Looking for a Post Processor to use arcs instead of lines...

This forum is for general discussion regarding VCarve Pro
Post Reply
Doug98105
Posts: 45
Joined: Thu Feb 04, 2016 3:48 pm
Model of CNC Machine: Centroid knee mill with 4th axis

Looking for a Post Processor to use arcs instead of lines...

Post by Doug98105 »

When milling a clipart dome (or dish) on my Centroid control using the Centroid inch PP I get thousands of short line segments rather than arcs. On another high dollar CAD/CAM system I can force arcs instead of line segments. The Gcode using arcs runs much smoother on my machine.

I'm hoping there's another PP I might adapt to my controller that will generate Gcode with arcs. Any ideas?

I prefer to use my Vectric software on relatively simple jobs because it's much faster to set all the cutting conditions than the higher end software.

User avatar
Adrian
Vectric Archimage
Posts: 14772
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Looking for a Post Processor to use arcs instead of lines...

Post by Adrian »

Looking at the Centroid (Inch) Post Processor in V12 and V11 (probably earlier versions too) it has all the functionality for handling arcs in it.

Are you using that post processor? If so are you sure the curves in your vectors are arcs and not beziers.

User avatar
IslaWW
Vectric Wizard
Posts: 1409
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Looking for a Post Processor to use arcs instead of lines...

Post by IslaWW »

The supplied postP for Vectric does support arcs as Adrian mentions, but only in the G17 plane. Vectric does not support arcs in the G18 or G19 planes. That said, you may want to look at your smoothing settings if you are not happy with machine motion while cutting concave or convex shapes.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

Doug98105
Posts: 45
Joined: Thu Feb 04, 2016 3:48 pm
Model of CNC Machine: Centroid knee mill with 4th axis

Re: Looking for a Post Processor to use arcs instead of lines...

Post by Doug98105 »

Thanks for the replies guys.

Let me start from scratch. I'm inserting a clipart dome. Using the 3D Finishing Toolpath with the offset strategy (as opposed to raster strategy) which gives what appear to be a series of concentric circular toolpaths in the G17 plane at different Z levels. Are those toolpaths considered vectors? Post processing with the Centroid inch PP gives hundreds or thousands of short line segments instead of four 90 degree arcs. As I mentioned when I do this same type machining operation on a higher end CAD/CAM using a dome shape I can get arc segments instead of the short line segments.

A couple things come to mind. Possibly clipart domes are not perfectly hemispherical. Or the dome slicing algorithm is not exact. Looking at the generated Gcode (short line segments) for a single circular toolpath I noticed the Z value will vary by +/- .0001" or more. That variation in Z value would indicate the circular toolpaths are somewhat wavy and not single plane arcs, constant Z level, as might be expected.

Just for fun I imported a CAD generated dome into v12 Desktop. Same situation, the circular toolpaths have that wavy variation in Z value. That would imply the Vectric slicing algorithm is not exact.

Thoughts?

BTW, I grew up with CNC starting with my first purchase in the mid 1980's of a machine with only 8K memory so compact code was always an issue. These days the PC based controls have practically no limit to the size of Gcode files.

User avatar
dealguy11
Vectric Wizard
Posts: 2536
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510,24x48 GCnC/WinCNC
Location: Henryville, PA

Re: Looking for a Post Processor to use arcs instead of lines...

Post by dealguy11 »

3d objects in Vectric are made up of 3d pixels. Each pixel is a point with a height. The 3d finishing toolpath is interpolating between those 3d pixels and doesn't see a circle or arc, it sees a bunch of moves between pixels. That's what you will always get with a 3d finishing toolpath, by design.

A toolpath that should produce arcs in this situation (I think) is the moulding toolpath. A dome is pretty easy to create with the moulding toolpath and I don't think it produces lots of short segments, but to be honest I'd have to look and see.

Having said that, there should be settings in your controller that look ahead and smooth out the movement on those short segments.
Steve Godding
Not all who wander (or wonder) are lost

User avatar
adze_cnc
Vectric Wizard
Posts: 4484
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Looking for a Post Processor to use arcs instead of lines...

Post by adze_cnc »

dealguy11 wrote:
Wed Apr 24, 2024 9:39 pm
A toolpath that should produce arcs in this situation (I think) is the moulding toolpath.
Should and does.

Doug98105
Posts: 45
Joined: Thu Feb 04, 2016 3:48 pm
Model of CNC Machine: Centroid knee mill with 4th axis

Re: Looking for a Post Processor to use arcs instead of lines...

Post by Doug98105 »

WOW, who woulda thought......?

A moulding tool path of all things?..... It does indeed create arc type Gcode.

Thanks you two guys.

User avatar
dealguy11
Vectric Wizard
Posts: 2536
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510,24x48 GCnC/WinCNC
Location: Henryville, PA

Re: Looking for a Post Processor to use arcs instead of lines...

Post by dealguy11 »

FWIW, one more thing that I'm surprised Gary didn't point out was that your controller converts ALL arc moves to tiny little straight segments before it sends the output to the motors to be executed. The g-code for an arc is an abstraction layer that allows you to define the move with a single human readable line, which is converted by the controller to thousands of machine-readable motor instructions. The thousands of lines you see in the g-code file do need to be interpreted, so there is a small amount of overhead for that, but they were going to end up as thousands of instructions anyway.
Steve Godding
Not all who wander (or wonder) are lost

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 986
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 12.007
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: Looking for a Post Processor to use arcs instead of lines...

Post by Tex_Lawrence »

dealguy11 wrote:
Thu Apr 25, 2024 1:39 am
... The thousands of lines you see in the g-code file do need to be interpreted, so there is a small amount of overhead for that, but they were going to end up as thousands of instructions anyway.
Have you heard of any estimates (perhaps from manufacturers of the controllers) of the difference in calculating from "lines you see in the g-code file" instead of a "toolpath that ... produce arcs"?

I'd suspect there might be a significant difference in some controllers; enough to make one decide to use one way or the other.
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

User avatar
TReischl
Vectric Wizard
Posts: 4766
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: Looking for a Post Processor to use arcs instead of lines...

Post by TReischl »

All controls have what is commonly referred to as a control loop cycle time.

Pretty simple really. When cutting the control is running in a loop. In that loop it is doing things like checking if the E stop has been pressed, a limit switch tripped, see if the machine has reached commanded position, etc. Only a portion of that loop is looking at actual motion.

Years ago we ran a test. Thousands of very short line segments, very high feedrate. It would take a bit before the control look ahead buffer would become depleted and the machine would start moving in short jerky motions.

During my career, it always surprised me how the control companies tended to buy the cheapest chips they could get. Like running an 8086 when much faster chips were available. Eventually the explanation I heard was that a lot of the control software was written in assembly for performance, so redoing that for newer chips was fairly costly. Didn't sound right to me then, doesn't sound right to me now.

Soooo, I have a tendency to run machines from computers that I purchase, not standalone controls that get to choose what cheap chips they want to use. Probably does not make any difference but it makes me feel better.
"If you see a good fight, get in it." Dr. Vernon Johns

Doug98105
Posts: 45
Joined: Thu Feb 04, 2016 3:48 pm
Model of CNC Machine: Centroid knee mill with 4th axis

Re: Looking for a Post Processor to use arcs instead of lines...

Post by Doug98105 »

My use of Vectric software may be a little different than typical users. I have a busniness with a number of production CNC machines. Vectric is nice because for some simple tasks it's much easier and faster than higher end software.

Another reason besides the possible jerky motion with the short lines is the arc commands make the Gcode very easy to read and trouble shoot. Often I like to edit/modify Gcode to improve something. It's very easy to find in the Gcode four arcs comprising a 360 degree circular toolpath than 1500 short line segments.

The Centroid control has macro programming with "if/then" type statements and user variables so you can do some real tricks with it. Also powerful conversational programming to write a program standing in front of the machine on the shop floor..

ElevationCreations
Vectric Craftsman
Posts: 187
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Looking for a Post Processor to use arcs instead of lines...

Post by ElevationCreations »

IslaWW wrote:
Wed Apr 24, 2024 1:29 pm
The supplied postP for Vectric does support arcs as Adrian mentions, but only in the G17 plane. Vectric does not support arcs in the G18 or G19 planes. That said, you may want to look at your smoothing settings if you are not happy with machine motion while cutting concave or convex shapes.
As Gary mentions, you may want to look at the Smoothing settings in the Centroid controller. You can search for it on the Centroid Forum, one of the users posted a very helpful document on how to set up and adjust the settings in the controller.

User avatar
IslaWW
Vectric Wizard
Posts: 1409
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Looking for a Post Processor to use arcs instead of lines...

Post by IslaWW »

dealguy11 wrote:
Thu Apr 25, 2024 1:39 am
FWIW, one more thing that I'm surprised Gary didn't point out was that your controller converts ALL arc moves to tiny little straight segments before it sends the output to the motors to be executed.
Gary figures that after he tells that to a hundred folks, that some of them will carry the torch into the future. :D
Post processing with the Centroid inch PP gives hundreds or thousands of short line segments instead of four 90 degree arcs. As I mentioned when I do this same type machining operation on a higher end CAD/CAM using a dome shape I can get arc segments instead of the short line segments.
Many of those higher end CAM engines were designed around the limitations of the legacy controllers they were feeding. You can set them to place an arc (very small radius) where there are intersecting lines, i.e., software smoothing. The inverse of exact stop. Software smoothing is for machine controllers that don't have their own smoothing built in. Today's controllers have much more advanced trajectory planners.

Here's the deal..... CNC machines, you know, the tools we buy that cut the most awesome curves and arcs, are not capable of anything but moving in a straight line. From one XY coordinate to the next XY coordinate in a straight line. All circular cuts are executed by the machine's controller as hundreds, if not thousands of straight line segments, most of which are only a few thousandths of an inch long. These segments can be generated by either the CAM program (as thousands of line segments) or by the CNC controller.
GCode arcs were invented due to lack of RAM in old machines and to save tape or file space. Side benefit is that humans can understand the machine action. In a modern controller there should be no difference in machine action between a file generated with arcs, or interpolated into segments.

I repeat, as I am pretty familiar with the Centroid controller, which has 2000 lines of look ahead AND the onboard processor sends arc and segment instruction back to the CNC-PC for processing and upon return is placed in the cache, IF your Centroid controlled machine responds differently to Vectric generated segments than it does to it's own generated segments, then your smoothing settings are messed up. They are pushed too far towards exact stop for that file type.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

Post Reply