the mystery of the wonky corners

[kingcreaky]

Gents.

Hope somebody clever than I is about this evening....

So doing some mild pocketing in ply... this is meant to be square


see how its rounded the edges of two of the corners but not of the other two?

this is compounded, by the other pocket its doing on the same job has done the same thing


It must be something physical with the machine rather than software because the toolpath looks fine in vcarve


only thing ive changed today is... ive tightened the belts... but it jogs around fine.... and ive increased the acceleration on X

ANY ideas will be welcome... im scratching my head.


looking at both the photos X is vertical... Y is horizontal

[Jonathan]

Intereting...

By 'meant to be square', do you mean it's meant to be a square, or that the corners are supposed to be sharp? If its meant to be cutting squares and you get that, then at least part of the problem is the step/mm value in the motor tuning settings has changed...so check those. On your machine it should be the same number on X and Y and two times that number on Z.

Is the machine loosing position, i.e. does it return to (0,0) when finished? If you suspect it might be a motor stalling, then run the program I made here:

http://www.mycncuk.com/forums/gcode/...or-tuning.html

If it survives that test without stalling it'll survive pretty much anything, so I'd do it anyway as you've changed the motor settings.

Does it look correct in the tollpath preview in Mach3? Zoom in on the corners...
If you run the program again does it follow the same path?

[kingcreaky]

By 'meant to be square', do you mean it's meant to be a square, or that the corners are supposed to be sharp?
CORNERS MEANT TO BE SHARP

If its meant to be cutting squares and you get that, then at least part of the problem is the step/mm value in the motor tuning settings has changed...so check those. On your machine it should be the same number on X and Y and two times that number on Z.
BOTH X AND Y STILL SET TO 80


Is the machine loosing position, i.e. does it return to (0,0) when finished? If you suspect it might be a motor stalling, then run the program I made here:

http://www.mycncuk.com/forums/gcode/...or-tuning.html
CANT RUN YOUR PROGRAM AT THE MOMENT BECAUSE IL LOOSE THE POSITION FOR THIS JOB
BUT YES, IT RETURNS TO THE SAME POSITION


If it survives that test without stalling it'll survive pretty much anything, so I'd do it anyway as you've changed the motor settings.

Does it look correct in the tollpath preview in Mach3? Zoom in on the corners...
If you run the program again does it follow the same path?
YES THE MACH TOOLPATH LOOKS OK... ALTHOUGH I CANT WORK OUT HOW TO MOVE THE PANNING POSITION IE (SHIFT AND DRAG, CONTROL AND DRAG) ... I DONT KNOW HOW TO DO EQUIVELANT OF CTRL + DRAG IN VCARVE WITHIN MACH...


SO WHILE WAITING FOR MY KNIGHT IN SHINING ARMOUR... IVE REDUCING THE ACCELERATION RATE OF BOTH x AND Y TO 2500.. NOW IT GOES VERY SLOWLY, IT DOESNT CUT THE INSIDE OF THE CORNER LIKE THE PICTURE SHOWS MY INITIAL RUN DID, BUT IT DOESNT SQUARE THE OUTSIDE OF THOSE TWO CORNERS EITHER.. IT KIND OF CUTS THE CORNER. IM VERY CONFUSED.

[jcb121]

I get the same problem with VCarve.

[Jonathan]

To pan in the toolpath preview it's either middle click and drag, or right click and drag...I don't remember which it is.

If the acelleration is far too low and you're using G64 (constant speed) mode, then your corners will all get rounded... but it would have to be very low for that to happen. 2500mm/s^2 is pretty high (sure that's not the rapid feedrate). You could try putting G61 at the beginning of the code to force the machine to stop at each co-ordinate precisely.

Where you've tried to cut the slot, parallel to Y, it does look like one of the X motors has lost position and skewed the gantry, causing the subsequent cut to not be parallel to the first. Are the pulleys definitely tight and not slipping on the shafts?

Can you post or send me the code so I can check it?

[kingcreaky]

here you go... thanks for your help buddy

2MM_POCKET_b.txt

[John S]

Not had chance to look at the code yet.

However if you look at the picture it cocks up on opposite corners, assuming the picture is taken from the front of the machine then it barfs out when the Y changes direction so I'd check couplings, pulleys belts etc, anything to do with the Y axis mechanically

[Jonathan]

The code is correct. It would be a good idea to use ramping though instead of plunging the cutter, since plunging puts a relatively high force on the cutter.

[kingcreaky]

if I put G61 at the beginning all is fine.... what is that all about then? why all of a sudden is it playing up?

only thing I can think of is I greased the Y ballscrew the other day and havent cut anything since.. perhaps im experiencing the momentum of the Y now it moves easier?

[Jonathan]

if I put G61 at the beginning all is fine.... what is that all about then? why all of a sudden is it playing up?

Looks like it's something to do with changing the acceleration settings then. Go into your mach3 folder (probably C:\Mach3) and find and copy the .xml file for your machine and post it here, then we can check the settings. It'll be called whatever the name of the machine profile is, which you click when loading Mach3, with .xml on the end. Or just post a screenshot of the X and Y motor tuning settings, but the whole thing is better.