Smoothing not working correctly??

[JeffreyTKomorowski]

I'm currently drawing parts on Fusion doing only 2d work on a plasma cutter that I have. The problem I have is that once I got through the whole process the GCode that is generated only consists of straight lines no arcs. My tolerance for smoothing is at .01mm 

Below is a clip of the G code I'm getting. I have been following this video on youtube and when he sets it up and shows his Gcode he has the arcs working so I'm not sure why it is not working for me. I did the exact same design and followed his steps exactly. 

The originally was using a SVG file I designed in inkscape and imported it but I thought it could be because the SVG file was imported and made up of tiny lines. Like I said I ended up redoing what was posted in the video mentioned and designed the part IN fusion but am still having issues.  

Youtube video with smoothing working in Gcode: https://www.youtube.com/watch?v=63irIPuvPwg

[seth.madore]

Could you share that model? What post are you using, as some post processors ONLY produce point-to-point moves (limitations of the controllers they're written for)

[JeffreyTKomorowski]

I'm not sure how to share the model. Im in the process of trying to figure out how to set up a post somewhat. I am running off my dad's industrial waterjet that he scrapped down and added his plasma cutter to to make it cnc plasma cutter. It has a centroid controller but I did not see centroid on the list for posts. My dad suggested I use Baileigh Plasma.

below is a picture of the controller. Using an Allin1DC board as I looked up in the books and confirmed by my dad. 

EDIT: I think I found out how to share. Link below

https://a360.co/3USrtD8

[seth.madore]

If you're on a Personal account, you are not able to share the file through that method. You will need to open the file in Fusion, click on File and then Export > Save to local folder, return to thread and attach the .f3d file  in your reply:

 

[JeffreyTKomorowski]

Correct attachment for review 

[seth.madore]

The first question: are you certain that your machine supports G2/G3 arc moves?

If so, and you'd like to have more compact code, you have a couple of options:

1) Use a post that gives you better code. I'd start with the Mach3 post processor

2) Edit the Baliegh post to output arc moves.

I think with either route you go, you're likely going to find other M codes that are incorrect..

[JeffreyTKomorowski]

I am positive that the machines supports G2/G3 arc movements. With that being said, I was curious how to edit the actual post. I figured I could not do that and needed to change a few commends as my dad has M07 firing his torch and figured I would need to go in the GCode file and manually edit that.

Is there a way to go in an edit a post efficently as you mentioned so I can change some of my codes around. Also how would I edit the Baliegh to output arc moves? Is it an option to turn on and off? Again my dad is positive it allows for G2/G3 arc movements.

[seth.madore]

Oh, editing the posts are rather easy, in most cases. First thing you're going to want to do is download Visual Studio Code and then the HSM Addin that we wrote (read more about that HERE)

Once you've done that, I suggest at least becoming vaguely familiar with the Post Manual as it contains darn near everything you need to know. I'll give you a shortcut though and show you what you need to edit. Change this from a 0 to a 1:

 

But really, get the Visual Studio and the Addin, it makes editing posts so easy, as you can generate sample code right there and not have to bounce back into Fusion to make sure the format is as you want it. Furthermore, you can click on a line in the g-code and it will jump right to the related post text. So, changing M codes and locations of them becomes relatively easy to do

[JeffreyTKomorowski]

Thank you!

[JeffreyTKomorowski]

do you still recommend trying to use the mach3 post over the Baleigh. I'm still learning and new to this so I don't know if one would be preferred over another.

[seth.madore]

Not necessarily, I'd compare the outputs of the two and see which one gets you close to your final goal (aside from changing the "allowedCircularPlanes")

[JeffreyTKomorowski]

So I am following the directions and I already had VS code installed. When I tired to install the post processor utility extension from VS code, I downloaded it, restarted VS and for some reason its not registering that I have the extension downloaded. I got to the part where it wants me to search HSM in the settings but no extension comes up. 

One of the things I did notice was that my cps file is not a javascript file. 

[seth.madore]

When you click on the Addins button, do you see this?

 

[seth.madore]

And I suspect it's intended that you use the left hand menus now, instead of the F1 commands:

 

[JeffreyTKomorowski]

I was able to download the .cps file for the baleigh as well as the mach3. As I mentioned when I open the file in VS code its in a text file. I can change it to JS at the bottom I just find it strange its not originally opened as JS. Anyway once it's in the JS file I do not see any of the information on the left hand side. I can't F1 search the HSM extension noting comes up. 

With all that said, I was able to go into the .cps file and find the location for the allow curves and changed it to one. It did change my code with the tab I sent using M2 and M3. I've exported and attached a copy.