To Machine a Free Form Feature

Unlike other machining strategies in Expert Machinist, Free Form machining does not require creating a feature and then machining it. You define the machining strategy in one step by referencing model geometry (or sketching) and specifying the machining method and options, as needed.

You can also use the Free Form feature just to supply certain CL commands between other tool paths, if needed. In this case, you do not have to specify a tool or define the Drive Geometry. When the Freeform Milling dialog box opens, click Play Path and insert the required CL commands.

1. Click Machining >

Free Form.

The Freeform Milling dialog box opens. The top portion of the dialog box contains two text boxes:

◦ Tool Path Name—The default name for the tool path file, such as FREE_MILLING_TP1. The system will use this file name for NC data output. You can type a customized name. You can also click the Comments button located under the Tool Path Name text box to type the Machine Strategy Comments.

◦ Cutting Tool—The name of the cutting tool. When you use a Machine Tool for the first time within the NC process, there is no active tool and the text box displays None. For subsequent machining, the text box displays the name of the active tool.

The middle portion of the Freeform Milling dialog box contains the options for defining the Drive Geometry and the Machining Method, and the lower portion lists the machining Options. At the bottom of the dialog box there are four buttons: OK, Cancel, Next, and Play Path.

If the Machine Tool has preset cutting tools, select the tool you want by clicking on the drop-down arrow and selecting the tool name from the drop-down list.

To access the Cutting Tool Manager, click

next to the Cutting Tool text box. This functionality lets you create new tools and modify existing ones.

Unlike other machining features, for Free Form machining you can use a sketched tool.

Click Show Tool below the Cutting Tool text box to display the currently selected tool in a pop-up window.

3. Define the Drive Geometry. The Drive Geometry defines the tool trajectory in the XY-plane of the Program Zero coordinate system. You can:

◦ Next to Use Model Edges, click

and select edges from the reference model or from the stock. To verify your selection, click

. The system highlights the selected edges in cyan and indicates with an arrow which side the tool will be on. Click Flip, if needed, to change the side.

◦ Click

next to the Sketch label and sketch the trajectory of the tool in the XY-plane of the Program Zero coordinate system.

4. Define the Cut Depth, that is, the height of the last tool pass. Click

next to Cut Depth and then use one of the CTM DEPTH menu commands:

◦ Specify Plane—Select a planar surface or create a datum plane parallel to the XY-plane of the Program Zero coordinate system.

◦ Z Depth—Type a value along the z-axis of the Program Zero coordinate system.

5. Define the Machining Method and Options, as needed, by selecting options and typing values in the middle and lower portions of the dialog box. Click Play Path at the bottom of the dialog box to display the currently defined tool path.

6. Click OK to complete machining the feature, Cancel to quit. If you want to use the same settings to machine a similar feature, click Next.

When you create a Free Form tool path, the system removes the appropriate stock material, the same as for the other feature types. However, for Free Form features you can specify that the system does not create the automatic material removal. To do this, set the configuration option freeform_toolpath_matrem to no.