Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: jonny quest on October 25, 2019, 01:14:56 PM
-
Mach3, ESS Smoothstepper, Rhino5, Madcam.
I've tried backlash compensation on and off. Have my CV settings at .1, no other CV boxes checked. Tried IJ mode absolute and incremental. Talked with CAM developer about all settings. Post is cutting with G2/G3.
I've played with motor settings. Tried cutting at 1IPM.... I'm stumped.
Pic shows what's going on. Black shape is what I'm trying to cut. Red shape is cut part measured on CMM. I'm always getting this deviation at around the 10 o'clock position no matter what I try. The toolpath is correct, I really believe it's something in mach3
-
Pic didn't load first time
-
And pic rotated, so cut issue is at 8 o clock. Not 10 o clock as mentioned in first post
-
Can you please attach your Gcode that is causing the problem ?
-
How is it being measured, 3 or more points on an arc or a digitised path?
-
I'll have to post the gcode on Monday.
It's measured with 3600 points, .0001" resolution. Very accurate. The cut part discrepancy is .023", so pretty obvious.
-
Are you cutting this on a mill or router type machine?
-
Mill. Cutting mild steel. I can do skim cuts of .001" and it will cut exact wrong shape
-
If you are cutting cam lobes then teh Black line is bad code. Teh acel / Deacel ramps should be symetrical on each side of teh lobe. The red line appears to be more symetrical than teh black line. The black line has an inverted ramp which is Bad lobe design in most cases.
From what data did you plot the black line. I would like to see teh Gcode that cut it.
Just a thought, (;-) TP
-
Are you using tool comp?
-
I just broke a belt tuning my X axis servo. Hopefully I had a bad spot on the belt causing this. Won't have parts for a few days.
Not bad code for a cam. Finger follower. Not direct acting
-
Can you post your Gcode for the lobe ?
(;-) TP
-
Belt was bad on my X axis... but still cut the same. Here is some gcode
G00 G49 G17 G80 G50 G90 G64 P0.05
(.25 4 FLUTE CARBIDE SLOW)
M6 T1
M8
M03 S2500
G17
G00 X0.438 Y-1.759 Z0.500
G00 Z0.000
G01 Z-0.270
G17 G03 X-0.044 Y-1.242 R0.500 F3
G17 G02 X-0.855 Y-0.901 R1.242
G17 G02 X-1.242 Y0.003 R1.242
G17 G02 X-1.185 Y0.404 R1.438
G17 G02 X-1.173 Y0.440 R0.692
G17 G02 X-1.089 Y0.647 R2.406
G17 G03 X-1.025 Y0.810 R3.070
G17 G02 X-0.797 Y1.198 R1.161
G01 X-0.792 Y1.203
G17 G02 X-0.310 Y1.502 R1.027
G01 X-0.305 Y1.503
G17 G02 X0.061 Y1.545 R1.197
G17 G02 X0.776 Y1.270 R1.197
G01 X0.787 Y1.260
G17 G02 X1.030 Y0.967 R1.164
G01 X1.035 Y0.958
G17 G02 X1.133 Y0.731 R1.161
G17 G02 X1.141 Y0.702 R0.692
G17 G02 X1.184 Y0.477 R1.752
G17 G03 X1.201 Y0.360 R4.175
G17 G02 X1.223 Y0.231 R8.824
G01 X1.225 Y0.222
G17 G02 X1.234 Y0.147 R1.412
G01 X1.237 Y0.114
G17 G02 X0.949 Y-0.802 R1.242
G17 G02 X0.068 Y-1.241 R1.242
G17 G02 X-0.030 Y-1.242 R1.190
G01 X-0.044 Y-1.242
G17 G03 X-0.561 Y-1.724 R0.500
G00 Z0.500
M5 M9
M30
-
Attached is a dxf drawing made from a backplot of the gcode you posted.
Suggest you print the cad file full size and trace your actual machines path on the print.
You can also compare original drawing to backplotted drawing.
RICH
-
OK that checks out now HOW did you derive teh Black line plot you used to compare to teh actual cut profile that you measured ?
(;-) TP
-
That Gcode is producing the black line perfectly by the look of it.
-
Thanks Rich. I'll print it out later tonight.
Both plots are measured on a CMM. Then imported into my CAD.
-
Seeing how teh Gcode is a centerline profile how could it match teh actual cut seeing how there is a .125" offset of teh cutting tool. A conversion had to be made to be able to plot teh cut profile based on teh Gcode.
Just a thought, (;-) TP
-
Try cutting it with CV turned off (G61). What is teh look ahead setting ?
I have drawn this in an XY plotter ran by Mach3 about 20 times now 20 different ways and each time Mach3 drew it exactly how it plotted it in teh toolpath.
But I am still looking for something that could case this OTHER than the hardware. What type machine cut this. Steppers or servos ?
(;-) TP
-
The code I shared is for an offset master. But the error is the same, no matter what size the shape is.
Servos, G0704 style mill. It's definitely not the frame or axis flexing.
The look a head was 600. I just changed it to 200. Same results.
I am using a ESS smoothstepper
-
I have tried CV off, on.... currently on .1 setting. No other CV checked.
Backlash comp on, and off. Same results
-
i just printed on paper the file Rich posted, and printed my cad drawing. They overlay exactly.
So I'm open to suggestions to try please!
Is there a bug in Mach3 version? What's the best version I should be using? Is there a stuck modal (correct term?) in my gcode I need to clear? Does this clear everytime I re start my computer?
-
First thing to test is to put a pen in your spindle and let teh machine DRAW teh part to see if cutting forces are contributing to teh problem.
(;-) TP
-
It's not cutting forces. I can do a .001" skim cut, take part in and out of fixture... black marker up part, cut again to exact same size and it will just rub original cut part.
-
Could G64 be the problem? Where does this function get it's rounding properties from?
-
Taking a skim cut is not like doing a full cut on teh machine flex wise. The pen trick will tell teh story.
Have you by chance tried reversing teh direction of cut to see IF it changes anything ? As is you are doing a climb cut.
(;-) TP
-
You said you already tried turning CV off with no change ??? Here I see no difference between G64 and G61
(CV on CV off) when ploting teh Gcode.
(;-) TP
-
I would turn CV on and off with the check box in MACH3 config only.
The post processor is still the same. Should I remove a string in post?
-
Just change the Gcode file for testing . Change G64 to G61 in the preamble.
(;-) TP
-
So your CAD file agrees with my backplot of the gcode you posted.
So it's not a gcode problem.
Do what TP said in reply 22. Have the machine draw over the full size print using
both G61 and G64. That will eliminate any doubt on those modes.
Someting that I would try is changing the Gcode to get rid of the two G01 moves.
Join the arcs such that there is no small lines between the before and after arcs.
Arc difference will only in ten thou's of an inch probably!
Seems like the machining goes off path because of G01 X-0.305 Y1.503
or the G01 X0.787 Y1.260. Easy to change and paper plot to check!
FWIW,
RICH