the mystery of the wonky corners

[stirling]

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.

[Jonathan]

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.

[stirling]

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.

[kingcreaky]

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

[JAZZCNC]

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

[stirling]

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

[JAZZCNC]

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.!

[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?

[kingcreaky]

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

[JAZZCNC]

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.