Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: fast89 on January 19, 2013, 08:03:18 PM
-
Jut got my clausing 12x36 up and running. Using machmotion breakout board and teco ac servo drives and a homemade tool turret. Machmotion does not support threading with their apollo I breakout board. I figured it was just a timing issue. I can cut a thread and it looks beautiful and the tool starts exactly the same on every pass. i mean the thread looks great. the problem is that the pitch is off. If i program a 20tpi, if i hold a tap up to it, the pitch is off considerably. My rpm is stable at 310 and drops to 308 for the first two or three passes then it is stable at 310 again. If i cut male and female threads , they fit good, so it is not a consistency issue. I messed with the debounce with no luck. i don't think it is the problem. I have spindle speed averaging checked. i also double checked the steps per for z axis. Anyone else have a similar problem? I'm running out of ideas.
-
Is the Apollo not just a breakout board? ie you use the computers parallel port.
If so then it will do threading as Mach controls it.
Are your axis moves correct, in other words if you command a move does it move that amount exactly?
Do you have a licence for Mach as threading doesnt work in demo mode.
Hood
-
Hood,
Thanks for the quick reply.I do have a license. The Apollo I has two parallel port inputs. The axis have been accurate, I've run a few jobs on it. It threads great, but the pitch is off.
-
Does the Apollow use a plugin? If not then it would seem it is just a breakout board and thus threading should not be a problem.
If you attach your xml I will have a look.
Hood
-
What version of Mach are you using?
Are you using a VFD?
What are you using to generate the threading code? ie; threading wizard, G76,?
Suggest you do a scribe test. Is the pitch correct for the scribe test?
RICH
-
I'm using version R3.043.022. Using a Vfd with a 5hp 1750 motor driven driving spindle 1-1. I am using the wizard and it is outputting g76. I did try it with g32 also and same difference. It is working great, just doesn't have the .050 pitch i specified. Looking under magnification, the pitch is smaller than .050" My rpm drops from 310 to 309 fir the first few cuts then it stays at 310 fro the remainder of the cuts.
-
Here is a thread i cut this morning. The tips of the threads are the original stock. You can see it picked up the thread on every pass. Just not making the right pitch.
-
Not seeing anything wrong in the xml regards threading, you seem to have that all set correctly.
Can you confirm your steps per unit for Z are correct, ie encoder count, pitch of screw (is it a ballscrew?) and gearing between motor and screw? Does your servo drive have any electronic gearing set?
Do you have a hand held tach you could use to compare spindle RPM to displayed RPM?
Hood
-
The servo is directly coupled to the ballscrew with a zero backlash coupling. The drive does have gearing and encoder gearing. Mach is set for 5000 steps per inch with the right gearing in the drive. I can jog it .01" and get exactly that on an indicator. I checked that last night before the wine started flowing. . I opened the turn diagnostics wizard and watched that while it was threading. The rpm was within 1rpm of programmed speed and actual speed displayed and it never showed a missed timing signal.???????
-
Disable turn diagnostics wizard, it is of no use except for the versions it was being used in to find problems, yours is not one and really it should be removed as it may cause issues.
Not sure if you had it enabled in previous tests or not?
Cant think what to suggest if the rpm is indeed being reported properly, the Z motion is accurate then all should be fine.
Hood
-
If you're confident the Z-axis is accurate, the only thing that can be of is the spindle speed.
How confident are you that the spindle speed is correct?
-
where is the spindle sensor
-
Slotted disc is on the back of the headstock on the spindle shaft with an optical sensor thru the c3 board then to the breakout board. I'm going to borrow an optical tach later today and double check it. I just did some more testing and for a 20tpi it was off by .0008" per tooth. I changed the pitch on the g76 line and it came out good. But i can't do this for every thread. I tried a 13tpi to see if it had the same inaccuracy and it did not, it was out further, maybe .001-.0013 per tooth.
-
Can you load a mill screenset and tell me what time in int and frequency say on diagnostics page. You will then have to go back to the lathe screenset.
Hood
-
Hood,
I use a modified mill screenset. I never liked the lathe multiple screen setup. Time in is unstable , bounces around 4.0-4.3 with intermittent blips to 8.1. pulse frequency is at 72665. I have this lathe running on a new very fast 3.2ghz pc with a solid state hard drive. I have Mach set to 75khz.
-
Agreed on the screenset, never used the standard one myself.
I had seen in your xml your kernel was 75KHz and that was why I was wondering. Time in Int is fine so no probs there.
Now regarding the under size you mentioned, did you mean 0.008" under size instead of 0.0008"?
If it is I am just wondering if that could be the cause, not sure how the driver locks in nowadays, think Rich will know more as he did some testing with Art. I havent use the parallel port for a long time now.
Ok my thinking
Pitch called for divided by pitch cut = 0.05/0.048 = 1.04
Frequency called divided by frequency actual = 1.03
Fairly close.
Hood
-
Or lets do it another way.
72665/75000 X 0.05 = 0.04844
Hood
-
No i meant .0008" off. Called for .050" thread pitch and if i made it .0508" it would cut a good thread.
-
just realised I can divide and multiply but cant subtract ;D
Next thought, think you said you had electronic gearing in the drive. Can you set it 1:1 and adjust your steps per unit accordingly. You will also have to drop the Vel to suit.
Run and see if its the same or not.
Hood
-
Also, have you turned off the Turn Diagnostics plugin, rebooted and tried again?
Hood
-
I would suggest that you set the rpm manualy. There is a difference of rpm which Mach is seeing and what your vfd is actualy providing. They are slightly out, not much, and may be fighting each other for Mach's adjustment of the feedrate. Don't change the pitch, but rather change the feedrate.The feedrate is set based on the rpm. If you use the wizard you can put pitch out to a lot of decimal places, the wizard will show the feedrate rounded to some number, but what you input will be used. Mach can read the rpm more accuratey than you can measure it.
Do scribing tests as that is easier and more accurate than cutting a full thread thus eliminating mechanical / cutting aspects
of threading. Thus there is no spindle slow down, but at 5HP you shouldn't have any anyway.
Do not use any diagnostics, disable them, as Hood noted.
BTW, make sure you use 3 to 5x the pitch to allow for acceleration of the Z axis, even 10x.
RICH
-
I have not put a tach on it yet to verify rpm. I changed the screen display to give two decimal places on the rpm. It is definitely moving around but not much. The vfd says 10.4hz. My calculations say i should have 299.866 rpm but i have 309-310. At 59.8 hz i should have 1726 but i have 1780. It is a consistent percentage off. At 310rpm the vfd does not move off of 10.4hz and the incoming 0-10v from mach 3 does not budge at all either. The feedrate display is showing correctly for 310rpm and .050 pitch. I added another decimal place to those too. I am leaning towards the rpm being off from what mach 3 is saying. Maybe the c3 index pulse board is off slightly. I might try another optical sensor that goes straight to the breakout board.
-
The only two things I can see it being is reported RPM is different from true RPM, but how that could be I am not sure as a single pulse per rev should be just that.
The other thing is it could be the way the servo is handling the electronic gearing. I have seen a few drives with that problem, usually the lower end ones but Tecos are a step up from them even if not what you would say top end.
I am not sure how hard it is to change the gearing in your drives, its a simple matter in the Allen Bradleys, so if its easy enough (must be easier than getting another opto ;) ) I would certainly give it a go at 1:1 to see if your result stays the same or changes.
Also have you disabled the Turn Diagnostics?
Hood
-
it doesn't matter if you command 300 and it actually rotates at 310, as long as mach is reading the pulses it will respond to the pulses not the commanded speed.
-
I disabled turn diagnostics and rebooted. No change. I changed the electronic gearing in the servo drive, made it 1-1. No change. The thread looked off by the same amount it has been. It just ran painfully slower at 50,000 steps per inch.lol I am leaning towards the rpm being inaccurate. My Diagnosis is that mach 3 is being fed the wrong rpm information from the c3 board. I don't know how it is possible though.
-
I'm using version R3.043.022.
Not the latest version, eh? Seems like I read there were threading problems in some versions that were corrected...somewhat.:)
-
i use this version without any probs
-
I just tried an optek opb917 optical switch wired directly to the breakout board. Rpm's read the same as with the old one running thru the c3 board. Grrrrrr. What version are you guys using that threads good?
-
I've had issues when bumping the kernel up.
Curious to see if it straightens out if you set your kernel back to 25k and re-tune ... just for a test.
Maybe, maybe not. Just a shot.
Russ
-
tried the kernel speed at 25k, it didn't make a difference. I have figured out that if i multiply the pitch by 1.018 i get a good thread that matches up to a tap. tried it with two different threads and it works. At least i have a workaround for now.
-
fast89,
- Do scribe test's for reasons I mentioned. The scribe tests that i did were used to measure pitch to 0.0002" and
you don't get that from comparison to a tap. The tolerances are noted in threading on the lathe manual, page 26.
So for a 1/4-20 the error allowed for a 2A over .3" is 0.001". Said a different way.....one thread is 0.50", .3"/.050"=6 threads,
thus 0.001" allowed. If 0.0008" per thread you are over by .0008 x 6= .0048" - .001"=.0038 lets just say 4X.
- Although I have a C3 board for the index never put it into use. I think Russ has used it so he may comment on it.
- How linear and accurate is your Z axis?
RICH
-
You may be getting tired of hearing this, but .... Can you verify the accuracy of you Z steps-per ?
Early on you said it was exact by referencing a move of .010". That would be difficult to verify, try a much longer move .. as long as you can accurately measure.
With a move of .010", the .0008 in .050 error would only show up as .00016 which would require quite q delicate indicator.
No problems ever with the C3 here, just that one got dirty from belt dust.
Russ
-
..and be certain that the backlash is taken out by first making a short move in the "verify" direction.
-
Yeah, i'm a moron. I thought my screws were .2 pitch which would be 5000 steps per inch. I have 5mm pitch screws which is 5080.01 steps per inch. Which ends up being about exactly the error i was off. Changed the steps and the first thread was perfect. The error was too small to see when jogging .010" with a .0005 indicator. Thanks to all who replied, i much appreciate it. I'll try to be a little smarter next time lol.
-
Has been done many times before but you were so convincing ;D
Hood
-
NOW you're cookin' with GAS ! ;D
Russ
:)
-
glad you're sorted, we'll remember this one.
-
Happy you found it.
We spent many hours with Art trying to get threading fixed and don't want to revisit testing.
Hope you now understand why we are so adamant on rpm and axis accuracy.
RICH
-
I just want a copy of his modified screen for the Lathe, don't like any of the lathe screens, most machine tool controls have the same screen for mill and lathe.
-
a copy of his modified screen for the Lathe
What screen are you referring to?
RICH
-
Fast89 said he modified his mill screen for lathe, would like to see it.