Views, Planes, and Coordinate Systems
Mastercam uses a 3D Cartesian coordinate system to locate your work in three-dimensional space. This means that geometry and toolpath positions are expressed in terms of three coordinate axes—X, Y, and Z. Each axis is signed, which means that it has a positive and a negative direction.
Because machining jobs often require you to work with coordinate locations in sophisticated ways, Mastercam includes several useful tools which let you transform, overlay, slice, and otherwise manipulate the coordinate system so that you can draw and machine your part in ways that make sense to you.
Options in the Planes Manager define the perspective from which you are looking at the part in the graphics window. There are nine pre-defined views. These views can be associated to planes, but that is not necessary. You can view the part from a perspective that is not your construction plane.
For example, you can be looking at the part in isometric view, while drawing geometry on the front of the part. The default plane, Top, corresponds to the standard XY plane for simple 2D geometry.
Use the Planes Manager to orient the graphics view. You can also use the functions in the Graphics View group of the View tab.
The main tool for applying coordinate systems in Mastercam is the plane. A plane consists of two main parts:
- A slice through the coordinate system
- An origin, or zero point
Planes have names, so they can be saved with the part and selected at a later time. Every Mastercam part includes, by default, nine planes. These correspond to the six faces of a cube (Top, Front, Back, Right, Left, Bottom), as well as an Isometric, Reverse Isometric, and Trimetric plane. In addition, you can create your own planes, name them, and save them.
The most important applications of planes include:
- The construction plane (Cplane). This is the plane in which new geometry is created.
- The tool plane (Tplane). This is the cutting plane for a toolpath, typically normal to the tool axis.
You choose one of these functions, and then select a plane to apply to it. To draw geometry on the back of your part, choose the Cplane function and select the Back view. To machine a contour on the front of your part, choose the Tplane function and select the Front view.
Because Mastercam breaks these out into separate functions, you can maintain the plane selections for each function independently. For example, you can be looking at the part in isometric view (Gview = Isometric), while drawing geometry on the front of the part (Cplane = Front). The default plane, Top, corresponds to the standard XY plane for simple 2D geometry.
Use the Planes Manager to set tool and construction planes. For most applications, you will want these to be the same, so this function sets both at the same time.
Mastercam also lets you shift and move the coordinate axes themselves. This lets you create a work coordinate system (WCS), which lets you move the coordinate system to your part geometry instead of moving or transforming the part geometry. Think of the WCS view as defining the "Top plane" relative to your part.
For example, an aerospace part might be drawn and dimensioned to the tip of the nose or wing. You can use the WCS to align the coordinate axes and origin with the part before creating the toolpath. Then, when you post the toolpath, the NC code will look like the part is flat so you can machine it simply.
Or, you can create different WCS's for different part fixtures and assign work offsets to each one, so that when you post the toolpaths each will start at the zero point with the proper work offset code included automatically.
Gviews, Cplanes, and Tplanes are all measured relative to the WCS and its origin. However, you change the WCS in exactly the same way that you change those functions: create a view or plane which captures the orientation and origin that you desire, and then set the WCS equal to it.
You should not use the WCS or custom views to model your machine tool or axis orientation—for example, rotating the coordinate system for a horizontal mill, or tilting it for your slant-bed lathe, or turning it around to machine at a different spindle. Instead, use the machine definition to do this.
Mastercam maintains a separate coordinate system, called the world coordinate system, that is used to model your machine tool. Use the machine definition to tell Mastercam how the axes of your machine tool are physically laid out and oriented - for example, the orientation of the Z axis on a horizontal mill. When you create your toolpath and select your tooling, Mastercam will also know about axis combinations, turret and spindle orientations, and how tools are mounted. This information is available to the post processor when you post the toolpath.
By separating machine-dependent coordinate systems from your part geometry, Mastercam makes it possible for you to move a part file transparently from a vertical mill to a horizontal mill, or from one spindle of your lathe to another, without having to manually transform the coordinate system in your part file.





