Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Cartierusm on October 22, 2010, 09:03:57 PM
-
OK I think I've posted this before years ago and don't think I got a response and can't find the post.
Anyway, I'm trying to thread some 304 Stainless on my Converted 9x20 Lathe, the piece is 4 1/2" in Diameter External Threads 16 TPI at 1000 RPM with a 16 TPI Thread Insert. What happens is when it's cutting it's losing some RPMs and I know the RPM and strength of the motor is the root problem I need to solve BUT what Mach does after the second or third pass cutting is it knows the RPMs are slowing, obviously, but instead of stopping or self correcting it starts to cut at a taper and ruins the threads. Why does it do this, why would it move X inward as it's cutting. I could see it moving X for the positive to make the cut more shallow thereby making the RPM stabilize, but CUT A TAPER IN??? Please help.
-
What version of Mach are you using?
I will remark that if is not 3.042.032 and above then you need to upgrade.
I would suggest you have a look at the Threading on The Lathe write-up as it will give you insight into how the threading accounts for slowing of the spindle RPM........ the range it may adjust for, what you can and cannot expect from the threading cycle. Also a whole lot of other threading related stuff.
Your threading will only be as good as your Lathe "System". I may also suggest that you just do a rough HP requirement based on the insert and
the cut depths, the inserts, rpm, etc. I suggest you also explore using the different methods of threading. Also do some of the tests.
I don't know what type axis motors your using, in my case they are steppers, so i always have the wizard check / calculate the number of passes which
will also display the IPM feedarate. I adjust the spindle rpm accordingly so i am at the max power level for the steppers ( ie; below the max axis velocity as it relates
to their torque ).
SS will work harder and what was easy at the first or second pass may require 2 or 3x the power to do the work hardened cut. You may be dropping below what Mach can do in recovering from a problem thread cycle ........( I have actually made the spindle briefly come to a stop and was able to recover).
BTW, on my 6" x 24" Atlas / 1/2 hp motor / 53 RPM / single 60 deg insert / modified 15 deg flank ( i think) i was able to cut a 3 1/2" x 8 x 2" long thread in steel. ( I will remark that towards the end of the threading i thought i was going to break the carriage or tool post and made 2 or 3 spring passes)
I will say this, the threading cycle is solid if the machines system is appropriate for the task.
RICH
-
Thanks. I'm using 3.042 from about a year or so ago, maybe a little newer. I switched out the motor to my old one and it seems to be working fine.
I've been cutting threads with this machine in all types of material for years and years, so I know there's nothing wrong with the machine. So my question stills stand, when the RPMs drop below what mach thinks is acceptable WHY does it start to cut a taper?
-
Cartierusm,
Simple question ......maybe be a long winded reply......the answer is not simple and threading is complex.
First just a few question's for my understanding:
-What version of 3.024.??? is it .032 or .033?
-Using exact stop and not CV?
-How much of a change in your rpm?
-Using a VFD?
-Using a single index?
-Spindle speed averaging checked / being used?
- Describe what you mean by taper.
Is the taper cutting over the complete threading cycle or are we talking about when the spindle slowed down?
How much of a taper?
What end is smaller the beginning of the thread or the end?
It is difficult to watch what is really happening when threading at say 60 ipm. I will comment that one needs to
isolate each controller reaction to a slowed down rpm in the threading cycle. There is the overall threading "picture"
and the individual parts that make up the picture. So as i continue in my reply keep that in mind as there is a lot going on.
When the rpm's drop below what mach thinks is acceptable WHY does it start to cut a taper?
Apparently a taper ( carefull as to what you mean by taper) will be cut if say the rpm's drop, lets say 30%, and then rpm goes
back up during that cycle. As a result of the slow down, the machine must cut a varing thread pitch, not a taper over that time period.
The "relative" thread root for that cycle would ideally remain the same since the X axis location by code is the same / never changed
code wise or manipulated by Mach. Because the chip curl changed, that would create a tapered cut and you can add cutter / machine
deflection to that cut taper. Just one part of the picture.........
Mach monitors the rpm and changes the NEXT thread cycle based on how much the rpm changed. All the sampled rpm's over the cycle time
period will provide an adjusted rpm on which to base the next feedrate. That feedrate or other feedrates over all the
thread cycles should provide an a properly cut thread cut. The big picture.......
Hope this simplified reply is an appropriate answer to your question,
RICH
-
Am I missing something here? Stainless steel, 4.5" diameter, and *1000* RPM?? That is WAAAAAAAY too fast, like by 10X or more!
Regards,
Ray L.
-
Rich is the threading expert when using the PP but I am almost certain this was an issue before Art fixed the Driver up with Rich's help, upgrade and try again would be my advice.
As for 4.5inch dia 304 threading at 1000rpm, as Ray says you are being a bit optimistic. If using carbide inserts I would be running around about the 200 to 250rpm mark.
Hood
-
Rich, thanks for the help.
Using Version 3.042.020
Using CV
can't really tell about how much RPM loss but looks like about 30 RPM
Using VFD
Single Index
Don't know what spindle speed averaging checked is, can guess what it is but don't know where to find that option or if it should be used.
As far as the taper. Let's say I'm making .002 depth of cut per pass so it doesn't bog down the motor, I think Mach may set it's own depth of cut anyway even though this is what I have it set for in the threading wizards setting page, because it doesn't take that long to thread as it sounds with a .002" depth of cut per pass. Anyway, let's say I'm making 16 TPI threads on 4" stock. First pass will be 3.996", next pass will be 3.992, then 3.988, by this time (with the old motor) it will start to loose RPMs and instead of the next pass being at a depth of 3.984", it will start at 3.984" and go down to something like 3.9645" tapering down the run and continue if I let it. I can't really tell what the exact end depth is on X as I'm just looking at the DRO on Mach and it's moving counting down as it moves. The beginning of the thread is larger in diameter and the back end is smaller. It happens after it makes a normal pass where it starts to loose RPMs, then the next pass is tapered and it continues.
@ Himy, I can't go slower even geared down motor with a VFD if I go to 100 RPM the motor will be very weak. I assume Himy, that you have a CNC lathe that you can actually gear down to 100 RPM? I usually don't have a problem at 500-700 RPM. I was trying 1000 RPM because my motor lowered to 500 RPM was losing RPMS during threading, but last night I changed to my 2 HP motor with gearing so the highest RPM I can get is 742 rpm, so that will give me full HP at that RPM.
@ Hood, thanks also, I'll try lower speed with the motor, with the old motor back in, if it continues to work I'll put a different pulley on it to make it's top speed 350 RPM or so.
-
@ Himy, I can't go slower even geared down motor with a VFD if I go to 100 RPM the motor will be very weak. I assume Himy, that you have a CNC lathe that you can actually gear down to 100 RPM? I usually don't have a problem at 500-700 RPM. I was trying 1000 RPM because my motor lowered to 500 RPM was losing RPMS during threading, but last night I changed to my 2 HP motor with gearing so the highest RPM I can get is 742 rpm, so that will give me full HP at that RPM.
RPM should be determined by recommended SFPM for the specific tool being used, and the material being cut, whether it's turning or milling. Excessively high RPM will destroy the tool very quickly, and with stainless can easily lead to work-hardening, which will make the material near impossible to cut. Most carbide tools recommend SFPM in the 1000-3000 range, but you're up at around 15,000. You may get away with it, but it'll be really brutal on the tool.
Regards,
Ray L.
-
I have never been keen on VFD's, they are great for varying the speed within a range but as you have found when you get down in revs they are not much use. Any commercial machines I have seen that use VFDs have much larger motors on them than would be expected for the size of the machine as that way they still have power in reserve for the lower RPMs.
My lathe originally had an 11KW induction motor and the speeds were changed in a gearbox which operated by electro magnetic clutches. It would have been a good candidate for a VFD as I could have varied within each range to give different speeds but instead I got my hands on a big AC servo which allows me to run from zero RPM up with no loss of torque.
You probably dont have either of these options so your best bet would be to fit more pulleys for different speeds ranges, problem would be is that you would need to manually change them.
Hood
-
@Ray, I used a different pulley and was able to thread at 200 RPM and I only lost 1 RPM, pretty good.
@Hood, what I ended up doing was ordering an actual Adjustable Motor Base which will allow me to easily change pulleys and belts without too much of a hassle. So by the time I'm dong i should be able to switch them out pretty easy without having to sacrifice when threading.
What I'm threading is some Sch.80 304 Stainless Pipe to 16 TPI. What does everyone suggest as a good cut depth for this material running at 200 RPM. I've tried .002 and .003 cut depth per pass, as you know that's total. So from 4" next cut would be 3.997" and so on. The only reason I'm asking is toward the end of the run, the last 7 or so passes it starts to get crunchy sounding and leaves little burrs. Then I have to rerun the cycle to clean it up. So I'm wondering if that's a factor of TOO little cut depth so it's scrapping instead of shearing? or too fast or little speed? Suggestions?
-
For stainless the secret is to cut aggressively to avoid work hardening, for 16tpi you would be looking to do a thread in 6 to 10 passes. Most of my lathe work is 316 stainless and I would tend to run nearer the six passes for that thread. Problem is you also have to work within the constraints of your machine, mine is fairly large so I dont have an issue but if you are low on HP and rigidity then you may have to aim for the higher end of the passes.
If I can find one of the threading catalogues I will scan and attach the numbers they give for pitch and passes, if you want.
Are you using carbide inserted tooling? If yes are you using full profile or partial profile tips?
Hood
-
Thanks Hood.
I use carbide insert tooling and have both full profile and partial profile bits, but when doing 16 or 32 I tend to use the full profile.
WOW that's very few passes, I'll go try it and see what I come up with.
-
As said it will depend on the power and rigidity of your lathe but being aggressive with stainless is the secret if you can get away with it.
Heres a couple of scans out of one of the tooling catalogues, its for Korloy inserts but most will be around about the same.
Hood
-
Afraid the surface speed is in m/min but should be easy enough for you to convert, will look see if I have some catalogues with the old fashioned units you Americans use ;D
Hood
-
Cartierisum,
Thanks for the info in reply #6. I'll comment a little more later. One to two years have passed since threading was addressed and i wanted to review some of my notes rather than relying on memory. I only have 500 pages of notes....... ;)
Using Version 3.042.020
Upgrade to at least version 3.042.32 ( there are numerous problems that were fixed from .020 on and you are experiencing some of them )
Using CV
Use exact stop as CV will affect how the pullout from the thread is accomplished.
See the note at the top of page 34 in Threading on The Lathe write-up.
Can't really tell about how much RPM loss but looks like about 30 RPM
If you watched the rpm DRO you would have a better feel for the drop, 30/1000=.03 or 3%,
So threading compensation shouldn't be a problem. 10 to 25% could be
Even 3% will affect the thread pitch though.
Using VFDI don't use a VFD and if memory is correct you should manualy set it to a fixed rpm. If the VFD is changing the RPM, Mach is planning the next pass,
they could be fighting each other, thus screwing up the compensation ( based on rpn reading) which will affect feedrate, which affect the thread.
Single IndexGood ........timing not longer works and should not be enabled.
more when i return in a little bit,
RICH
-
Cartesium,
If you download this programme it may be of use, I used the metric version a while back and found it handy. You can go through all the stages and at the end if you click manual it will give you a depth per pass etc. Again its all dependant on machinery available but it gives you a good starting point.
http://www.secotools.com/CorpWeb/Service_Support/cutting_data_calculators/Threadturningwizard_inch.exe
Hood
-
Thanks a lot for the help!!!
I'll look at the program and pages you scanned now.
@Hood, I went ahead and threaded at 200 RPM 16 TPI with 8 passes and it came out fine, thanks. The only thing is the last 2 or 3 passes vibrated the machine a ton. I guess it could be one of two things, either my bit is not exactly on center or that's when it's topping the thread. I persisted and reran the program and it did fine. Still a tiny bit of vibration at the end of the run, mind you I do 6 spring passes to clean it up so it's probably just rubbing.
Two important questions, will upgrading to the newer Mach mess up any settings, macros or VB buttons I run? Also what will exact stop do for regular lathe work when not threading, do I keep exact stop on all the time? Thanks again.
-
SPINDLE SPEED AVERAGING
Mach3 can keep a running average of the last 8 revolutions. At the start of any pass it either uses the
average OR the last measured time. Every thread starts with an unloaded spindle, the 8 rev average is
typically unloaded average. ( unless your turning very slowly on the spindle and very unlikely it's less
than 8 turns in the air prior to a thread pass)
So the correction code is all that controls speed during the cut to take into account the spindle slowdown
caused by hitting a hard spot or an average slowdown due to harder material.
The averaging is discounted for correction, it cares only about the real last index to index time,
and it compares that to the locked in average or locked in last rev just prior to the thread pass starting.
Rule of thumb is 3 to 5 diameters times total thread depth for unloaded spindle travel of the Z axis.
I use and would recommend you use spindle speed averaging. It helps if there is a "out of rage / fluke / high" rpm
included in the averaging. You then get a more refined feedrate. One "fluke" may not influence as much as you
would think.
Some of my words but mostly Art's, ;)
RICH
-
Where do I enable spindle speed averaging?
-
Where do I enable spindle speed averaging?
Ports and Pins, Spindle Setup.
Hood
-
Thanks a lot for the help!!!
I'll look at the program and pages you scanned now.
@Hood, I went ahead and threaded at 200 RPM 16 TPI with 8 passes and it came out fine, thanks. The only thing is the last 2 or 3 passes vibrated the machine a ton. I guess it could be one of two things, either my bit is not exactly on center or that's when it's topping the thread. I persisted and reran the program and it did fine. Still a tiny bit of vibration at the end of the run, mind you I do 6 spring passes to clean it up so it's probably just rubbing.
Two important questions, will upgrading to the newer Mach mess up any settings, macros or VB buttons I run? Also what will exact stop do for regular lathe work when not threading, do I keep exact stop on all the time? Thanks again.
You may need to upp the passes a bit but personally I would cut down on the springs, I normally only do one but again its all dependant on your machinery so messing around with things is really the only way to find out what is best for you.
Shouldnt have any probs with upgrading, just make sure you have any custom things backed up first just in case the worst happens.
Hood
-
OK, I upgraded to the 3.042.040 version and everything is the same. I already had Spindle Speed Averaging on.
So the only thing I need to know do I keep exact stop on while doing regular lathe stuff?
-
I tend to work in exact stop on my lathe but as I have fairly fast acceleration and the lathe is a big lump it works fine. Try both G61 and G64 and see which works best for you.
Hood
-
OK, so I know there is an exact stop and CV mode in general settings, but are you saying I should change it in Gcode?
-
BTW wondering what a 9x20 lathe is as I think you call things out differently there. I know the 20 is the between centres but is the 9 centre height or turning Dia? Just trying to get an idea of the size of lathe.
Hood
-
turning diameter, may be small but I've made some very complex precision parts over the years.
-
Yes you can change in code, have a G61 and all code after that point will be exact stop until that is you call a G64 which will put things back to CV.
If your default in General Config is CV it will start up that way next time you start Mach.
Hood
-
OK great, now I just have to setup my motor plate so I can pulleys. Thanks a lot.
-
turning diameter, may be small but I've made some very complex precision parts over the years.
My first ever lathe was a drummond M type and I did some crazy huge stuff that should never have been attempted ;D Thing is you have to work with what you have and if you mess around you can usually find a way to make things work..
Hood
-
Sounds like your on a roll......
Have fun,
BTW, i will probably move this thread over to the problems threading on the lathe thread.
Will keep it here until your happy all is going well.
RICH
-
Thanks. Yeah over the years I've done some crazy stuff with my lathe, but it all works out in the end.
BTW Giants GOING TO THE WORLD SERIES>>>>>> SAWEEET...I'm in SF if you didn't know.
-
OK, so that didn't work. I tried going to V3.042.040 and the RPMs only said 7 or a low number when the lathe was on, so I went back to 3.042.020. Is there a different version where the threading problem was fixed but that's not .040?
I tried a whole host of other things trying to get this thing threading correctly. I tried 100 RPM, 200 RPM and 400 RPMs and different DOC. The BIGGEST difference was using thread cutting oil, before I was using the Cool Mist solution in a heavy spray.
So in the end I got one good test thread now I'm going to try to reproduce it. My specs were 16 TIP 4.475" OD down to 4.3984, .005 DOC, 400 RPM and brushing on the thread cutting oil. Now hopefully that works with a REAL piece.
Oh, I also am using a carbide insert that's coated, before the ones I used were uncoated.
-
Did you try a different setting for the Index Debounce in 3.042.020?
You should be able to get most other versions on the FTP site, you will find its link on the downloads page.
Hood
-
oh another thing, not sure how your spindle is controlled, if not via Mach you need to have at least a M3 to tell Mach your spndle is started before it will look for the RPM and I think you may also need to enable the relay for spindle on spindle setup, even if you are not using one.
Hood
-
Mach controls the spindle through a board from cnc4pc and a vfd. I didn't mess with the debounce, didn't know I needed to. What version do you recommend?
-
Normally you dont need to mess with the Index Debounce but maybe with the threading changes it has affected things and you may need to. Note it is the Index Debounce I am talking about and not the Debounce Interval.
I am afraid I cant recommend any version for threading except to say one from 3.042.32 or newer. Reason I cant say is I use the SmoothStepper so threading is not an issue for me, then again threading was never an issue even with the earlier revisions, probably due to plenty of HP at the spindle.
Hood
-
Is there a different version where the threading problem was fixed but that's not .040?
Prior to version .032 threading was not done in real time so to speak. There also was the problem of a goofy X axis move and also loss of snyc with the
spindle index caused by a driver problem such that you could end up having the Z axis trash the threads. The threading code was then
redone and tightened up to provide for improved pitch control. The compensation ( spindle slow down ) was adjusted during the revisions.
You may epxerince problems if there is a slow down say 15 to 25%, i know you can't have a complete spindle stop anymore in the later versions.
A lot more went on but that is the gest of it.
You don't want to go back to any version before .032. ;)
I would strongly suggest that you first do a search for all versions of MACH.sys and Mach exe Sometimes old versions are reinstalled.
Also go into Windows device manager and delete the driver. To reinstall the driver you need only run the driver test and the driver test you run should be from
.032 or whatever later version you installed.
INDEX DEBOUNCE will affect the sensitivity of the index signal. IT basically is how many interrupt periods the signal must be present, or not present before
a change is rpm is actually sensed. SO if set to 2 for example, when the index appears it will be ignored for 2 periods to make sure it isn't noise.
Same with when it disappears. Setting debounce too high will make the index go away altogether, setting it at zero will mean it reads whatever is sensed, even
noise. If the reading time is too short you may not get a reading at higher rpms.
Practicaly speaking, if no rpm showing in DRO after some rpm, lower the debounce. Try 0 , 10, and see what happens. You should have full rpm reading with
a good index signal.
You have a VFD, then manualy set it at a desired rpm, and not have it controlled. You should see that rpm in in the DRO. If the VFD is changing the rpm
and mach is compensating before the thread cycle they could be fighting each other and not sure what you will end up with.
Do the tests described in the write-up, ie; spindle check out and do a scribe test. If you can't scribe an accurate line around the cyclinder then you will never
thread properly. The spindle and the motor is unloaded when you do that. ;)
Simply said, the better the rpm reading from the index with less change to displayed rpm the more accurate the threading will be. If you can scibe it accurately,
and then in practice it dosen't work, it could be a number of things related to motor settings and machining practice, etc.
Hope this helps,
RICH
-
Thanks both of you for the help...I HAVE SUCCESS!!
Nothing was wrong with my setup, but when my spindle slowed down I got that taper thing happening which is what started this whole thing then I was having problems with the stainless.
What I did today was upgrade to V.032 and I threaded 4 perfect parts.
What, I think, made all the difference was using an insert that was TiN coated and using actual Thread Cutting Oil. The difference was amazing.
First I cut a 16 TPI thread 4.475" to 4.3984" .005" DOC 400 RPM 1 Spring Pass, that came out good but wasn't nearly deep enough. I'm using the same parameters as before, maybe it's the new version, doesn't matter it cut fine. Then I redid the threading going deeper this time to 4.38" .01 DOC. Still that wasn't deep enough so I went to 4.37" .01" DOC and that was perfect. Absolutely beautiful crown. I had to brush on, heavily, the Thread Cutting Oil during the entire process and got lots of smoke. But it worked and I got 4 perfect parts.
Again, thanks for all the help.
-
One can say your now on thread ............ ;)
Glad it's working,
RICH
-
thanks.
-
What is interesting here is Cartierusm stated no spindle speed with Vn .40, just 7rpm, that is exactly what I got. When Vn.32 was tried looks like it was sucessful.
I`ve tried vn.20 and spindle speed is ok, vn.40 no spindle speed,no matter what the debounce or M3. I now need to try V.32, but I`m 6000miles from my workshop at the moment so that will have to wait! Anyone got spindle speed with Vn.40 and parallel port? Can you share your relevant "Turn" settings please!
Thanks, Woody.
-
Hello,
a little bit older, but actual: I have updated from 042.020 to Vn.043.022. Everything o.k. but no Spindle Speed?
I have two LPTs, Pokeys, all o.k.- but no Spindle Speed at the Display. "Downdate" to 042.032 was not sucessful, same failure.
What the failure?
Greetings from Germany,
Tom
-
Are you telling Mach your spindle has started by issuing a m3 or m4?
Hood
-
Yes, but nothing...
Greetings, Tom
-
Can you attach your xml andI will see if I can find a problem.
Hood
-
Here comes...
Tom
-
Go to config menu then Ports and Pins then Spindle Setup and take the tich out of the Disable Spindle relays box. Doesnt matter if you dont have anything assigned for the outputs.
Hood
-
Yeah,
hier comes the speed. Many thanks!
But: If I turn off the speed, even when turned off is still a low speed (continous) in the display ... Is there also a change?
Greetings, Tom
-
Did you tell Mach the spindle was stopped by calling a M5 or pressing the spindle button?
Hood
-
No,
The control of the Spindle via VFC is manual. That was until now correctly ...
Greetings, Tom
-
Sorry Tom, not quite sure what you are meaning, is it all fine now?
Hood
-
Hello Hood,
well almost, I would say.
I turn on the frequency controller by hand. While running, the correct speed is displayed, but when i stop the spindle, run out of the spindle shows the last value to slow even at standstill. I hope you understand what I mean, my English is a little rusty. But Threading is always o.k. Only the continued displayed low Spindle Speed, for exampel 125 1/min is an irritation...at standstill.
Greetings, Tom
-
Did you tell Mach the spindle was stopped by calling M5 in code or MDI or by pressing the spindle button on the screen?
Hood
-
That makes no difference.
Tom
-
Can you attach your xml please and I will see if I can replicate it
Hood
-
Here Comes (after updating on last Rev)
Tom
-
Tom I am just simulating here with the index pulse but if I command a spindle speed or press the spindle button the S True DRO shows the value equal to the pulses I am simulating. When I stop the spindle or command a M5 the S True DRO returns to zero, so afraid I do not know why it does not do that for you.
Only thing I can think of is you are meaning the commanded spindle speed DRO is staying at the last commanded speed. If that is what you mean then that is normal and I think it has always been that way. If you want that to zero then you could alter the M5 macro to zero it.
Hood
-
Hello Hood,
at the DRO is the latest average of the last spindle rotation bevore stopping. You realize well, if the spindle rotates slowly by hand, changes the DRO accordingly, but never returns back to 0 at stopping.
It shows, as the DRO ist "waiting" on the next Index Impulse.
Not Nice, but threading works.
Greetings, Tom
-
I dont know what to suggest, the DRO goes to zero for me (with your xml) if I tell Mach the spindle has switched off, ie press the button on screen to turn off, have code call a M5 or call a M5 from MDI.
Hood
-
Toms,
I would suggest you create a new xml.
I couldn't get my spindle rpm to display in the DRO no matter what was tried with your xml from reply #55.
RICH