CNC Simulator

From ShapeOko
Jump to: navigation, search

Overview

CNCSimulator Windows program to simulate and test G-code before sending to the machine.

CncSimulator.jpg

Downloading

Download from CNC Simulator web site.

Using CNC Simulator

Load Machine

Select File-->Load Machine to pick a type of mill (or lathe). The "Router Table" works well to simulate ShapeOko.

CncSimulatorSelectMachine.jpg

Create Tools

You need to create your end mills for the simulator to use. Select Settings-->Machine Tools to bring up the tool browser.

CncSimulatorToolBrowser.jpg

Select Add or Edit to create your tools.

Note: Notice the index of your tool. In this picture 1/1 means tool index 1 (out of 1 tools). We'll need this index number later.

Workpieces

You need to create a workpiece to mill. Select Settings-->Workpieces-->Mill to bring up the Mill Workpiece Form.

CncSimulatorMillWorkpieceForm.jpg

Edit, or select the "+" to create additional workpieces.

Note: Notice the index of your workpiece. In this picture 1/1 means workpiece index 1 (out of 1). We'll need this index number later.

Creating New Materials

If you'd like the material in the simulator to look like the material you're milling, you need to create the material. Select Settings-->Simulation Settings.

CncSimulatorSettingsEditor.jpg

Click the [...] next to Materials (Collection) to create a new material.

CncSimulatorMaterialCollectionEditor.jpg

Load G-code

Select File-->Open CNC file to load your g-code.

Modifying G-code

Select File-->Open CNC file to open your g-code. You need to add a few lines to the top.

($Inches) (Alarm if not inch machine)
($Mill) (Alarm if not a milling machine)
($AddRegPart 1 0 0)
G92 X4 Y4 Z0.2
T1 M6

($Inches) and ($Mill) are CNCSimulator commands to ensure things are setup properly.

($AddRegPart 1 0 0) is a CNCSimulator commend that says to use workpiece index 1 (see Note above), and place it at x=0, y=0 on the mill.

G92 is a g-code command that tells the mill, relative to the mill origin, the origin of the workpiece. In this example, G92 X4 Y4 Z0.2, the g-code should start 4" in on the x-axis, 4" in on the y-azis, and 0.2" above the z-axis.

T1 M6 is a g-code command that tells the mill to use tool index 1 (see Note above), and M6 tells the virtual machine to go to its tool change position and execute the tool change.

Running the Job

Press the play button at the bottom of the screen to start running your simulation.

  • Dragging the simulation window with the left mouse button allows you to change viewing angle.
  • Dragging the simulation window with the right mouse button allows you to change viewing position.
  • The mouse wheel allows you to zoom in and out on the simulation.