CNCSimulator Pro

user guide
Index Roughing

To create a roughing operation, you need to have drawn a contour of the part on the layer.
Then draw two points on the layer. These are very important as the points will represent the corner points of the "operation window" or workspace. The first point you draw on the layer will be the starting point of the operation and the second one will be the endpoint (the opposite corner of the operation window).
First double-click on the contour layer (or click its gear button) to open the parameters for the layer. Then make sure you change the layer type to Roughing.
Close the operations parameters dialog by clicking OK.
The layer will be turned red to indicate that it is missing its start and endpoint. Let us add them.
Click [Point] in the SimCam menu and click where you want the rough cuts to start.
The startpoint will be orange with a green outline
Now click again to place the endpoint.
Notice how SimCam draws a rectangle around the operation window.
All work that SimCam will do, will be inside this window. Also, it will be looking in the direction from the startpoint towards the endpoint to decide the cutting direction. In this case, as the endpoint is to the left of the startpoint, the cutting direction will be from the right to the left. Also as the endpoint is lower than the startpoint, it will cut downwards in X.
Open the parameters for the layer again and set values like Depth of Cut, spindle RPM, feedrate, etc. to your liking. Close by clicking OK.
Let us go through the parameters that you can set for a roughing operation.
Contour Cut If you check this option, a final contour cut will be automatically added to the operation.
Zig Zag This option will create a toolpath where the tool goes back and forth in a Zig Zag pattern. Please note that your tool insert needs to be able to cut on both sides for this method to work.
Zig Zag return depth If this value is set to other than 0, the cutting depth for the return cut when using a Zig Zag method will be controlled by this value. Many times it can be practical to use a lower cutting depth on returning cuts to prevent damage on the tool.
Clearance Here you enter the amount of clearance to the final contour. Normally you set a value here to save some stock material for the final fine cut.
Separate X, Z clearance Check this box and enter your values if you want different clearance for the X and the Z-axis.
Cut along axis Here you tell SimCam along which axis it is going to do the length cuts. The most common are length cuts along the Z-axis.