the mystery of the wonky corners

Gents.

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

So doing some mild pocketing in ply... this is meant to be square
Attachment 8481

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
Attachment 8482

It must be something physical with the machine rather than software because the toolpath looks fine in vcarve
Attachment 8483

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

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?

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.

I get the same problem with VCarve.

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?

here you go... thanks for your help buddy

Attachment 8484

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

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.

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?

Quote:

---

Originally Posted by 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?

---

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.

4 clues... you said...

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

only thing ive changed today is... .... and ive increased the acceleration on X

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

if I put G61 at the beginning all is fine....


What you're seeing is the classic behaviour when in G64 with unequal accel on X and Y. If your accel was equal but "poor" you'd get 4 rounded corners. If equal but "good" you'd get 4 sharper corners. If you'd increased your accel on Y instead of X it would be the other two corners that rounded. The rounded corners will switch to the other 2 if you reverse cut direction. etc. etc.

Yes, just what I was thinking...I'm expecting that if we get the configuration file it will show that the acceleration on one of X and Y is lower than the other. Perhaps a typing error was made and the acceleration has actually been reduced significantly (decimal point in the wrong place) since it would have to be very low to make the large difference we're seeing here.

Given the cut direction (from the code) and the statement that X is vertical and Y is horizontal on the pictures (curious but what was stated) then X accel HAS to be greater than Y. So if the accel HAS been accidentally REDUCED then it would HAVE to be Y that was changed and NOT X (as stated) otherwise the rounded/sharp corners would be swapped.

thankyou all for your help.

appears xml is an unsupported attachment type so it can be found here
http://pensys.co.uk/cnc/Mach3Mill.xml

Try lowering the CV Dist tolerence In Mach go to General config and in the CV Control section and "CV Dist tolorence" to lower number and see how it goes.?. . . .OR . . . Try setting the "stop CV on Angles>" to 90 deg.
Both will have an affect just in different ways depending on the G-code.

If it works then basicly your trying to go too fast round the corners.? Go read this . . http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

OK - That xml you posted has accel set to 400 for BOTH X and Y so methinks 'tis NOT the one you were using where you get two rounded and two sharp corners. That said an accel of 400mm/s/s is pretty p*55 poor. Why have you got it so low?

Hi Jazz - just a note about the CV doc you linked to. I've been banging on for over 5 years on the Mach forum that the description of CV angles in that doc is just plain wrong.

Ian

Quote:

---

Originally Posted by stirling

Hi Jazz - just a note about the CV doc you linked to. I've been banging on for over 5 years on the Mach forum that the description of CV angles in that doc is just plain wrong.

Ian

---

Ye know what you mean and not got time to get into it or look at the Xml etc. Mentioning the link was more to give an explanation of what CV does rather give figures to use.
If the Accel settings are what you say then I very much doubt CV is the problem anyway.? Unfortunately not got time or energy to help more so leave you all to it.!

Hi Matt,
what did you do in the end to overcome this problem? my machine was doing this the other day on a simple rectangular profile with rounded corners. It was only happening on the 2 opposite corners. will check if the settings are the same for x and y, but if they are identical how did you resolve it?

Dan. These lot will correct me when im inevitably wrong, but ensure you velocity and acceleration values are the same for both X and Y axis

make sure your acceleration is not too slow

that always sort it for me. Im not too sure of the technicalities of why. There is a code you can inject... like 'G60' or something you append to your gcode file before opening with mach. but it makes the machine stop at every change of direction. but I managed to sort it with the explanation as above.

Matt

Quote:

---

Originally Posted by Danielroyal25

Hi Matt,
what did you do in the end to overcome this problem? my machine was doing this the other day on a simple rectangular profile with rounded corners. It was only happening on the 2 opposite corners. will check if the settings are the same for x and y, but if they are identical how did you resolve it?

---

Dan if it's jurking just in the corners then chases are your running G61 Exact stop mode. Your better running in G64 constant velocity (CV) mode.
If your using Mach standard 1024 screen set then you can tell by the LED light just to the right of the Reset button and next to Dwell LED. It will be lit green when in G64 CV mode and off when in exact stop.

To test this type G64 into MDI before running the G-code again. First check the G-code for G61, it will be somewhere near the top of the code and delete if there. You could always put the G64 command in the G-code file but I wouldn't.

Better place to do this is the initialzation string in the General Config so when Mach starts up it's always in G64 mode. There is actually a setting in Gen config for this as well so check that but having both doesn't hurt.