Half Circle on Y-Z

This forum is for general discussion regarding VCarve Pro
Post Reply
dankitchen
Posts: 3
Joined: Thu Apr 12, 2018 9:42 pm
Model of CNC Machine: Frankenstein :-)

Half Circle on Y-Z

Post by dankitchen »

I have been able to cut the shape I want which is a half circle cut on the X-Z or Y-Z axis. I have been using a moulding tolpath where the drive rail is a 0.0001" rail then the profile is a half circle. I have attached a screengrab of this cut at the edge of a block to show the result.....so all is well but I find the way the stepover is handled makes for about a 15 second cut. I am setting up for production and feel that it is possible to get these cuts down to a few seconds.
This is the mounding path that works great but is slow to cut due to the up down nibbling/stepover.
This is the mounding path that works great but is slow to cut due to the up down nibbling/stepover.
I have tried using a fluting path with a curved ramp in on each end of a profile but, I can't get it to do a proper half circle shape. I have attached a pic of what this profile looks like.
This is the fluting path
This is the fluting path
The final profile is a 1.5" long, 0.75" deep but 1/4" wide recess cut with a 1/4" bullnose bit.

Thanks in advance for any advice!

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Half Circle on Y-Z

Post by IslaWW »

Hand code with Gcode arcs in the G18 or G19 plane. Works like a charm, but this will not be generated by Vectric products. Very few will do this.

The "advance per revolution is much higher than you would desire, but here is a hand coded version with full circles:
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

dankitchen
Posts: 3
Joined: Thu Apr 12, 2018 9:42 pm
Model of CNC Machine: Frankenstein :-)

Re: Half Circle on Y-Z

Post by dankitchen »

Thanks for the quick reply! I'll have to try the G18 G19 I have to do 8 passes of the shape on one job so it will take a bit of g-code but i'm sure the learning experience will be worth it.

cheers
-Dan

PaulRowntree
Vectric Wizard
Posts: 1687
Joined: Sun Oct 24, 2010 7:28 pm
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)
Location: Guelph, Ontario
Contact:

Re: Half Circle on Y-Z

Post by PaulRowntree »

The FlutePlus gadget can do it from the Vectric programs, and let you visualize the results too.
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com

dankitchen
Posts: 3
Joined: Thu Apr 12, 2018 9:42 pm
Model of CNC Machine: Frankenstein :-)

Re: Half Circle on Y-Z

Post by dankitchen »

Hey Paul, Thanks for the additonal suggestion, I will have to upgrade before I can install that addon as I only have VCarve Desktop. On another note I was able to do some hand coding to get pretty much where I needed to be. To make live easier, I created a gcode file where I just did straigt lines where I wanted the half circle cuts on the z-y to be. Then I only had to make a couple changes to the overall file to switch to g19 and program the half circle.

The one issue I ran into is that if I cut an exact half circle, it is off shape because the point of the ballnose cutter is following the line so if I am doing a 1.5"x0.75" deep half circle with a 1/4" ballnose, the resulting cut will be 1.75" wide by 0.75" deep. So I had to actually do 2 separate arcs and make the distance of the cut 1.25" and adjust the radius of the arc. I know that with the moulding toolpath I was using mach3 did calculate proper compensation for the cutter. For reference sake, I have included 2 previews

Standard half circle near the top the cut ends up 1/8" wider on each side.
Standard half circle near the top the cut ends up 1/8" wider on each side.
Version with some guessing at compensation that worked pretty well but....not perfect.
Version with some guessing at compensation that worked pretty well but....not perfect.
Of course, if you are viewing this post and thinking ..... all this jackass has to do is __________ to get proper compensation for the bit I am all ears :)\

Thanks
-Dan

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: Half Circle on Y-Z

Post by ger21 »

The one issue I ran into is that if I cut an exact half circle, it is off shape because the point of the ballnose cutter is following the line so if I am doing a 1.5"x0.75" deep half circle with a 1/4" ballnose, the resulting cut will be 1.75" wide by 0.75" deep
You can program to the center of the tool. Make the toolpath 1-1/4" x 5/8", starting at the surface, and set Z zero 1/8" below the surface.

Fwiw, Mach3 is not calculating any offset or compensation with your moulding toolpath.
Gerry - http://www.thecncwoodworker.com

Post Reply