CNCSimulator Pro

user guide

12.1.15. More about contours

There are two more ways of creating contours. Besides tracking guides you can also create contour rectangles and create contours by [Follow mouse].
If you create contours with these two functions, no arcs will be created. This is not a problem though as we have functions to modify the contour too (adding arcs to corners for example).
Two contours, the upper one created with [Follow mouse] and the bottom one with [Rectangle].
If you click on a contour you will see a popup menu. In that menu we have functions to modify the contour in various ways.
Let's start from the top going down.


Here you can select if you want to delete the whole contour or just the last object. Please note that if you want to delete the first object in the contour, you can just reverse the contour by using the function [Reverse contour]. If you select [Segment only], only an unconnected part of the contour can be deleted. We call parts of the contour, that are not connected to the rest of the contour (can show up for example after a DXF import or after you merge layers) for segments.


You can move a contour. First click the point you want to move from, and then where you want to move to.
If you hold down the SHIFT key on the keyboard when you click the new position of the contour, a copy will be created.
You can also type in the new position using the coordinate bar that will be shown at the bottom of the SimCam screen.


With this function, you can rotate the contour around any point.
Same here, you can hold down SHIFT to make a copy.
The angle can be entered at the bottom of the SimCam screen.


To mirror a contour, you need to create a guide line to be used as the "mirror".
Here we created a mirrored contour holding down shift to make a copy.


Used to scale up or down a contour. If you want to make the contour double the size, enter 2 in the scale value input box shown. If you want to make it half the size, put 0.5 in the box. The scaling will be done around the contour origin (see Origin below).


When a new contour is created, the origin of it will be X0 Y0 (X0 Z0 in Lathe machines).
The origin of the contour will affect scaling operations. Origins are also important when creating lathe tools.
With this function, you can move the origin of the contour to a place that makes more sense to you.
The origin is shown as a small green/orange dot when you hold the mouse over the contour.


Click near a corner where you want to add a fillet radius. Select [Modify] - [Fillet] and enter the radius in the Radius input box at the bottom of the SimCam screen and press Enter.


Click near a corner where you want to add a chamfer. Select [Modify] - [Chamfer] and enter the chamfer distance in the input box at the bottom of the SimCam screen and press Enter.


When importing DXF files or after a merge operation the order of the individual lines and arcs in a contour layer can be messed up. This is where the Optimize function comes in. It will try to find the start of the contour and then order all objects in a subsequent order.

Break apart

If a contour contains several parts that are not connected (segments) you can break it apart so that each segment will be a stand- alone contour. This is useful after importing DXF files or after you have done a merge of layers.


You can append (extend) an existing contour with this function. There are two options, one to use the tracker to follow existing guide lines and circles and the other to follow the mouse.
There is also a shortcut menu you can use to quickly create contour, engraving and pocket milling operations.
If your drawing is made with a well defined contour of drawing objects, more like a conventional CAD drawing, you can use this menu.
Note! Drawing style projects might take slightly longer time to create but are easier to use as a base for toolpath generation. It is up to the user if he/she prefers using guide or drawing objects or a mix of both. We suggest putting dimensions, guide objects and drawing objects in different layers for convenience.
If you click on one of the objects on a drawing contour, you will see a [CAM] menu.
Here are the options in the menu:
[Pocket] This option is only visible when the contour is closed. It will, as the name suggests, create a pocket milling operation using the contour as its borders.
[Contour] This option will create a contour milling operation. If the contour is closed, the tool will go all the way around it. If it is an open contour the operation will stop at the last object (or at an intersection).
[Engrave] This option will automatically create toolpaths for all objects on the layer. It is convenient when you want to engrave everything on the layer with the same tool and parameters.
Let us click on [Contour] and see what happens.
The first thing you will see is a dialog window asking for same basic parameters regarding the operation. Tell SimCam what tool diameter you want, the Z level of the cut and the Z level for transports (usually G00). Then click OK. Please note that you will be able to edit these, and other parameters in the settings for the layer at any time.
Next you will see a window letting you select the toolside as well as the direction around the contour. Changes will preview directly as you click on the buttons. When you are done, click OK.