CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Software > FUSION 360

Reply
 
Thread Tools Display Modes
  #1  
Old 04-28-2019, 07:37 PM
Dan Schmidt Dan Schmidt is offline
CAMhead Friend
 
Join Date: Mar 2018
Posts: 14
Default WINCNC Errors

I'm having lots of trouble with the Fusion360 WINCNC post. I am using wincnc_atc.cps from http://wincnc.net/webfiles/Post%20Pr...DeskFusion360/.

Below is a short GCode file with a simple drill operation and a 2D pocket. When I try to open the file in WINCNC, I get "Error - Multiple Commands". Can you tell me what looks off? Any tips on how to debug a gcode file when it fails loading into WINCNC?

[1001]
[DP Tray]
[T3 D=0.375 CR=0. - ZMIN=0.1575 - flat end mill]
G90
G20
G53
[2D Pocket4]
T3
S18000
M3
G0 X1.2318 Y3.7756
Z1.3386
Z0.9449
G1 Z0.8465 F130
Z0.1575 F65
G3 X1.2968 Y3.7106 I0.065 J0. F130
Y3.8406 I0. J0.065
X1.2318 Y3.7756 I0. J-0.065
G1 Z0.195
G0 Z1.3386
X2.2187
Z0.9449
G1 Z0.8465 F130
Z0.1575 F65
G3 X2.2837 Y3.7106 I0.065 J0. F130
Y3.8406 I0. J0.065
X2.2187 Y3.7756 I0. J-0.065
G1 Z0.195
G0 Z1.3386
X3.2682
Z0.9449
G1 Z0.8465 F130
Z0.1575 F65
G3 X3.3332 Y3.7106 I0.065 J0. F130
Y3.8406 I0. J0.065
X3.2682 Y3.7756 I0. J-0.065
G1 Z0.195
G0 Z1.3386
M5
G53
__________________
Dan Schmidt
  • PT404 Panther w/ 3kW spindle
  • Cyclone Vacuum System
  • Indexing Lathe
  • FTC/Laser/Assist/Remote
  • Fusion 360 / Vectric V-Carve Pro
Reply With Quote
  #2  
Old 04-28-2019, 08:25 PM
Ken Rychlik Ken Rychlik is offline
CAMaster Owner
 
Join Date: Jun 2011
Location: SW Houston
Posts: 78
Default

The G3 move is an arc requiring x y and radius info.
The line below it is just a Y with a radius. To me that doesn't look good. You can't have an arc move with just one axis moving.

After is does any type of move like a G1 move command, any command below that without calling a different type of move is going to be considered a G1

So with the move after the g3 arc move, it is confusing.

I would delete the line after the G3 moves and see if it loads. Not to run the file, but to see if that's it.
__________________
Fixing machines and making sawdust.
SW side of Houston
Reply With Quote
  #3  
Old 04-28-2019, 08:39 PM
Charlie_L Charlie_L is offline
Stinger II Owner
 
Join Date: Mar 2012
Location: Wisconsin
Posts: 1,490
Default

I experimented and found that the simulation in WinCNC didn't like having the G3 commands, without the G3 in front of the x y I commands. Just like Ken explained. Maybe adding a G3 works?
__________________
Charlie L
Stinger II, 48 by 48, 1.7 kW Spindle, FTC + Laser + Recoil + Vacuum, July 2012
WinCNC 2.5.03, Aspire 9, PhotoVCarve, Windows 7 Pro SP1
Reply With Quote
  #4  
Old 04-28-2019, 09:15 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Consultants and Trainers
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,948
Default

Add the line: "g2modal=1" (without quotes) to the WinCNC.ini file and see if that works

If you have input parameters in Fusion 360, you maybe able to check, or enable G2/G3 modal/nonmodal or force the G2/3 commands to be placed on every applicable line
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"

Last edited by Gary Campbell; 04-28-2019 at 09:17 PM.
Reply With Quote
  #5  
Old 05-01-2019, 10:59 PM
Dan Schmidt Dan Schmidt is offline
CAMhead Friend
 
Join Date: Mar 2018
Posts: 14
Default

Thanks to each of you for your replies.

Ken, deleting the lines after the G3 moves resulted in "Error - Radius" when loading the file.

Charlie, when I added G3 in front of the lines as you suggested WORKED!

Gary, I was concerned that I'd have to learn and modify the post. The g2modal=1 setting worked perfectly!

You guys are awesome!!!! Thank you!

Dan
__________________
Dan Schmidt
  • PT404 Panther w/ 3kW spindle
  • Cyclone Vacuum System
  • Indexing Lathe
  • FTC/Laser/Assist/Remote
  • Fusion 360 / Vectric V-Carve Pro
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 09:35 AM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2019, Jelsoft Enterprises Ltd.