I brought a MDL-A3-BSX-Un-Z100 from Marchant Dice a year ago and have only done a little with it.
So I have not explored all of its potential just done a little engraving and that’s it.
So I come to start to do some more crafty things with it and it does not do what it is told?
So I think I know I will do a square…….big mistake …….
I set it up to do a simple square with straight corners and I got round corners?
So I ran it again and watched the mach3 window
I could see the tool path and then I could see the path it had taken …mmmmm very different?
So I contacted them and sent them the tool paths and they said that they are good.
They suggested to me that I check all couplings which I have done and all seem good.
I also did a few other tests and doing a simple O it comes out good.
So it looks like when it comes to change direction from a straight line I get the issue.
I’m using Vectric VCarve Pro 7 and Mach3
So please does anyone have any ideas.
I cant help,theres lots of info out there on the problem and more than likely software related.
Last edited by deisel; 23-06-2014 at 05:46 PM.
Are you trying to do a square with an external cut or an internal cut? ..Clive
Thank you ..I will look these up
Its not a squsre im trying to do it was a test which showed me im in trouble with my machine.
Originally Posted by Clive S
Originally Posted by deisel
Thank you I will look these up.
I seem to remember reading a discussion on this problem a while back although I can't immediately find the thread. However, Deisel's link covers the topic - it could well be due to the settings you are using when you create the gcode. Mach3 needs to know whether to follow the toolpath exactly, which means that it has to stop at corners and then restart in the new direction but gives accurate results, or round off the corners to save it stopping and restarting. The G64 command tells it what to do, and this is generated by VCarve. There are good reasons why you might want to do one or the other in certain cases, which is why there is a choice. I'm not sure how you change the setting within VCarve but it's easy enough to edit the gcode afterwards if this is an issue. You probably won't have noticed it when engraving because the machine never goes fast enough in a straight line for it to show up, and of course if you are cutting a circle, then there aren't any corners...
Can you post your gcode file for the square test piece?
If this is a small square then chances are your going to fast. Like Neale says chances are your working in CV mode(G64)(constant velocity) which is the same as saying Don't slow down for this corner and keep same speed.!! Then me saying NO WAY am I going to get round that corner at that speed so I'm cutting the corner otherwise we'll crash & burn.! . . . . Well that's what Mach3 is doing to fulfill your request of keeping a constant velocity.!
So your choices are go slower or change the CV mode to Exact stop(G61).! Now problem with Exact stop mode is that it will pause at every start and end point of every line or arc segmant and often CAM software create there arc's using lots of tiny lines and this makes the machine judder like crazy.!
So mostly CV(G64) is used unless Small squares are needed.
Now there are some settings in Mach3 general Config to control CV so it is stopped on angles greater than you choose. If you go to Artsoft web site there is a tutorial on how to set CV. It's a bit hit n miss and does depend on the type of work your doing but you can tweak it to your liking with a bit of trial and error.
Last edited by JAZZCNC; 23-06-2014 at 09:04 PM.
Originally Posted by deisel
Thank you for this ...it seems to have done the trick.
Now all i have to do is stop the machine juddering and all will be ok
Originally Posted by JAZZCNC
Thank you for your help.