Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Rkjohn on November 07, 2007, 08:56:47 PM
-
Having a problem cutting circles. They don't come out exactly round. There will be a small flat spot on one side. The machine cuts squares within .002".
-
Hi, Rkjohn
Check for backlash in the axis's, It's usually the cause.
Thanks, Chip
-
I'm new to this. How do I do that?
-
Put a dial against the quill (if a mill or router) and jog the table so that the plunger is pushed in. Either zero or take a note of both the axis and dial readings then change to step mode so that your axis jogs in small incriments and back off the dial, as soon as you see the needle moving stop and look at the DRO for the axis you are using and the difference between that and the previous noted reading is your backlash. Repeat for all other axis.
Hood
-
Hi, Rkjohn
First theres a Jog/MPG Screen if you haven't found it, Under the Tab key, It may make it easer ? Learning curve.
Jog Mode, "Step", Cycle Jog Step, "click on it or to the right click to enter value.
Check for backlash in Axis's.
Best done with a dial indicator with 1 inch of travel,
Setup as Picture below, Jog left .750 then re-zero dial indicator 0 mark, Zero X on Mach3 Prog. Run Screen.
(this takes the backlash out to the left if any when your moving right).
Now jog .500 to the right, Dial indicator should read .500 and Mach will indicate .500, Record the distance moved.
(If the indicator shows above/below .500, Your steps Per. Unit are incorrect in motor tuning for the axis).
I would repeat Above until you get units set as correct/close as you can.
Now Jog left .500, Mach will show 0 and indicator should read 0 again "if no backlash".
If the pointer didn't make it back to 0, The distance to go to 0 is your Backlash value.
Backlash can be turned on and set under Config, Backlash, Enter the value for axis, Check the Enable Box then OK, Re-start of Mach Required.
Where to start where to stop.
Hope this Helps, Chip
-
Normally when operating a lathe/milling machine etc, one always tries to move the axis in the same direction, the problem being that the screws that move the tables have play in them, so when you reverse, the first part of the turn of the screw is lost by the thread moving across the gear to the opposite tooth, to move the table the opposite way.
This is not a problem in manual operation, because you do not tend to make such complcated moves - i.e. straight lines generally.
If you try and cut a circle using CNC, the table changes direction on both the x and y axis. You might start by moving the table from x0 to x1, but when you move back to x0, although your DRO's will say you have moved back by 1 unit, you may have only moved back by 0.995 i.e. 5 thousanths short. You can test this as outlined above - move from x0 to x1 - to make sure that any backlash is taken up in the positive direction. (I use a G0 X1 command rather than jogging) and measure the distance you have moved. I use digital calipers to measure, and now zero them. Move from x1 to x2, then x2 to x1 and measure again. The calipers should read 0, but will not - they will read the "backlash" figure. Repeat for the Y axis. Repeat for the Z axis. (Actually repeat on the same axis several times to check your figures - if you are not getting the same figures consistantly (and it is difficult to accurately measure small distances) take a mean average.
It doesn't matter in which direction you actually do this - you could go 2 - 1 - 0 - 1 if you wanted, because , in theory, at any rate, backlash should be the same in both directions.
Under Config/Backlash enter the measurements and tick "backlash enabled". If you restart Mach3 these figures will be remembered.
This means that when Mach3 is traversing - if it hase to change direction on any axis, it will insert the extra pulses at the change of direction of the move to take up the "loose" movement of the screws, so that you maintain accuracy.
My lathe, when cutting a ball shape in the middle of a rod will traverse, then cut the G2 or G3 curve up to the crown of the ball and stop. Backlash is taken up (You can see the motors moving, but the table doesn't) and then it cuts down the other side of the ball. It leaves a faint mark on the work where it has changed direction. If the backlash was not enabled, there would be a flat area on the ball, where the Z axis (the main traverse) was still moving (because that has not changed direction) but the x axis was not moving because the backlash in the gearing was being taken up.
-
Thanks for your help. I just ordered a dial with a magnetic base. Don't know why, my table is wood. But thas all I could find.
-
Hi, Rkjohn
Is this flat spot in line with one axis, Clock angle 9:00 3:00 X, 12:00 6:00 Y, or a combination of X,Y 1:30 4:30 7:30 10:30.
You could get started by enabling the backlash and putting in an estimated value's for X, Y or both X Y.
Thanks, Chip
-
Chip
Thanks
The flat spots are on both X & Y. I'm in no hurry so I'll wait till I get the Dial...Just want to get it right so I can sell it. I'm about done with my new machine.
Ron
-
I tested the X & Y with a dial & they both came out to "0" backlash. I built this machine very tight so I'm not supprised. Maybe I was running to fast. Any other suggestions?
Thanks
Ron
-
How did you program the code to machine the circle ???
(;-) TP
-
Ran my DXF file thru LazyCam.
-
What diameter is your circle and how long are the flats?
Graham.
-
Had 2 - 1/2" circles & they turned out to be rounded squares. Had a 1 1/2" circle & it was better but had some small flats. Useing an 1/8" bit.
-
Use the circle cutting wizard and see what the circles turn out like.
Hood
-
I can't figure out how to use the wizard. Here is the extracted code from the Gcode for the 1/2" circle. It looks good to me. Maybe you can see something.
N1450 G0 Z0.5000
N1455 X7.2003 Y2.2248
N1460 Z0.1000
N1465 G1 Z-0.2500 F30.00
N1470 G2 X7.5000 Y2.3750 I0.1122 J0.1502 F15.00
N1475 X7.2003 Y2.2248 I-0.1875 J0.0000
N1480 G0 Z-0.1500
N1485 G1 Z-0.5000 F30.00
N1490 G2 X7.5000 Y2.3750 I0.1122 J0.1502 F15.00
N1495 X7.2003 Y2.2248 I-0.1875 J0.0000
N1500 G0 Z-0.4000
N1505 G1 Z-0.7500 F30.00
N1510 G2 X7.5000 Y2.3750 I0.1122 J0.1502 F15.00
N1515 X7.2003 Y2.2248 I-0.1875 J0.0000
Ron
-
I took out the 1 1/2" circle, put it into Mach3Mill & then loaded it into LazyCam. The top & bottom look OK but the right & left sides do not & thats where I had the problems with being off. Here is the code.
N5 (File trimer hold mold and top bottom z axis )
N10 (Default Mill Post)
N15 (File Posted in Mill Mode)
N20 (Tuesday, November 06, 2007)
N25 G90 G80 G40 G91.1
N30 M5 M9
N35 M6 T1(TOOL Change)
N40 G43 H1
N45 G0 Z0.5000
N50 X1.0767 Y0.5987
N55 Z0.1000
N60 M3
N65 G1 Z-0.2500 F30.00
N70 G2 X2.8750 Y1.5000 I0.6733 J0.9013
N75 X1.0767 Y0.5987 I-1.1250 J0.0000
N80 G0 Z-0.1500
N85 G1 Z-0.5000
N90 G2 X2.8750 Y1.5000 I0.6733 J0.9013
N95 X1.0767 Y0.5987 I-1.1250 J0.0000
N100 G0 Z-0.4000
N105 G1 Z-0.7500
N110 G2 X2.8750 Y1.5000 I0.6733 J0.9013
N115 X1.0767 Y0.5987 I-1.1250 J0.0000
N120 G0 Z0.5000
Ron
-
rkjohn
if you can run a .250 end mill this cuts a 2.5 circle. it will make two rough passes and one finish pass.
g00 g20 g91.1
g00 z.100
g00 x-.975 y.975
g01 z-.250 f25
g02 x-.975 y.975 i.975 j-.975
g01 z-.500
g02 x-.975 y.975 i.975 j-.975
g01 x-.9723 y.9723
g02 x-.9723 y.9723 i.9723 j-.9723
g00 z.100
g00 x0 y0
m30
-
I changed your code to cut 1/4" & slower. Here is a pic of how it turned out.
I must have some backlash but I can not measure it with a dial.
I also tried to load the gcode into LazyCam & had an unrecoverable error.
-
Hi, Rkjohn
Have you checked if your in CV Mode, May be causing the Problem, Config, General Config, "Motion Mode", set to Exact Stop.
Thanks, Chip
-
rkjohn
lcam is having some problem with arcs,they are working on that.
you say your backlash will measure pretty good with a dial indicator,so you might have to consider this.
my machine fliped out 6 weeks ago,and was cutting a circle that looked like yours,but not as bad.
the problem was in my device drivers.when i upgraded mach some how it messed up some drivers and the machine started cutting weird.
the worst one was the video driver.then the printer port.try uninstalling and reinstalling drivers.
-
rkjohn
loaded that circle program in two differant lcam programs here ,they loaded well.that makes it a stronger case to look at the video card and drivers.
-
RKjohn, as a reference how did you measure the backlash?? Is backlash turned OFF in mach? Is the CV setting as it was when installed?
(;-) TP
-
Backlash is not enabled. I tested backlash like the photo on page 1 of this post.
-
Turn off backlash comp on Mach and restart Mach.
Now if you put a pen/pencil (not a felt marker type) in the spindle and draw a circle with it (code below). Do you still get an error in the circle?
G20 G40
G00 G90 X1. Y0 Z1.
Z.05
G01 Z0 F1.
G03 I-2. F10.
G00 Z1.
M30
If you say you have no backlash then it must be movement under load, the pen will have no load so should draw a perfect circle.
If the circle is still wrong, then you have got backlash.
Graham.
-
Guys, just while we are on the subject regarding cutting a circle, when i load up gcode for cutting a circle from the wizards
the circle shows up way outside my table perimeters and i can not place it within the table perimeters for some reason, can anyone please tell me how this is done? :-[
Cheers.
-
Try putting a G20 (Inch) or a G21 (Metric) at the start of your NC program.
Graham.
-
Same problem here. One side of the circle ends with a flat. If the circle is about 8 inches, the flat is about 1 inch long. We generated code with lcam, cut2d from vectric and with Rhinocam. We used lines segments to create the circles, and we used arcs to create the circles. We used a stepper based machine and a servo based machine. Within small differences, the problem staid the same. We continue to look into paramaters here and willa lso try and run EMC on a PC to see if there is a mach problem. It seems that this issue is a tricky one...
Cheers
Rainer
PS:Nice meeting you in York Graham, Brian, and the rest of the gang!
-
Hi Rainer,
when you used small line segments how long was a line segment move in X & Y ?
What is the resolution of your machine axis ?
If you put a long travel clock on the bed so it will show the last 1/4" of movement of the axis, watch to see if Mach is counting and the table stops in the area of the flat.
Are you getting a 1" flat in one place or 2 opposite each other.
It could be you are running out of resolution ? :(
Graham
PS: I had a great time in York, it was nice to put faces to names. Funny I set off 20 miles outside York UK and 3500 miles later ended up in York PA
-
I have a servo driven machine using 1000 line encoders and the axis is geared down 1:5. I use steel loaded timing belts which have no backlash. They are pre tensioned with 160lbs and sound like a guitar string. No movement there... per revolution of the drive shaft I get about 5 inches of travel. So I need 5000 ticks per revolution and that yields roughly 5 inches travel. And that's a theoretical 1/1000 of an inch resolution. Is there another resolution I have to be concerned about? The smooth stepper has a few settings regarding resolution and precision but due to a lack of documentation I have not bothered to dive to deep into it's settings. I run the default settings. However, the problem also shows up using Mach3. I'm in the shop today and will collect sample g-code and such. It's impossible to get closer to this without hard facts. Ha, York, UK to New York, NY to York PA. That's a lot of York for one trip 8).
R
-
lemo,
Have no answer, curious, and just some thoughts.
From a numbers point of view, if you divide a 8" circle into 50 equal parts the length between
two parts is 1.0026" and if it was a true circle with just one flat you would have a change in diameter of
.0315" ( 1/32" ).
What are you cutting?
Can you post the Lazycam, cut2d code that you tested with?
What version of Mach and SS plug-in are you using?
RICH
-
ITS ALL MACH3's FAULT!!! >:D
Well... cough cough.... NOT... ::)
Today the problem was found... The Z Axis carriage is pulled around on the gantry using a timing belt and that is linked to the carriage with a little AL block which also tightens the belt. Two 1/4 inch screws are used to lock that block onto the carriage. All was tight... but... the holes were bottomed out... HA! The darn thing was tight enough that there was no indication of a fault while manhandling it. But when the 250lbs gantry stops or accelerates quickly, then it slipped a tiny bit, thus leading to the symptoms of backlash. The holes have been set deeper, the screws tightened tighter. And the friggin flats have taken a vacation. Circles are nice and round now.
Flats -> some sort of backlash or slippage of some kind.
Next time I will rivet, braze, weld, glue, and fuse that bugger to the parts.... Did I forget a method?
Cheers
Lemo
-
Mach 1 - Lemo 0 ;)
Glad you figured it out, now what are you going to do for fun? :)
RICH
-
Nice one, you will not forget that one in a rush.
:)
Graham