Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Overloaded on July 22, 2008, 02:45:09 PM
-
:)
I am curious as to how Mach Turn is designed to operate when threading.
Here is one of many very informative topics with some different views of the process.
http://www.machsupport.com/forum/index.php/topic,6707.30.html
1. When the G76 sequence starts, does Mach just sample/average the RPM, then calculate the feedrate for Z and maintain that pulse train to the Z axis motor REGARDLESS of any fluctuation in the spindle speed ?
2. If so, is this calculation done at the beginning of each PASS, or just the once for the entire G76 cycle ?
3. If YES to 1 or 2, would it be true then that all Mach needs is a good clean true sampling of a ROCK STEADY RPM at the beginning, and sufficient power to maintain that RPM throughout the cycle ?
4.Does Index/Timing inputs, Single slot/Multi slot discs, or any combination thereof, ONLY serve the purpose of establishing the initial RPM input for Mach to calculate the Z feedrate, and serve absolutely NO function thereafter in the G76 cycle ? (other than maybe a Watchdog trip if extreme) Or can Mach actually change the Z feedrate during the pass accordingly ?
I have read where production machine DO follow the spindle and can cut "Progressive Pitch" threads, but there seems to differences of opinion on whether or not Mach cannot follow the spindle at all after the G76 starts.
I am attempting to maintain consistency on close tolerance threads and the spindle RPM fluctuation must be the culprit.
Which brings up:
5. I have an extra 1KW, 1.34HP ac Servo motor and drive. Can I do away with the VFD and run Step/Dir to the servo and get rock solid stable RPM?
(monitoring the following error with the drive)
To the best of my knowledge, these questions have not been definitively answered anywhere in the forum...however, I may have overlooked some while searching. ::)
Thanks,
rc
-
Here you go RC, Art posted this a day or so ago.
Hood
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. :-) )
-
Where in the heck was THAT posted ? ?? A day or so ago ? ? ?
Thanks,
rc
-
Unfortunately for us Art prefers the Yahoo group and that is where he posts all this wonderful info.
Hood
-
Holy CRAP....never been there.
Thanks, that pretty well sums it up for me.
so...how bout that servo spindle ? No advantage to that I guess.
Thanks Hood,
RC
-
Many advantages to the Servo on the spindle but at this point in time not as far as threading is concerned, hopefully the SS will make that a thing of the past and rigid tapping will be easily achieved.
Hood
-
wow...TWO forums to search now ::).....AND review the manuals..... :P
probably just as well save some time and just post questions...even if they HAVE been posted before. :-\
rc :)
-
Excellent topic.
"then the axis motion is slowed by 14.28% during the next rotation"
Will the amount of slow down be any restricted or limited to some percentage?
RICH
-
What I understand by that is the rotational time is calculated every revolution and the axis slowed or increased accordingly for the next revolution. No percentage restrictions at all, it will continue to speed or slow until the thread is completed.
Hood
Hood
-
Well everything looks like clear as water.
When I was test wizard threading I would like to have some more thin end turn like 0.05mm but not only in to the last turn. Can I edit the wizard G76 or maybe better write some threading in G33. Anybody hows have wrote som G33 (or if mach3 have any othe code) always better to se some code before any test.
Regards
Dan
-
Hi Dan,
I'm not familiar with G33...didn't see it in the Mach Turn manual.
I don't normally use the threading wizard, I prefer to set the parameters manually using the syntax found in the manual.
Here is a clip of the settings. The full description of each parameter is in the manual.
RC
-
Hood,
Thanks for the post on how threading cycle is supposed to work. I must have read the index part a 100 times.
I fooled around with my little lathe today. The index pulse was monitored using my multimeter ( has HZ capability ) allowing a comparison to the mach rpm readout before, during, and along the cut. The motor speed was set at 100 rpm / 1.67 HZ. so it was easy to monitor. A slow feed rate of 5 IPM. I use a single slotted disc, backlash compensation, and exact stop. The rpm didn't wander enough to mention when not cutting.
Since a 20 TPI is a stretch for the little Sherline the motor slows down. Now when it slowed down the mach dro never changed by by more than 2 rpm ( from a 100 to 98 ) but the measure index pulse reading at times went down to 94 rpm.
You could see the effect of motor slow down by the change in the width on the uncut surface . ( at this point you would think a botched thread, missed steps ) Towards the end of the thread cut the the feed rate display would change briefly to something different than initial feedrate.
Z returns for next cut, backlash implemented,rpm is back to 100.
During the next cut, visually watching the cutting ( with a mounted microscope ) you could see that the z feed rate is changed ( even though the feedrate indication is showing 5 ipm) since it's not following the bottom of the v in the thread of the last cut.
The cycles repeat until .....finished good thread!
I did this test and others not to question if the programed cycle worked as stated but rather to confirm my machine was doing what it was instructed to do. Sometimes it behaves like me and dosn't listen!
:)RICH
-
Good to know it works as its meant to. There is no way for me to test it as my spindle has over 20HP at 1000 RPM so not much is going to slow that down in a threading operation.
Hood
-
Just a bit more from the "Founding Fathers".
Hi Guys:
Having read the various experiences I think I can shed some light on the
matter. I havent decided how to
"fix " the trouble as yet. But I think I have ahandle on whats happening..
to explain , I have to go a bit deeper
than Id normally go. This sort of problem is hard to repair because each
person has their own theories on what is going on,
and often those theories are based on faulty logic of what exactly Mach3 is
doing internally. I think Im seeing a pattern though..
1) How mach3 times the spindle..
When feeding a index input to mach3, mach times how many interrupts it
takes from pulse to pulse. Knowing that the pulse
frequency of your machine is a known constant I use the formula:
RPM = 60 / (IntsPerRotation * (1/ ((double)Engine.PulseCount)));
This gives me the true spindle RPM based on your pulse count from the Diags
screen.. and the number of interrupts taken between spindle pulses. I
probably should have designed it on the actual CPU clocks taken between
Index inputs. The end result of the way its done means that if your diags
page shows a rock solid pulse frequency, as it does for most, the rpm
reading will also be accurate. BUT if the diags page shows a fluctuation on
the pulse count, the RPM will be in error by the % variation of the pulser
frequency.
2) How do we correct the feed during the thread. (assuming 25Khz for numbers
mentioned)
The system plans the motion as always in advance of the thread being cut,
the pulses are all lined up for output. If the number of interrupts between
index pulses stays the same as the premotion samples, then no correction is
made. ( Those that get perfect threads likely have no slowdown so no
correction is applied or have a rock stable pulse count on the diags). If
the index pulse time for the any rotation is found to be longer than the
sampled time ( say 600 interrupts per rotation is normal, and we now have
610 during the cut..) the system know knows that we put out 10 step slots
too much to the steppers or servos. So for the next rotation, we inject 10
waits states evenly though the single rotation so that 10 slot steps are
delayed by 40us each evenly spaced though the next rotation. This means at
the end of the second rotation we now are evenly matched in number of
rotations vs the number of total step slots produced. A step slot is not
usually a step itself. Again this requires a bit of an explanation. Mach 3
works on step time slots more than steps. The buffer hold in it 2 seconds of
motion, evenly divided to 40us slots. Actual motion steps may only occur
every 25th slot or so depenfing on speed. You can think of it as a buffer ot
4096 slots, but if the motor only has to move 100 steps in that time, then
though there are 4096 slots, only every 409.6 slots is a step put out.
Correction of the threading stretches the 4096 slots to be put out a bit
slower by injecting a wait state where the current slot is held until next
interrupt and then output resumes. The motor sees this as a very minor
jitter in time, and the total number of steps is correct. The buffer may
look like this for example before correction...
i = interrupt, S = Step
i,i,i,i,S,i,i,i,i,S,i,i,i,i,S ...ect..
The above is clocked out at interrupt rate. The disance between S's is a
function of acceleration and velocity. During a thread correction.. we'll
add a wait state.. so the buffer may look like this..
i,i,i,i,S,i,i,w,i,i,S,i,i,i,i,S,i,i,i,w,S..etc.
The spacing of the w's, ( wait states), is derived from a bresenham
divider and is very accurate as to how best to slow the precreated stream.
This has proven itself in many area's of mach3, so thats not where the error
must lie. these waits states, unless your traveling at top speed of the
motors have very little effect if any on the motor motion other than to slow
it. For each w state imposed, there may be up top 100 or more i states where
nothign happens anyway, so the induced jitter is less than 1% typically, and
thats a pretty safe spot. At most it creates a sligh "correction" sound in
the motors motion. I havent heard of anyone losing steps as a result, so as
a corrective action for spindle slowdown it does achive its proper end
effect as long as we dont have any of the problems below..
2) So wheres the error:
My thinking is that the error only shows on some machines due to 2
possabilities. First, that user with trouble may not have a solid pulse
number on the diags page. This can be caused by many things, interfering
processes or bad driver operation where it wont lock to speed. PRobably
unnoticable unless your threading as Mach3 tends to smooth the output train
enough that variations cuh as this only become critical in threading runs.
The second possability is a slighly varying index pulse in time.Ive seen
many sensors, ( my own included) that vause RPM variations due to being too
sensitive and varying in time from pulse to pulse. Adjusting senstivity
solved my own issue with that.
Bottom line.. the best performace will be if the diags shows a rock solid
pulse frequency, and the RPM shows as stable when your just running a
spindle and not threading.
I have to give some though as to if perhaps using the CPU clock rather
than counting interrupts woudl solve most of this, the CPU clock I can read
in nanoseconds time base, so if the pulseing engine is a bit erratic in
timing , then the cpu clock woudl self correct for that.. in the meantime,
check the pulse frequency on the diags..is it stable? if not, try shutting
off everythign in the startup of msconfig, even if your unaffected in other
situations. Threading is very suceptable to variations, and since my
computers tend to be rock solid in this, Im suspecting its why the variation
inthreadin is hard for me to track down..
Im really thinking that I need to option the "correction" algorithm so you
can turn it off to see if that stops the threads from destroying
themselves.. Ill talk to Brian about updating the application code to give
you a checkbox to turn off correction while I
think about a driver update to switch to actual nanosecond time base instead
of interrupt count time base. Being able to turn off correction, but leave
triggerign alone will IMO, probably fix up almost all problematic threads to
only show the effect of a
slowing spindle. Most have no slowing spindle during a thread, so the
floating pulse frequency causes the corection to hurt rather than help the
final product..
Let me know how your experience match the above explanation or not.. :-)
Thanks,
Art
-
If any of you are experiencing any discrepancies while threading, as I am, I strongly suggest that you follow this topic on the Yahoo forum.
http://groups.yahoo.com/group/mach1mach2cnc/message/96098
AND this:
http://groups.yahoo.com/group/mach1mach2cnc/message/96103
There's ONE guy there.... Art somebody ::)..... that really seems to know what he is talking about. ;)
RC 8)
-
RC
I would have thought that by now, about a week since your first post, that there would have been a lot of
users posting problems with threading or about threading. I gave up about 2 months ago on threading figuring I would waite for the SS to mature and went back to another program which allows electronic gearing ( use of an encoder along with a stepper). But I want to use MACH, plain and simple!
I started looking at the Yahoo posts, CNC zone, there's a lot out there. What can be frustrating is trying to filter out or find what Hood posted. So if you guys find relevant info please continue to post here. It will shorten the learning curve and and eliminate frustration for manny.
Understanding of how something works provides a good basis for solving individual problems. Why this thread is so good is that it starts putting in one place what I believe are key elements which allow you to analyze or look for what should be going on.
So you got me off my duff and I am now threading on the lathe. :) And it was fun!
Still not satisfied with the results but at least gaining valuable experience and will use provided insight to try some things in an progressive way.
PS: I now understand Art's comment saying "that threading is lot more complicated than someone may imagine".
RICH
-
Well Art has it fixed for you puny spindle motor guys :D
It will be available in the next release of Mach, not sure when that will be as its a biggie this time, loads of bug fixes from what I gather :)
Hood
-
Rich, what is not good about your threading? is it similar to the problems the guys on Yahoo were seeing?
Hood
-
Hood,:D :D :D :) :D :D :)
Rich,
I would have thought so too. I don't think there are quite as many Turners as there are Millers and Routers. The ones that do threading, probably have them big ol' hosses like Hoods or are just cutting a regular class 1 or 2 thread. Mine works beautifully for that...all day long if it had to.
It's the delicate closer tolerance stuff that I'm having problems with. 48 and 56 TPI in brass and 0-1.
Part of my problem is that I have a V belt from the motor to the spindle that is not perfect. It rides at varying depths in the pulleys and causes the index to wander 1 to 2, maybe 3 rpm. I made new pulleys that are dead true but cannot find a perfect V belt. If the new fix doesn't correct the threading, I will go to timing pulleys and a flat timing belt, probably will regardless.
Looks like the new release will be soon. (Get well quick Brian...that's what you get for taking time to eat) :D
RC :)
-
Hood,
I havn't done enough tests to put in perspective, yet........ I was doing some 1/4 - 40 & 10-32 x 1/2" long and looks like the first and last 1/3 of the thread are cut well but the mid 1/3 looks like more cutting is occuring one side and it looks like crap when magnified. I didn't check if there is any gain or loss of pitch. Using gummy Al dosn't help so will fool around with brass or some 1012L. I just scanned the Yahoo posts at work so got only a little flavor.
Need to look over the ones RC just posted.
Have a nice Gaertner toolroom microscope so I can measure things accuractely. Same goes for magnified pictures.
If you want me to try some stuff let me know. I'm in no hurry and have time . Will keep track of things and can post how things turn out.
The machine is limited for threading, but in a way, it allows for finding stuff that you would not otherwise come across.
RICH
-
FROM ART'S POST
"There is an LED on the diags, can you tell me if its staying on during the thread, I fear Mach3 may be killing it as soon
as it starts.. This may be a side effect of the pause removal we fixed earlier on in the year for the pause in drill cycles."
"If it goes out during the pass or rigth away when the pass starts, then we
have found the bug.. if not, "
------------------------------------------------------------------------------------------------------------------------------------------------------------
I just checked this out / dry run some threading. The trigger will flash green, then threading flashs green , but as soon as the threading move starts the thread light indicator in diags on my machine goes out. This repeats for each cycle when the threading starts.
Using MACH 3 R3.041
Hmmm! Maybe what Taut taut he saw he only taut he saw during his other test! ??? Tomorrows another day
MODIFIED 7/28/08 PLEASE SEE ANOTHER POST MADE BY ME TODAY 7/28/08.
:)RICH
-
If it looks like steps down the back edge of the thread then maybe you have too much of an infeed angle.
Hood
-
It steps down the front side / tail stock side of the thread. Infeed angle used is 29.5 degrees for a sharp 60 deg pointed thread tool. This may sound dumb, but i assumed that the infeed of the x was perpendicular to the od of the
piece and not an x-z move . I know some programs do a progrssive cut to the front side of the thread.
Can you clarify?
PS: One of the tests i did was to set depth to .0001" and let it run thru a lot of passes, maybe 60 or more then stop
the threading, reposition back to original start point, then redo the threading. ( piece not removed from chuck
and motor left running ). Want to play around with this some and inspect the cutting marks. But I know what will
be seen can be influenced by a number of things, so need to think more about it.
RICH
-
If you are using the wizard then its a G76 which I think is a flank infeed thread, try setting the infeed to 15 dgerees and see how that goes.
Hood
-
Hey Rich,
If you get a chance to, maybe try this test also as I did. Set up a thread, say 32 tpi, cut it in 6 or so passes and set 10 or 20 spring passes. The spring cuts, after 1 or 2 should stop cutting..but here it varies. Cutting the front, the flank, none...very sporatic.
RC
-
Hi all,
This may be of interest to you or someone in the future. It sums up some testing i did on the lathe today using the diag screen.
RICH
MODIFIED 8/3/08 - ADDED THE FOLLOWING:
The attachment will be modified in the future. If you have been following the Yahoo threads you know that there are discussions on threading
going on. Art informed me that the threading LED should always be on. In my attachment that is not the case, so comment #1 in the attachment is probably wrong, but then, that is what was found during my test. So....just a heads up until additional info is recieved.
RICH
-
Better than info are results. Attachment at 12 to 15X shows 20-40-80 threads which I just cut.
Will fool around some more and do some measuring.
RICH
-
Hi All,
Still fooling around cutting threads. Dimensional results are good; Pitch diameters are .001 to .003 over the length of the
thread, the pitch cut for all practical purposes is right on ( hard to measure at the bottom of the v but stays witin .001),
using a sharp 60 deg tool and the v as cut is about 62 deg when done radialy. Will try flank cutting some and see how things turn out. Will be interesting to see how the electronic gearing compensates when the spindle speed really drops.
So far with minor drops, a few rpm, things seem good at the practical level.
Now if the fix comes out along with the SS also providing threading and backlash compensation life will be really good.
RICH
-
What are you using as the thread cycle, G32 or G76? I use G76 with an infeed of 15 degrees and dont have any problems at all, just finished a load of 30 pullstuds the last day and all threads were perfect, then again the spindle motor doesnt slow down so Mach doesnt have to do much in the way of calcs :)
Hood
-
Using the G76. Art was kind enough to send me a Mach test file which he recently did. I assume the next release of Mach will include the fixes. When monitoring in diag screen, the threading box should turn green and STAY ON for every thread cycle. Mine was not doing that as shown by the test. So the comments I made are actualy incorrect and that's the reason the post was modified adding a clarification.
I needed to confirm that my lathe backlash setting was correct, etc, as it dosn't take much for a thread to get screwed up. With the machine mechanics confirmed, a working program, and the knowledge that threads can made to tolerance
on my punny lathe, I can now play and see effects of the program.
Will deliberately do things like heavy cuts, radial & flanked cutting, testing the limits of a small machine. The electronic
gearing will allow for around a 50% rpm reduction from started rpm. Dry running showed it's working but don't know
the quality the threading that will be produced. This may sound like a waste of time to some but it's darn good practical
experience on my part using a CNC punny lathe.
RICH
-
Thanks for the info Richm good to know the threading fix that Art did has sorted things out.
If you were doing a G76 what infeed angle did you have?
Hood
-
Hood,
0 for radial cutting so will start with 29.5 for flank cutting.
BTW, not trying to be a purist on the measurements, info given is a whole lot better than the nut is loose or tight and for most folks they coudn't even measure the angle of the cut accurately. So I'm happy what is being cut. Will try 15, 30, 45 ( just for kicks ) on flank cutting to see how the threads look for comparison. Will a write up on threading ( good grief don't want to do treatise on it) but thoughts are for the
newbie.
RICH
-
yep look forward to it.
Hood
-
Hi All,
The attached shows a comparison of some thread cutting tests. One is a radial cut and three a flank cut. All were cut using G76 with I=0, 45, 15, 29.5. So a few questions.........
1.Can you name the I used from top to bottom?
2.Which did the test nut fit on?
Here's a hint, all cut using the same tool and settings.
:)RICH
-
I would say the third down is the only half decent one and even it doesnt look perfect, could just be because the crest has not been cut so I presume you are not using a full profile insert.
Hood
-
Oh and as far as the test nut fitting on, depends how good the testnut was ;)
If its like some of the nuts that are available, ie some of the junk ones that come in from China (not all are junk BTW ) then its likely it fitted all. If the crest was machined on the third down then I would say that is the best thread but without seeing them in person its hard to tell from a photo.
Hood
-
Hood,
The picture was a tough one to take and the lighting was crucial as reflections disfigure the thread form.
I was curious as to how the actual cutting would turn out since I never did any flank cutting. The cutting tool was just a
sharp 60 deg. Don't have any of those fancy forming full or partial ones.
From top to bottom with comments:
45 deg flank cut - the flank side is smooth and at 30 deg and you can see the 45 deg ragged cut done on the back side
of the thread. But it did do a "avg" 45 deg and you can see the steps. So as expected no nut will go on
to that thread.
I think this one will really show just how well a lathe will work. Should backlash, timing, etc. be sligtly
off it will show up on the back side. A .001 step looks like a mountains ridge when magnified.
0 deg radial cut - the nut fit just fine. 1000 grit paper was used to clean the top edge burrs. It's probably the cleanest cut
thread of them all.
29.5 deg flank cut - The nut fit rather snugly. I didn't clean it up any and there was a little bit of belly on the flank side.
15 deg flank cut- The nut didn't fit on this one and you can see the difference in the thead form ( 45 deg total instead of
60 deg ).
I made the test nut by drilling and tapping a piece of oct shaped rod and checked it with go / no thread gage.
Hate to make generailized statements, but would quess that if a your lathe can't provide a good radialy cut thread then
you may never get a good flank cut one.
Next test should be interesting to see what happens when the spindle slows down some 25 to 50%.
One thing thats nice with CNC is that I can also duplicate a grappy thread!
RICH