New to V-Carve Pro

This forum is for general discussion regarding VCarve Pro
Post Reply
lakemfg
Posts: 1
Joined: Tue Feb 11, 2020 7:44 pm
Model of CNC Machine: shopbot

New to V-Carve Pro

Post by lakemfg »

Hi, I just purchased v-carve pro software and am having a hard time figuring out how to get the fonts to become smooth? I am familiar with g-code programming and am stumped as to why when I save the tool paths for say a letter "O" that it saves it with a g-code of G1 and not G2or a G3.....???
I have tried....watching a bunch of videos, changing nodes to curves, used different fonts, different post processors but haven't found anything that works. My gantry is solid and have done perfect circles (machine cost around $10,000/$20,000 when new)....just doesn't do fonts smooth...….!!!!
There has to be a simple answer!!! Can somebody please, please help me before I go crazy.

User avatar
scottp55
Vectric Wizard
Posts: 3573
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: New to V-Carve Pro

Post by scottp55 »

How big are fonts you're trying it on? (Less than .25" height and you get into a small different world on settings)

Can you show an example cut in your material please?

Which machine is it? I take it you bought used? (I have ballscrew, but Pinion gears are considered consumables...check for slop?)

If preview is smooth in Vectric...PP problem(?)(do a UR for Your machine also?)...then it's a machine problem, and a pic can help us.
scott
"One accurate measurement is worth a thousand expert opinions"

GMH


scott

User avatar
Adrian
Vectric Archimage
Posts: 10225
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: New to V-Carve Pro

Post by Adrian »

All depends on how the font is constructed. If it's made of arcs and you're using a post processor that supports arcs then it will have G2 G3 commands in the code. Otherwise it will be output as short moves.

Smoothness should be nothing to do with the output though. My machine cuts letters comprised of bezier curves identically to ones comprised of arcs.

Have you zoomed right into the letters while in node edit mode? In my experience a lot of fonts look smooth to the eye but when you get in close the nodes are all over the place. No problem for screen display on web pages and type etc but no good for a CNC cut. You can use the "Fit curves to selected vectors" tool to smooth out the lines and/or convert to arcs etc.

User avatar
TReischl
Vectric Wizard
Posts: 3330
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: New to V-Carve Pro

Post by TReischl »

Just so you know. . . . a cnc machine operating in X,Y,Z cannot cut a true arc. A G2/G3 move is broken down internally into extremely small straight line segments. The only place you can cut a true circle on a cnc machine is on a rotary axis.

Can you post a pic of one of the fonts you are having an issue with showing the straight line segments? It will be helpful if you can tell us the font name, too.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
wmgeorge
Vectric Craftsman
Posts: 273
Joined: Sun Nov 23, 2008 6:12 pm
Model of CNC Machine: Fine Line Automation Saturn 2 4x4 ESS

Re: New to V-Carve Pro

Post by wmgeorge »

TReischl wrote:
Sun Feb 16, 2020 2:47 pm
Just so you know. . . . a cnc machine operating in X,Y,Z cannot cut a true arc. A G2/G3 move is broken down internally into extremely small straight line segments. The only place you can cut a true circle on a cnc machine is on a rotary axis.

Can you post a pic of one of the fonts you are having an issue with showing the straight line segments? It will be helpful if you can tell us the font name, too.
Even if my Mach4 Post processor says arcs and curves?

User avatar
IslaWW
Vectric Wizard
Posts: 1291
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

Re: New to V-Carve Pro

Post by IslaWW »

wmgeorge wrote:
Thu Feb 20, 2020 6:45 pm
Even if my Mach4 Post processor says arcs and curves?
In reality G2/G3 (Gcode arc) commands, although relevant, are a bit of a holdover from yesteryear. They simply reduce the lines of code required to cut an arc in a given file.

All circular or curved cuts are performed by the machine executing a series of very short straight segments. These segments are either generated by the post processor (no arc type postP's) or in the machine controller itself (arc type postP's). In any case a cnc machine is incapable of making a curved move. They ONLY make straight point to point moves.

The difference to the user comes in when the controller does not handle the externally created segments as well as those created internally. In most cases using modern controllers there is no perceivable difference in speed or quality unless the difference in segment length is noticeable. This is a product of better controllers with more lookahead. 2000 lines being the current norm for quality controllers.
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com

User avatar
TReischl
Vectric Wizard
Posts: 3330
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: New to V-Carve Pro

Post by TReischl »

Exactly what Gary said.

Here is my take on the situation. Unless you are running an antique control there is every reason to NOT get hung up on arcs thinking they will be the smoothest curves you can cut. Bezier and other mathematically defined curves are much more flexible (pun intended) than circular arcs. A good example is automobile body work. You would have a hard time finding a circular arc since they are not designed with arcs to begin with.

Like pretty much everyone else I thought that two arcs tangent to each other was the smoothest transition possible. Turns out that is not the case. But it is a long winded subject that I only partially understand.
"If you see a good fight, get in it." Dr. Vernon Jones

Post Reply