G-Code output for cutting arcs and circles

Post by **FastCote** » Thu Jul 13, 2006 2:35 am

I have been crazy-excited to get my hands on VCarve and I finally bought myself a copy. I hate to make my first post a negative one, but I was disappointed to find that all G-Code produced is in the form of linear moves (G1). I guess I assumed it would produce G2 and G3 moves for arcs and circles.

Admittedly I may be mis-using VCarve, but my main interest at the moment is to turn a bunch of DXF files into G_Code. VCarve has excellent tool offset capabilities (cut inside, cut outside, pocket) that are dumb-easy to use. That, combined with the automatic multi-pass you get from the tool settings make it wonderful. The only disappointing part is the lack of natural arcs in the output files. With my crappy home-grown CNC, the difference is obvious. All those linear moves to make a circle make my machine vibrate at high speeds.

It their a post-processor choice I could be making to get different G-Code output? I am using the latest Mach3 release, so I tried both the Mach2/3 post processor as well as the generic G-Code option.

I am still happy to have made this purchase, as VCarve Pro give you more bang for the buck than anything else out there.

Thanks for all the hard work and attention to detail.

Ben.

Post by **Jason Marsha** » Thu Jul 13, 2006 6:36 am

I have a home built machine and the linear moves are not even nearly obvious, the linear moves should not result in vibration if your machine in CV mode (constant velocity).

Jason

Post by **CRFultz** » Thu Jul 13, 2006 10:57 am

Ben,
Welcome to the Vectric forum.

Like yourself and Jason, I to have a home built CNC running Mach 3. I only run at speeds between 30 and 60 but I haven't had any problems that you spoke of. The circles that have been cut have been nice and smooth.
Like Jason said....maybe constant velocity mode might work for ya.
Good Luck!

Chuck

Post by **dighsx** » Thu Jul 13, 2006 11:50 am

I too am running a home built machine and if I showed you a something cut with G2 and G3 codes and something created without them, you wouldn't be able to pick which was which.

What feed rate are you running at and has your machine cut circles and thing of this nature smoothly before?

Post by **FastCote** » Thu Jul 13, 2006 2:06 pm

You guys are great. It is a pleasure to have this many polite and helpful folks available to newcommers like me. I have tried the attached piece at 60 ipm and 80 ipm. In both cases i either get real jerky arcs (if my acelleration is rapid) or way-slow arcs (with a gentler acceleration) depending on motor tuning in Mach3. the straight runs manage to get up to the feed rates, but the arcs get to 8-12 ipm.

I'm not sure if im in CV mode in Mach or not. I am not sure what other issues CV mode implies. i guess that is a better question for the Mach forums. When i import this same piece using the LazyCam app that comes with Mach, i get G2/G3 and the arcs cut at or near feed rates, but i would MUCH prefer to use VCP as my only CAM solution.

By the way, this item to be cut is one of many MANY pieces from JoeChevy's 2006 CNC machine. I hope he does not mind me using it for demo purposes. His machine(s) and his efforts are what got me interested in DIY CNC. if you have not seen his stuff, you should.

http://www.cnczone.com/forums/showthread.php?t=15139

Thanks again,

Ben

Post by **BrianM** » Thu Jul 13, 2006 2:21 pm

Hi Ben,

We had hoped to get support for G2 and G3 into the intial release of VCarve Pro but we unfortunately ran out of time. We have done the 'donkey work' at a lower level but there is obviously testing to be done with each updated post processor and at least one willing volunteer

before we can release a new VCarve Pro and updated post processors.

I am working on this at the moment (it was also requested here http://vectric.com/forum/viewtopic.php? ... hlight=g02 ) and may have something to play with by the weekend or early next week.

I am however suprised that it is making such a difference on your machine. Our experience with most modern controlers has been the same as the others that have posted here - the files sizes are larger but the control software usually has no problem creating a smooth path through the linear representation. For the VCarving toolpaths G2/ G3 support makes no difference as the VCarving moves do not contain any circular arcs.

When it is ready we will release it in the first free service update for VCarve Pro V3 and let all registered customers know.

Regards

Brian

Post by **dighsx** » Thu Jul 13, 2006 2:39 pm

Ben,
I just ran the code created from your file at 75ipm and didn't have any slow downs. What speed is the computer that you have Mach3 running on? I'm wondering if it's just not fast enough to get the data out at the rates you want? It's a long shot but maybe?

Post by **FastCote** » Thu Jul 13, 2006 3:43 pm

My machine is a P4 - 2.6. I Think it is ok.

I am actually hoping that Jason was right about NOT being in constant velocity mode. I am not sure why i would have switched that off, but it is entirely probable (there are only 16 bazillion settings in Mach3)

It is bugging me enough I may have to leave work early to go find out!!!!

Post by **FastCote** » Thu Jul 13, 2006 3:46 pm

Brian,

If that was a solicitation for a guinea pig, I’m your man. I actually sent Tony an email about beta testing, but that was before I actually purchased. I am more than willing to beta anything you would like to throw at me.

Post by **Jason Marsha** » Thu Jul 13, 2006 9:58 pm

To ensure you are in CV mode, open Mach3, CONFIG > STATE > Select Constant Velocity check box.
Good luck.

Jason

Post by **FastCote** » Fri Jul 14, 2006 10:54 am

Well, constnat velocity took away the jerkieness (thanks Jason), but my corners are so far from square its almost funny. i think there is a way to tell Mach to do CV on mild angles and exact stop on sharp ones. Ill try and figure that out. I see a setting in the settings tab, but its less than intuitive.

Thanks again everyone.

Post by **BrianM** » Fri Jul 14, 2006 10:58 am

Hi Ben,

I think I have the circular arc support working now so I might drop you a mail in the next few days to take you up on your testing offer if you dont mind.

However, it would be worth perseveringwith your CV experiments as these settings will still be important if you are machining curves which are not composed of simple arcs.

Cheers

Brian

Post by **FastCote** » Fri Jul 14, 2006 11:26 am

Thanks Brian. It's like Christmas every day around here!!!

Post by **dighsx** » Fri Jul 14, 2006 12:48 pm

What are you using to control your motors? (geckos, xylotex, etc...)

Post by **FastCote** » Fri Jul 14, 2006 1:04 pm

Mach3 (parallel port, not Gecko) and the HobbyCNC $AUPC board. http://www.hobbycnc.com/4aupc.php.