Problem- G02 and G03 not working correctly

[Aircraftman]

Check this problem out.....

My shop recently purchased this very used Mighty bridge type vmc. It has a Mitsubishi Meldas 520AMR control. I got it up and running and ran a few simple programs to check for axis position repeatability. To my amazement when it tried to do a basic square tool path, with cutter comp on, every time it rounded a corner with the G02 or G03 command it would be way off in X and Y on the next depth cut pass from .005 all the way up to .100!! Each time it went around the square the location would be random on the next pass, no pattern at all. Program does the same thing whether it's Radius or I and J called out. However if I remove cutter comp so the tool path does 90 degrees on the corners with no radii it's perfect. Is it backlash or parameters?
Any ideas?

[Superman]

I would not yet say one or the other,

But I think you test may be flawed, toolpaths are not the same

Create 4 toolpaths for the tool to follow around your shape

• 1- one to use G41 with a comp of the tool radius around your shape.( sharp corner mode )( tool goes past the endpoint off the part )
• 2- Same as #1 but roll cutter around corners.
• 3- offset your shape by the tool radius, use G41 with a radius of zero in the control.
• 4- same as #2 but with no G41 in the program
  
  all programs would create the same shape

What you are checking for is cutter comp functionality

Is having a comp value creating the problem ?
Is the tool finishing the last block of info before commencing the next ( in-position tolerance toooo large )
what happens if you single step each line when using comp ? it should give same results as not using comp

To check for backlash
-mount a clock in the spindle and set against the side of the vice
-winding the axis in one (-) direction only, zero the axis
-move it away and re-check
-( using fine scale ) wind past zero (-) on the clock, and reverse direction (+)
clock should not jump ( over compensated backlash )
not move for a few clicks ( backlash exists)
- keep moving (+) to zero point on clock --- control should also read zero

repeat for the other axes
---if backlash exists- you have to determine if components are worn and need replacing ( do backlash test near travel ends and centre of leadscrew should show if is wear- different readings )

You should also check parameter settings and compare back to the factory default settings, just to tighten the machine up again ( you don't know what they changed ) suggest first looking at the one in red or something of similar function.

[dcoupar]

Why not post your program here?

[cogsman1]

Is your "Plane select" correct? G17, G18 or G19. That would make the axis positon change.

[Aircraftman]

We have answers gentlemen!

After fearing I had ball screw problems, or backlash issues with this machine, I was able to look at the manual for my Mitsubishi Meldas 520AMR control on line at meau.com (Mitsubishi Electric Automation). After finding the control parameters page I spotted parameter 41 (R Compensation).

When this parameter is set to on it says:
In circular cutting, an inward move caused by a servo delay against the command is corrected.

When this parameter is set to off it says:
In circular cutting, an inward move occurs because of a servo delay against the command resulting in a smaller arc than that specified by the command

Anyway, I don't really understand what either one of those means but when I looked at the control parameters page on my machine, parameter 41 was set to on. So I set it to off, and ran my basic cut a square program with cutter comp on and walaaa! the tool path ran perfectly including all the arcs.

Everything is working fine now, but I will look into the parameter 41 thing so I can understand what the purpose of it is.

Thanks for all of your suggestions and ideas.