this manually threading, and that's how it works. Only I heard it cutting a few times. This is how it came out. Clearly it looks like the cutter was never in the right place twice. The name on this picture is well-deserved!
http://www.pbase.com/montana_aardvark/image/108407099
In light of what I got, I turned this piece around to work on the clean end, and wrote a little G-code to go back and forth 20 times along the threaded rod, advance the cutter into the work to make a mark, then pull it back out, go to the other end and repeat. It did this at both ends of a 0.5" gap. Afterwards, I find no places where the mark is not where it's supposed to be, so it was repeatable doing this. No missing steps, and the spindle was running.
What else? I cleaned the chuck with a good degreaser to make sure the blank wouldn't slip, and I always use a live center touching the center of the blank.
If the Sherline motor has enough torque, my Z axis is not missing steps, and I'm running at slow speeds on Z, doesn't this say my wimpy Z-axis stepper is not the problem? Then what is?
Bob
-
Bob,
Wimpy is yours and punny is mine. ;)
I just posted 1 min before you.
Take a cleanup cut for say .75", and use the wizard to generate gode based on the cleaned up diameter,
use the 100 RPM, .....BUT......set the pass depth for .0001" in the wizard. This way you are checking the threading cycle. You won't do any deep cutting so slipage of belts or motor slow down should not influence the following of the tool along the thread. It should repeatedly just give you a fine scroll around the rod at pitch.
BTW make sure the Z starts some distance , .1 or .2" before threading starts as this will give some time
for the stepper to accelerate.
RICH
-
This is getting really old.
Another couple of wasted pieces of brass. This time, trying to cut a 6-32 screw. Turned down a piece of .250 bar until it matched the outside diameter of a #6 screw. Set the motor to 150 rpm and the "first cut" depth in the wizard to .0001". Made the number of passes it set, and the the thing I have is not a screw.
(http://www.pbase.com/montana_aardvark/image/108434363)
The one on the left is the second try for the night, after the first one failed. The first one was a different screw up. I cut the outside diameter too large, using my machinery handbook. Then I measured that cheap, zinc-plated, $1 per pound screw at the top, re-cut it to the right diameter, and ran the threading wizard's output again. It looks more like a screw, but you can see each thread peak is quite wrong.
Questions: I'm using a live center - seems like I have to, because these things are well beyond the 2 or 3:1 aspect ratio that you need a center for. When I do that, it's hard to get much of a running start into the thread (letting Z accelerate). I have used about 0.1" beyond the screw end, but it's crowded there.
Oh, before I cut the thing, I sized the quarter inch rod down to .130 with my CNC lathe, running the motor at full speed, and the Z axis as fast as I dare. No problem. Every pass ended in the right place. So it's not the motor causing EMI getting into the controller box (seen that before).
How fast should the feedback pulse to Mach from the spindle sensor be? Should it be a tiny pulse (thin piece of tape) or is it just looking for the leading edge? What problems should I look for there? The motor speed display looks stable. It drops about 2 to 4 RPM when using 150 RPM, but Mach is supposed to handle that, right?
Bob
-
For some reason, the picture link didn't show up:
http://www.pbase.com/montana_aardvark/image/108434363
Bob
-
Bob
No need to turn the piece down to the dimension first for testing, just cut the thread you want on a lrger dia to see if the pitch is right, that may make it easier for you to try without the tailstock to get a run up. Also it will allow you to use a larger Dia then you can cut off the thread and thread again at the new dia thus not wasting material. I would say you should be fine with 5x dia out of the chuck as long as you have a solid enough grip on it.
Have you enabled the turn diagnostics plugin and then monitored to see if there are any problems with your index pulse?
Hood
-
I don;t think anyone has asked if you are running the 'evaluation' version of the software.
If so, single point threading is disabled and you will simply waste more time and materials until you eventually discover that the feature is crippled . . . as I did.
I have evaluated and then purchased a lot of software, but this is the first time I've come across a 'demo' version that does not make clear exactly what is crippled, leaving the evaluator wasting many valuable hours chasing unsolvable problems. Very annoying. Unconscionable actually, in my opinion.
-
bOB,
Just a few program setting checks here:
1.In config>input signals> index is checked and port & pin iis assigned along with proper pulse setting
" >spindle setup> in special functions box, the spindle feedback in sync is checked and also
spindle speed averaging
2.in config>general config> I use .005 for shuttle accel, 500 for debounce interval / 100 for index debounce
3. in plug control>turn diagnostics - you can use this to monitor the threading as it shows info on rpm, index etc
Don't get frustrated. There is more to just putting in a piece into the stock and running a program.
Why i say this is that, to do threading, a number of things all need to be in place or else poor results.
More so for a punny lathe.
For now all we want to know is the machine is set within it's capabilities, the program settings are correct,
basic threading movements are working correctly. Accurate threads is another story in itself which is greating
influenced by the machine and tool .
So, with just doing a skim cut numerous times we can eliminate some influences which can screw up a thread and check things out plus you waste no material.
Sorry, i walked along your same path and there is no short cut to do a thread.
RICH
-
"When the impossibility has been ELIMINATED, whatever remains, no matter how improbable... is possible."
- Sir Arthur Conan Doyle
We geeky pocket protector types love to quote that . . . but it works . . . so to identify what is NOT causing the problem is useful:
Steppers cannot 'catch up' with lost steps, so eliminating the stepper, lead screw and controllers should be as easy as seeing if the axis returns to their start point after the thread cutting. If they do, then unless I am missing something about how steppers operate, you simply can eliminate the steppers as a suspect.
If your pulse counter is on the spindle with the chuck, then you can eliminate belt slippage as a cause since that would show up immediately in the chuck speed.
The way I read it, you are considering replacing the spindle motor with a stepper. Is that correct? If so, forget about that idea. You can't compare the power available from a stepper and from your spindle motor in terms of torque.
I'll try to explain, but most people have a lot of trouble with these concepts:
How much you can cut is going to be determined by how much POWER you have available.
Torque is not POWER.
Torque is a STATIC measurement of twisting force. POWER (often expressed as horse power), is a measurement of work done over TIME.
The term 'work' involves movement, the force is given as torque and the distance is RPM.
A stepper producing 200 oz in of torque at 400RPM is not producing anywhere near the power of the spindle producing the same 200oz-in at 6,000RPM.
A formula: RPM * TORQUE (in ft-ibs)/ 5252 = HP
so . . power at the chuck: Stepper .0793 vs Spindle motor 1.19
Same torque spec, yet 15 times more power.
Sorry this info won't solve your threading problem, but I think it is relevant to a proposed solution that's been contemplated. Hope it helps.
-
Hey Bob,
This from your first post:
I currently have an opto-coupled feedback sensor that appears to give me stable RPM numbers.
What type of sensor is this ? Later you mention reflective target or such.
Is it sensing on the actual spindle and not the motor or other shaft ?
I for some reason suspect the index signal to Mach to be the problem.
And did you follow Hood's suggestion ?
Have you enabled the turn diagnostics plugin and then monitored to see if there are any problems with your index pulse?
Hood
Threading is working flawlessly here. Actuall threaded 900 pieces today and yesterday, 48 TPI. My best run yet.
-
Threading is working flawlessly here. Actuall threaded 900 pieces today and yesterday, 48 TPI. My best run yet.
We need video!
Dave
-
Wow! So many good replies to answer to. So let me do the simplest one first:
I don;t think anyone has asked if you are running the 'evaluation' version of the software.
If so, single point threading is disabled and you will simply waste more time and materials until you eventually discover that the feature is crippled . . . as I did.
I have evaluated and then purchased a lot of software, but this is the first time I've come across a 'demo' version that does not make clear exactly what is crippled, leaving the evaluator wasting many valuable hours chasing unsolvable problems. Very annoying. Unconscionable actually, in my opinion.
Nope, fully registered. I've owned it for quite a while, although I use it most often on my mill.
Thanks,
Bob
-
Bob
No need to turn the piece down to the dimension first for testing, just cut the thread you want on a lrger dia to see if the pitch is right, that may make it easier for you to try without the tailstock to get a run up. Also it will allow you to use a larger Dia then you can cut off the thread and thread again at the new dia thus not wasting material. I would say you should be fine with 5x dia out of the chuck as long as you have a solid enough grip on it.
Have you enabled the turn diagnostics plugin and then monitored to see if there are any problems with your index pulse?
Hood
I tried a couple of times, but have not been able to get any results from that, and (blush) to be honest, I have not tried to read up on it and learn how to use it.
Bob
-
"When the impossibility has been ELIMINATED, whatever remains, no matter how improbable... is possible."
- Sir Arthur Conan Doyle
We geeky pocket protector types love to quote that . . . but it works . . . so to identify what is NOT causing the problem is useful:
Steppers cannot 'catch up' with lost steps, so eliminating the stepper, lead screw and controllers should be as easy as seeing if the axis returns to their start point after the thread cutting. If they do, then unless I am missing something about how steppers operate, you simply can eliminate the steppers as a suspect.
If your pulse counter is on the spindle with the chuck, then you can eliminate belt slippage as a cause since that would show up immediately in the chuck speed.
The way I read it, you are considering replacing the spindle motor with a stepper. Is that correct? If so, forget about that idea. You can't compare the power available from a stepper and from your spindle motor in terms of torque.
I'll try to explain, but most people have a lot of trouble with these concepts:
How much you can cut is going to be determined by how much POWER you have available.
Torque is not POWER.
Torque is a STATIC measurement of twisting force. POWER (often expressed as horse power), is a measurement of work done over TIME.
The term 'work' involves movement, the force is given as torque and the distance is RPM.
A stepper producing 200 oz in of torque at 400RPM is not producing anywhere near the power of the spindle producing the same 200oz-in at 6,000RPM.
A formula: RPM * TORQUE (in ft-ibs)/ 5252 = HP
so . . power at the chuck: Stepper .0793 vs Spindle motor 1.19
Same torque spec, yet 15 times more power.
Sorry this info won't solve your threading problem, but I think it is relevant to a proposed solution that's been contemplated. Hope it helps.
Thanks. I am the pocket protector/engineer type myself, but my field is radio design. I design high performance receivers for a living. So math is second nature, and I have gone through some of the calculations you talk about since those postings. The only advantage I see to the stepper spindle is that the spindle speed will be under actual closed loop control, but the disadvantage is that the Sherline's motor by itself has way more torque than the steppers I was looking at. Being a designer of control loops (PLL frequency synthesizers), I really like closed loop control, but when open loop works, it's cheaper, simpler, and "good enough".
Bob
-
Quote
Threading is working flawlessly here. Actuall threaded 900 pieces today and yesterday, 48 TPI. My best run yet.
We need video!
Dave
Hey Dave, Video is not allowed in the Blue Room of the Club but I might sneak a photo.
I'm soon moving to the Red Light District.
RC
-
Hey Bob,
This from your first post:
I currently have an opto-coupled feedback sensor that appears to give me stable RPM numbers.
What type of sensor is this ? Later you mention reflective target or such.
Is it sensing on the actual spindle and not the motor or other shaft ?
I for some reason suspect the index signal to Mach to be the problem.
And did you follow Hood's suggestion ?
Have you enabled the turn diagnostics plugin and then monitored to see if there are any problems with your index pulse?
Hood
Threading is working flawlessly here. Actuall threaded 900 pieces today and yesterday, 48 TPI. My best run yet.
The spindle sensor shines an IR LED at the spindle shaft and uses a phototransistor to sense it. The shiny shaft is interrupted by a piece of black tape.
The design is from Dave Hyland's website, http://davehylands.com/Machinist/CNC/CNC-Spindle-Encoder/index.html#01-Encoder.jpg and I know Dave has successfully used it. I have had one screw of many turn out acceptably.
As I told Hood, I did not spend enough time trying to use that tool but tried a couple of times and didn't see how to get info out of it.
I am also suspecting my feedback pulse, although I want to go check that the settings that Rich pointed out are correct.
Here's where I think I am:
1) I think I've ruled out the Z-axis stepper loosing steps. I've run repetitive back and forth motions (20 round trips one time) cutting a rod down and the lathe returns to the same point every time. I've done this a couple of times and different ways. The cut pieces are the right shape without stairsteps from being cut in the wrong place.
2) Since I'm running the spindle at full speed while I'm doing this, I think that rules out EMI from the motor into the Xylotex controller. I had that problem on my mill, although it took hundreds of back and forth moves to really show up.
3) I think I've ruled out the Z axis motor being too wimpy by doing everything at slow speed. The Sherline motor should have around 450 in-oz of torque at the low speeds I'm running. My Z axis is running at 50% of top speed, or less.
4) I've actually watched the threading progress under a 10X magnifier, and I see the cutter not following the thread. It's like it's starting out of sync by some "phase error" (30 degrees, 60...90... it varies). It could be starting in the wrong place in Z, but I think I trust the Z axis (as I said in (1) ).
I think what might be happening is that the spindle pulse doesn't "look" right to the interface. I think it's possible that the spindle sensor might be putting out false or extra edges - perhaps caused by EMI to the sensor from the stepper motors, or the Sherline motor. That is what I wanted to try and test tonight.
Bob
-
I have never used the turn diags myself as it only works with the parallel port and I have a SmoothStepper now. I think the important thing in it is whether it reports problems with the index pulse.
Just out of curiousity can you post the code that you are using for the thread, just in case there is a problem there. Also have you tried cutting a larger dia without the tailstock so that you can get a longer start at the thread.
Hood
-
Another thing Bob,
Is your black tape as wide as this illustration ?
I should only need to be about 3/8" wide for that dia., I would guess.
Also, most other similar applications show a flat black wheel with a shiny spot for the index.
I would try it with a narrow tape first.
Juast a thought,
RC
-
BOB,
I am attaching a file's in two posts which you can use to test your lathe out with.
I still suggest you just do a clean up cut and then color the end of the shaft as shown in
shaft setup pic. Use your 1/4" stock and note that I have the threading tool point at the end of
and on centerline of the stock. Set your cutter the same ( you don't have to have the diameter
the same as mine ) and then set the "X" value to 0.246 in the DRO and also set Z to 0.0.
Set the spindle to 100 rpm.
Note that you can use the diagnostics pulldown to see what is happening as your threading.
You will see the variation of the speeds and also a percent which MACH compensates for.
Additionaly there will be status and also show triggering of the thread cycles. This is a nice feature.
Since the depth of cut is only 0.0001" and 78 passes your should only get a small scribed
line around the shaft.I have attached pictures of the thread path at 20, 40 , 78 passes.
You should get the same results if the all is set up. The last pic is at 30x showing pitch
and width of the cut. Sorry about the picbut it was off hand thru the microscope and the scale turned.
Doing this will enable you to save your brass and check out your system.
If you can't get these kind of results you will never cut a thread worth a darn.
Hope this helps,
RICH POST#1
-
BOB,
POST#2 MORE PIC'S
RICH
-
Another thing Bob,
Is your black tape as wide as this illustration ?
I should only need to be about 3/8" wide for that dia., I would guess.
Also, most other similar applications show a flat black wheel with a shiny spot for the index.
I would try it with a narrow tape first.
Juast a thought,
RC
Mine is actually on the spindle, not the pulley. Here's a shot of mine.
http://www.pbase.com/montana_aardvark/image/108459041
The tape is aright around 5/16" wide.
Bob
-
BOB,
POST#2 MORE PIC'S
RICH
Rich,
Thanks a million for this. It's fantastic. I am carrying the file out to the garage to give this a try.
Bob
-
BOB,
I believe i was looking at your lathe on your site and noticed that the wiring from your sensor was not shielded and ran under the motor. Not good as you'll get noise from the motor brushes getting into the pulse to MACH
Whip out that old specturm analyzer of your's and sniff around! ;) NY3P here! ;)
Shield wires as close as possible to the al box and ground the shield back at the controller.
You mess up the timing pulses and start the z too soon or late relatiive to what was prior cut and your thread is history.
RICH
-
That may be the biggest part of your problem. The sensor is reading/reflecting off of a small radiused surface.
It might be better as illustrated so it reads on a flat surface.
How is yours RICH ?
Good luck ,
RC
-
RC / HOOD,
Is G76 all fixed up now? I havn't tried it in a while.
RICH
-
Hi RICH,
This is 76 all the way.
http://www.machsupport.com/forum/index.php/topic,10344.0.html
RC
-
RC,
Pulse setup here is just like in the manual with a single slotted disc and the opening width based on the calculation they gave in the manual ( slightly under ). For the thread test i just posted, the max variation in rpm was 1.46% and the turn readout will just flicker once in a while from the 100 to 99 rpm in the display. I don't even do an rpm check anymore with the speed indicator anymore as I trust what Mach is telling me.
I can fool wiith my punny lathe manualy, by hand,slowi ng the spindle down and seeing what happens and must say that Art took care of the hobbiest. As you well know, when it comes to thread tolerance, we haven't gone there yet in this thread.
I tend to agree with you that Bob's problem may be the index pulse. I am only quessing, but if the pulse triggers Z start at say a diifferent point of the mark on the shaft, then you will see it by the change of the scribed line. Will need to waite for Bob to get back from the garage.
In the mean time wine and pitza, moma's nice, so i hope he dosn't take too long. ;)
RICH
-
RICH,
I'm using the slotted disc as well. I think the "Through Beam" type sensor is far superior to the reflective type.
It's more positive...ie: either ON or OFF.
I wouldn't wait for Bob if I were you !
I LIKE pitza !
RC
-
RC,
Pulse setup here is just like in the manual with a single slotted disc and the opening width based on the calculation they gave in the manual ( slightly under ). For the thread test i just posted, the max variation in rpm was 1.46% and the turn readout will just flicker once in a while from the 100 to 99 rpm in the display. I don't even do an rpm check anymore with the speed indicator anymore as I trust what Mach is telling me.
I can fool wiith my punny lathe manualy, by hand,slowi ng the spindle down and seeing what happens and must say that Art took care of the hobbiest. As you well know, when it comes to thread tolerance, we haven't gone there yet in this thread.
I tend to agree with you that Bob's problem may be the index pulse. I am only quessing, but if the pulse triggers Z start at say a diifferent point of the mark on the shaft, then you will see it by the change of the scribed line. Will need to waite for Bob to get back from the garage.
In the mean time wine and pitza, moma's nice, so i hope he dosn't take too long. ;)
RICH
Rich,
I'm back.
The final result looked like a frosted rod. It did a thorough job of removing all of the marker, not a clean little spiral.
Now to figure out why.
I readjusted my lathe Z axis and got it down to .001 backlash. I take that out with backlash compensation. My x axis had .0022 backlash (I'm in diameter mode - does that mean .0011 radius, or does diameter not matter in backlash??). Whichever, I'm able to crank that out in backlash compensation so that a dozen back and forth moves on each axis (one at a time, of course) doesn't end up with the needle of my DTI off at all.
But I did move the wires from the power cord and sensor apart and it was a noticeable difference. The first few turns were everywhere, moving them made a difference and slowed down the wander. It's still intolerable, but it did get better. I did one wrap of the power cord on a big ferrite toroid I had lying around, but that didn't do much.
I opened up the diagnostic panel, and it never showed my RPM off by more than 1%. It never showed the pulse missing or anything. It seemed perfect.
Tomorrow, I'll re-wire that sensor. I think I put a simple filter on the board, but I'll double check and add one if I need to.
Thanks for all the help.
Bob
-
I had issues with my indexing on my lathe when I first got it going. I have the single slot type. I used to get rpm readings in the millions sometimes, and nothing made sense. Fixed it by; Adding a diode across the signal wires off the sensor, shielded the signal wire, and moved the signal wire away from the toroid transformer. It works flawlessly now, am very pleased with it, and have excellent results with the G76 wizard on version 1.84.001.
IMO, I think that your reflective sensor is a certain problem, and on a small diameter is bad as well. Go out to the machine and change all that out for a slotted type and I bet you'll finally be able to sleep nights for once....!
DaveA.
-
Bob,
Backlash is just the non-movement of the axis. The value you use has nothing to do relative to radius or diameter
mode. So if the X has .0022 non movement then that's the value you input in the backlash screen.
My x axis has .004" also i also use 60% as a backlash speed.
Let me explain:
The z has done a rapid ( it is not returning at the F feed rate which was used to cut the thread) back to it's starting
location. In the program i think the distance is 0.1" in the plus z direction, so lets call it point "A". Now when it reaches point "A" the z comes to a stop. You defined to Mach that there is non-movement via backlash in your configuration. So MACH is smart and thinks "before i let the Z travel to do another thread" i need account for the non-movement by macking the stepper turn some. Thus the stepper gets pulses to turn enough to take out your .0022 inches and lets call this "B". Now when the stepper rotates for that small amount, it can rotate at your max velocity or a percentage of the velocity. I just use a value of 60%, there is a setting in config>shuttle wheel setting>shuttle accel which affects how fast the stepper will rotate also. Now the Z is at point "B", it gets a signal ( that index pulse ) from MACH to move and should arrive at point "C". Point "C" is a point realtive to the thread, and thus the next thread cut is done.
So, return to the start point "A", squirt some clorox on the tires and smoke them soft and sitting at point "B",
rev limiter and line lock on......red-yellow- GREEN....., pop that clutch and let them horses go wild, off to and cross point "C" and the parachute opens at "C" taking care of what needs to be done after the finish line.
OOPS, I lost the race, disqualified, and hit the dirt bank. What went wrong, ??? dam i was running for brass pink slips. >:(
The little vw bug beat me! :-[ Think i need to look at what is happening on his end. ;)
RICH
-
Rich,
I guess it really isn't that important to my threading issue, I just wanted to understand what I saw. I turned off the backlash compensation and commanded the X axis to go 0.2" so it would go one full revolution on my 0.100" per turn DTI. I measured it being about .0022" off, entered that in the backlash compensation, and now it hits the indicator "dead nuts" on 0.100" every time, each way.
So I started wondering did I have .0022" or .0011" and Mach was outsmarting me? No big deal, because (like I say) I know by watching my DTI that I can go back and forth and that needle never misses the zero mark by a tenth (.0001). I think X axis has to matter less than Z for threading. Yes, the depth of the thread may be wrong, but you can make more cuts if they're in the right place every time.
Now off to look for a way of shielding or filtering that feedback wire....
Thanks,
Bob
-
Bob,
Try wrapping some Al foil neatly around the wires or slipping some brade over them, also twisted pair adds
impedence to noise, and a tight loop over a pencil or such can assist also.
As far as the X axis not as important as compared to the Z. Not when you start cutting some of the small stuff as
there's not much room for error in a nice thread. And I don't know how to pick-up a thread in CNC threading.
RICH
-
Rich, running the thread again if you have it still in the chuck is not a problem, if its been removed from the chuck then that is not going to be an easy task to get set up for a re-run.
Hood
-
Bob,
Try wrapping some Al foil neatly around the wires or slipping some brade over them, also twisted pair adds
impedence to noise, and a tight loop over a pencil or such can assist also.
As far as the X axis not as important as compared to the Z. Not when you start cutting some of the small stuff as
there's not much room for error in a nice thread. And I don't know how to pick-up a thread in CNC threading.
RICH
Not much difference.
Rummaging around the house, I found I had a MIDI cable that I haven't used in ages. This is 4 conductor, with a shield wire (5 conductors in all) and aluminumized Mylar ground shield around it all. So I hooked up three ground wires, power and signal. Brought them up to the other end of the harness (plugs into my box) and spliced it there.
I just don't see much difference. Maybe a bit cleaner, but nothing to write home about.
I guess I'll plug the motor into a completely different outlet. I had to do that once before. Right now, everything is plugged into an UPS.
Bob
-
Bob,
The easiest way to check it would be with a scope to see if progress is being made, as you do only .....ONE .....
change at a time, .....even minor....., otherwise you may be chasing you tail around ( sometimes just black magic works and i can't explain that ). The best approach is to eliminate the source but then sometimes that's not even possible. For the amount of time invested, i would just change to the simple index as stated before, get it running, and then go back and see if you can get your pick up working.
That's my nickle,
RICH
-
Hood
After removing from the chuck is what i ment. One of these days i'll fool around and try post removal.
Fortunately, for what i do, only a penny of material is wasted. Pretty soon i will have enough for
ball screws. :)
RICH
-
Bob,
The easiest way to check it would be with a scope to see if progress is being made, as you do only .....ONE .....
change at a time, .....even minor....., otherwise you may be chasing you tail around ( sometimes just black magic works and i can't explain that ). The best approach is to eliminate the source but then sometimes that's not even possible. For the amount of time invested, i would just change to the simple index as stated before, get it running, and then go back and see if you can get your pick up working.
That's my nickle,
RICH
Rich,
I think I spotted something odd. You said a while back
1.In config>input signals> index is checked and port & pin iis assigned along with proper pulse setting
" >spindle setup> in special functions box, the spindle feedback in sync is checked and also
spindle speed averaging
I did not have the "spindle feedback in sync" button clicked. When I did this, running your 78 line program, it moved very oddly. Sort of step, sit a while, step, sit a while, and so on. It was so odd I stopped it without running it any length of time.
Any idea what might be going on??
Bob
-
Wow, this is turning in to quite a thread . . . yuck, yuck.
There are two ways to single point threads; a straight plunge, or cutting only one side of the 'V', which I would imagine would be far better for the 'puny' lathes. In either case, backlash is irrelevant as you always cut in the same direction. Your error far exceeds the backlash so it would be an academic discussion even if you were improperly cutting the 'near' side of the 'V' where backlash might come into play.
Having seen the picture of your pulse trigger setup, I believe that is your suspect. The color is not as relevant as the surface, I would imagine. You have shiny tape on a small radius. It is probably only slightly less reflective than the shaft itself. Perhaps even more so to IR light. You can see the highlight on the shiny black tape even in your photo. That's also probably what the sensor is seeing.
To support the consensus, I'll add that I also use a slotted disk. Single round hole of about 1/4" dia. Mach seems extremely accurate picking up deviations of a few RPM at speeds over 6,000 and also reading steady at slow speeds.
My sense is that at very low speeds like 100RPM, more than one slot would be beneficial, but it appears from several people who have posted their successful threading experience, that one pulse is sufficient.
There is enough information now to suggest that moving your black area to the face of the disk instead of the shaft as suggested by RC (Overloaded) would probably solve your problem. You also should use flat black, and not something shiny. Even better, as has also been suggested, go with a slot or blade arrangement for the most positive trigger.
As a minimum, strip off that shiny tape and spray some flat back paint in it's place,( and you might consider making it significantly narrower as well) - or - (for diagnostics and not as a permanent solution) take some 600 or finer grit wet/dry and at least scuff off that shine!
-
Bob
Sounds like Mach is not seeing the Index properly if it is jittering about like that.
Simpson
Art did a bit of a write up regarding Index versus Timing , if I remember correctly , it all boiled down to if anything Index was best.
Hood
-
Bob
Sounds like Mach is not seeing the Index properly if it is jittering about like that.
Simpson
Art did a bit of a write up regarding Index versus Timing , if I remember correctly , it all boiled down to if anything Index was best.
Hood
But Mach reports a solid RPM reading, and the threading diagnostic plug in says 1.39% maximum speed error. Does that report properly if the pulse is missing?
BTW, the jump does seem to occur every RPM.
Bob
-
I think you need that enabled for threading so enable it and run the plugin again and see if it reports differently this time.
Hood
-
BOB,
You need to have the spindle feedback in sync mode checked or threading WILL NOT WORK right.
At one time, if memory serves me, threading wouldn't work at all if the index wasn't checked.
I also agree with HOOD on the single index pulse is all that is needed. That's all you need know for now
and can discuss it later on if wished.
What do you mean by step / sit a while? ie; did the z actaully move then stop? or did the stepper just turn very slowly a "small" amount and stop. In the lathe diagnostic info screen was it jumpiing back and forth between
Waiting for index trigger / threading in effect? It should be green in the box when waiting for the index trigger
and upon a trigger, the threading in effect box should turn green.
Can you look at the pulse signal with a scope?
RICH
-
Hi All,
This is going to be a bit long, and I'm going to address a bunch of things.
The big news: I got it working.
One of Rich's "78 passes" tests yielded a bunch of nice parallel grooves. Then I did a 1/4-20 bolt. I started with .250" rod and didn't realize that's too big, but I was able to cut the threads and it looked great. When I turned the finished screw down to the same size as a bolt I had, that (of course) buggered up the thread profile. So a nut doesn't fit it, but it looks gorgeous compared to everything I've been getting up till now.
The problem? The big problem was that I believe it was using the wrong polarity for my sync pulse! It was "active low" and my pulse is active high. Sheeeeshhh. But to get to the point where I found that I had to take everything apart again and test all the hardware. I got to the point where I was absolutely sure the hardware was right - or as sure as I could be. Then I was convinced it was software or configuration. I just didn't know what it was.
Not having the "spindle feedback in sync" in software setup was a complication. That didn't work, and threading would not have worked without it. When I set the sync pulse active high, it started to work properly.
I have a good oscilloscope, a Tektronix 475 if that means anything to you. I looked at the pulse train out of my sync pulse encoder and it was as clean as can be. No extra pulses, no glitches, no noise - nothing but clean square waves. While I'm sure the kind of pulse encoder many were recommending would be really good, this one works as well as it needs to. When I set the RPM rate low enough, I could watch the tape go past the sensor and see the pulse hit on the o'scope. When I set the speed to 60 rpm in Mach (1 rev per second), I can measure 1 pulse per second on my oscilloscope. When I set it to 600 RPM (10 PPS), I measured 10 pulses per second on the scope. Likewise for other easily figured out speeds in RPMs. Since Mach was telling me the right numbers, numbers I can verify at the spindle sensor, I had to conclude the whole path from the IR sensor through my Xylotex controller and into Mach must be good.
So I dug back into all the configuration menus and found that "active low" thing. I must have looked at it a thousand times. I actually threaded some screws about a year ago, so it must have all been right then. I have no idea how it changed.
Right now, I'm pretty tired. I will try to put up some interesting pictures tomorrow. I'm hoping if anyone needs to learn about threading, this message "thread" might be helpful, especially if it's complete.
Bob
-
Excellent news Bob and thanks for coming back with the conclusion. So many times a thread just stops and we kind of guess a resolution has been reached but are never sure, when it is actually written that the conclusion has been reached then it, as you say, gives others a lot of help if they have similar problems.
Hood
-
:) Good for you Bob and have fun. :)
You may want to check out the Canned Cycle - Threading G76 item 10.7.18 on page 10-16 of
Using Mach3Turn.
RICH
-
Bob
Sounds like Mach is not seeing the Index properly if it is jittering about like that.
Simpson
Art did a bit of a write up regarding Index versus Timing , if I remember correctly , it all boiled down to if anything Index was best.
Hood
Hood, can you elaborate on this or point me to the writeup?
-
Simpson36,
Think you may want to have a look at this posting. There may be a few others that Hood can point you to.
There's a lot about threading in that thead as it progresses from being broken to having it fixed.
http://www.machsupport.com/forum/index.php/topic,7646.msg49006.html#msg49006
RICH
-
Simpson, below is the writeup Art did, I have put the relevant paragraphs in bold but left the rest so you can see it in context.
Hood
Re: [mach1mach2cnc] Index or Timing?
Hi Guys:
Just to help clear confusion..
The INDEX input takes a one per revolution pulse. IT then calculates the speed
of the spindle from that timing,
and during a thread, calcuates if the timing from rotation to rotation slows. If
for example, the average rotation is 350us
prior to the actual motion of the thread.. ( Average time per rotation is
calculated when the spindle is on and no motion
is in effect ), and during a thread the time of one rotation is found to be
400us, this means that the last rotation took 50us
longer than the standing average ( a 14.28% slowdown) , then the axis motion is
slowed by 14.28% during the next rotation,
this repeats from rotation to rotation to end up with as near a perfect average
time of axis vs spindle rotation speed.
When using the TIMING input instead of the INDEX input, the system looks for
multiple pulses, but in particular looks
for a pulse 50% wider than the others. This 50% wider pulse is then considered
the INDEX, and the system does the
rotation speed calculation only from that pulse for the spiindle speed display.
However, the other pulses are counted, and
the total rotation time is divided by the number of pulses. SO lets say you have
4 pulses, one of which is 50% wider than the
rest. Any threading will begin on the widest pulse as the trigger, but the time
from pulse to pulse will be calculated and
compared to the total average time of rotation divided by the number of pulses.
The system will slow down axis motion to
correct for deviations between the pulses.
So more pulses will not give you a faster DRO update of rotation speed, but in
theory will correct more often for slowed
down rotations. Its been proven however, to have no advantage in the thread.
While a mathmatically theoretical advantage
exists in the multiple slot theory, any advantage gained seems to be lost in the
disadvantage of additional complexity of the
correction. There are several reasons for this internally and in the required
timing and math. My suggestion is to use INDEX
and not TIMING as a result. KISS is an important principle here IMO.
The SS is being written to use the INDEX method of timing sync at first, it
will then branch to encoder sync which is much
more exact and allows for things such as stopping a spindle and having a thread
stop and continue when the spindle is restarted.
This really required only a much higher granularity of timing than the PP
driver. TO sync to a encoder in the PP woudl require
the ability to vary the interrupt timer on granularities smaller than the
available 40us ones ( in 25Khz mode). Since the SS has
a 4MHZ maximum granularity, its much more possible to vary timing in smaller
increments thus matching exactly ( pretty much) with the varying encoder count
to count time. It is this granularity issue that guides the threading design in
current Mach3, and forces the consideration as above. By all that I mean if the
system determines a motion must slow to match a spindle, the PP driver has only
the power to create a bresenhamed output timing based on 40us granularity, the
SS could use a sub microsecond timing variation which would be invisable to the
end drivers. Any such correction can be thought of as purposely added jitter to
the output stream, Jitter slows the output stream by the required percentage but
causes a phase shift on the drivers output, so it must be kept low and the PP
driver is limited to 40us pulse to pulse variablity, usually thats much lower
than a driver can effectively see in its resultant phase shift, but in the SS
the timing jitter should be able to be much much smaller and totally invisable
to the driver which is the sought after end effect for a perfect threading sync.
Jitter, often thought to be a problem in pulsing output, is actually used as a
benificial effect in Mach3, and the amount of jitter is tightly controlled to
take advantage of its good effects, and keep it low enough to minimise its
negative effects on the drivers phase timing stability. All digital based output
timing has jitter, its a matter of understanding it and using it effectively. In
threading , Mach3 uses a system of control very similar to Mariss's look forward
trajectory smoothing technique, but it was developed long before that.
End analysis: stay with INDEX when using a PP unless you have some inherent
reason for trying the TIMING input. The theoretical advantages dont outweigh the
mathmatical disadvantages.
Thanks,
Art ( just a user who knows a little bit about timing. :-) )
-
Hood,
Thx.
I wasn't considering 'timing' vs 'index' in terms of Mach3 specific vernacular.
As I read it, 'timing' is theoretically better, which is what I was thinking, particularly at slow rotations. However, the real world limitation is the PP and granularity at 25khz, which is also understandable.
For steppers, I'm learning more and more advantages to the Smooth Stepper.
When I do another conversion, it will be with servos, so I won't be able to benefit from that piece of technology, but I find it interesting none-the-less.
-
Simpson, the SmoothStepper has been badly named, well not so much badly named but rather unfortunately named as it tends to make people think it is for Stepper Motors only. That is not the case and actually it is servos that can really take adavantage of the SmoothStepper. I have big AC Servos on my lathe and previous to the SmoothStepper I could only get 3.4m/min rapids due to the high encoder count and that was with 1:2 electronic gearing in the drives. Now I can easily get 20m/min, if I dare, with no electronic gearing, but have actually settled for 10m/min as 400Kg of saddle flying up to a chuck at faster than that has me a bit frightened ;D I did do a vid of the Lathe doing a job with the parallel port and then I did another with the same job and the SmoothStepper.
Hood
-
Rich,
Thx for the link. This excerpt from Art's explanation defines what I was talking about exactly:
"The second possability is a slightly varying index pulse in time.Ive seen
many sensors, ( my own included) that cause RPM variations due to being too
sensitive and varying in time from pulse to pulse. Adjusting sensitivity
solved my own issue with that."
I'll read thru the entire thread when I have more time.
Hood,
Thanks again! Obviously I have to do some more homework on the Smooth . . . uh . . . 'driver' board before discounting it! Thinking a bit further thru the idea, the servo drivers from Gecko (for example) take the same inputs as their stepper driver? And SS is generating those inputs, so it does not care what is being driven? Is that basically the crux of it?
BTW< I commend you both for infinite patience with an endless stream of stupid questions from we newbees.
-
Simpson,
yes basically the SmoothStepper is just replacing two parallel ports and actually gives you an extra 6 inputs on top of that, of which 3 are differential. Another great thing about the SS is that you can use the Index pulse from an encoder for the spindles Index and hopefully soon Greg will get a chance to work on full encoder integration which will tie the spindle and feed together, I think Art mentioned that in the write up but have not reread it in full for a while. The SS puts out a very nice pulse right up to 4MHz and I seem to remember Greg thinking 8MHz would even be possible, but dont quote me on that.
Hood
-
:) Good for you Bob and have fun. :)
You may want to check out the Canned Cycle - Threading G76 item 10.7.18 on page 10-16 of
Using Mach3Turn.
RICH
Thanks Rich, and especially thanks for all your help.
I've put a few shots up on my pbase account to show a little of the process:
http://www.pbase.com/montana_aardvark/image/108518311 is a scope shot of my RPM sensor output
http://www.pbase.com/montana_aardvark/image/108518321 is a "backed out" shot showing how the scope probe was attached http://www.pbase.com/montana_aardvark/image/108518327 is a gratuitous close-up inside the box.
http://www.pbase.com/montana_aardvark/image/108518329 shows my first successful pass of your GCode, 78-pass file.
I need to read that section and not rely on the threading wizard. I really don't know enough about this subject. I need to learn everything I need to know to sit down with hunk of raw material and end up with a finished threaded "part". That 1/4-20 screw I made last night was too wide at the far end, probably due to deflecting at the far end because of the force from the cutter. So I need to use my live center - or some kind of center - and still get enough room at the end of the screw to do everything.
The guys that cut tiny screws, 2-56s and smaller, have to know this. If 1/4" inch brass rod bends, a 2-56 has to be like overcooked spaghetti.
All the best,
Bob
-
Bob,
Couple tips . . .
To reduce the power needed and the flex on your single point cuts:
1) Sharpen the tool. Your photo shows a tool sharpened with a pretty rough wheel. You need a razor edge and a min 7 degree negative rake for that brass. While it is not a necessity, but you could benefit from using some cutting fluid also.
2) increase the spindle speed . . . a lot . . . . I mean . . . . a LOT
3) I don't know how the wizards or the Gcode macros function, but you can reduce thepower required significantly by only cutting one side of the 'V', if that is doable with the wizard/macro.
For cutting those tiny threads on soft material, unless you are doing it for the pleasure and/or the challenge, you should consider just getting a die holder for your tail stock and cut your threads with a die . . . much easier and faster.
-
Hi, Simpson36,
Thanks for you inputs. I'll answer one at a time.
Bob,
Couple tips . . .
To reduce the power needed and the flex on your single point cuts:
1) Sharpen the tool. Your photo shows a tool sharpened with a pretty rough wheel. You need a razor edge and a min 7 degree negative rake for that brass. While it is not a necessity, but you could benefit from using some cutting fluid also.
The tool is a brazed carbide cutter (not that negates what you're saying), and that's the way it came. I didn't attempt to sharpen it, but have gotten some diamond polishing stones so that I can try. I do use cutting fluid (Tap Magic), but usually make a point to clean it up before photos.
2) increase the spindle speed . . . a lot . . . . I mean . . . . a LOT
That's where this all started, wondering whether or not my wimpy steppers were able to keep up with faster spindle speeds. They aren't. But I wanted to make sure I could thread slowly with light cuts so I didn't blow $500 on better steppers and drivers only to find it still didn't work. I have confidence I can get the more macho steppers and go faster now.
Having said that, I'm a hobbyist and if I my lathe takes 2 minutes to cut a thread rather than 30 seconds, I really don't care. A lathe doesn't seem very practical to me for things I can go get in the hardware store. If I need some 1/4-20 screws, I'll go buy them. I have some things that I will probably want to thread, but they're things I can't just go get, or get a tap and die for, like camera filter sizes. If I need to thread a portion of some other assembly I'm making I want to be sure I can do that. It isn't my main interest.
3) I don't know how the wizards or the Gcode macros function, but you can reduce thepower required significantly by only cutting one side of the 'V', if that is doable with the wizard/macro.
For cutting those tiny threads on soft material, unless you are doing it for the pleasure and/or the challenge, you should consider just getting a die holder for your tail stock and cut your threads with a die . . . much easier and faster.
My reference to something like an inch long 2-56 was for emphasis. I have seen the pieces I'm working on deflecting under cutter load and I figure I need to find a way to fix that in the long term. Some day I'll see it for real in a part I care about and want to make sure I can work around the bending.
All the best,
Bob
-
Hi Bob,
Just a few comments for what they are worth.
Carbide has it's place, but for the wimpy and punny I'll go with razor sharp cobalt tools anyday.
Now that you got it running, play around with it some and a 1/4-20 thread requires small depth of cut.
Doing small threads can be a challenge because there is not much room for error becuse of your machine or setup.
To help with the spring of small diameters you may want to make a small live center like the attached.
The tip is replaceable or a custom one can be made ( ground rod was used). The one i made has three small bearings in it. Stock was placed in chuck, the front piece turned true on the outside, drilled and reamed thru for drill rod removable tip, match marked reversed in the collet chuck, and bored for the od of bearings, the beariings and tail shaft pressed in.
It is rigid and turns true. Better than some of the ones you can buy.
Now the one model maker at the model show last year does threading over 300 tpi and makes his owne taps and has written some articles in magazines about it. Small stuff and makes a 0-80 look big!
RICH
-
Rich,
I need to get an internal threading tool, so where would I find the cobalt steel tools you refer to? Enco?
That live center is a neat project. Strange is at may seem, I sometimes forget I have these tools that can make other tools. As my wife says, "we can do _any_ thing". Well, anything that fits in the puny/wimpy work envelope. ;)
Bob
-
Bob,
Emco, Little Machine Shop, MSG, J&L Industrial supply.
Just a few places that come to mind.
For internal threads i like the boring bars made by Bokum. You can regrind them if your carefull and can find other manufactures which make similar.
RICH