Hello Guest it is October 19, 2019, 04:12:54 AM

Author Topic: Unwanted rounding off of tool motion at line cut intersections in Mach3  (Read 8893 times)

0 Members and 1 Guest are viewing this topic.

I have a gcode file which specifies two straight cuts intersecting (and ending) at a point. This is correctly  shown as two straight lines intersecting at a point in blue in  the Mach3 tool path display. After a failed part, ( Corner radius too large) and subsequent detailed investigation I discovered that  Mach3  appears to round off the angle between the two straight cuts with a small radius not giving the effect I required.  On close inspection this is shown by the dotted green line  showing actual tool motion  in the tool path  display. Effectively this corner/intersection  now has a cut radius greater than the cutting tool radius. I had deliberately chosen the tool radius to equal the corner radius I was seeking.
Why does this happen and how can I get Mach3 configured to follow the G code  lines exactly?


 :'(

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Is this a fairly high speed light machine such as a router?
It will probably be because of constant velocity and your machines acelleration capabilities. You could run in Exact Stop mode and see if it then works but motion will be jerky at the endsof cuts because it will come to a stop before it changes direction. If Exact stop cures your problem put back to CV mode and have a look at the "Stop CV on angles > degrees" option, its on the General Config page.
Hood

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
There are two ways of running - Constant Velocity and Absolute Stop - see on the Config page.

In absolute stop, the cutting axis will come to an absolute stop BEFORE the other axis starts to move - this will produce a "square" corner - althoug cutting internally you do, of course loose the tool radius - which you can file out if you wish.

In Constant velocity - Mach3 reads forward and anticipates the next command, and as one axis is decelerating, the other axis accelerates so the tools ic constantly cutting - but this leads to a rounding of the corners - and the faster you go the "worse" it gets, becasue the axis need more time to accelrate/decelerate.

As Hood stys there is the ability to alter the parameters of Constant Velocity to make the acceleration/deceleration quicker, or only active between certain distances,

On a right angle cut as you are doing, absolute stop may not be too much of a distraction. Where you get an arc to cut, which a cad program makes up of many small straight lines, then Mach3 still stops between each one - producing a very jerky movement - hence the need for constant velocity.


Not me driving the engine - I'm better looking.
Thank you gentlemen for your help. I now appreciate why Mach 3  tries to smooth off the corner and why it might be generally useful (Although not in this case).

My machine is not a lightweight machine , it is a mill drill of about 200kgs mass, but as I was cutting a foam pattern for a spoked wheel for casting purposes, I had set the feed rate near to the  maximum allowed in the machine set up! I was surprised to see a corner radius of around 0.125" on some of the spoke  intercept points  with the rim andr centre( Not all the intercepts were in error-some were correct/cutter  radius), when using a cutter of  0.09375" radius . As it is a symetrical pattern , the radius errors really stand out.

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Is this a spoked wheel for a railway locomotive ???

I would be interested in seeing the code for it.
I am wanting to write the code for a spoked wheel for my next locomotive - a Garratt 2-8-0 0-8-2 which I was thinking of milling out of a blank - about 8" diameter (10 spoke, I think). I say this becasue good foundries, to do small work are a bit few and far between up here now.

I have a Warco lathe/mill which I have converted to CNC
Not me driving the engine - I'm better looking.
yes it is loco wheel and the Mill/drill is a Warco one  I converted to CNC!.

Thw wheel was simply draw in a 2D cad program, the cutter path was draw in a separate layer spaced a cutter radius from the desired wheel/spoke outline . Any fillets would be automatically produced by the cutter radius.  The DXF file was passed through to Lazycam, the cutting parameters entered layer by layer and the g code auto generated from there. It is in no way a sophisticated or polished program, I can see lots of ways of improving the efficiency of the code,  but the above was quick and easy to do and adequate for cutting out the the few examples I needed .

I don't have  3D CAM software so this was a 2.5D example with straight sides and flat top. Any spoke rounding etc needed  would be done using fine sandpaper on the foam prior to casting, which is very easy to do. ( A lot easier than rounding cast iron!)