Facing

	This task shows how to insert a Facing operation in the program. To create the operation you must define: the geometry to be machined the tool that will be used the parameters of the machining strategy : the proposed tool path styles are: Inward helical, Back and forth, and One way the feedrates and spindle speeds the macros (transition paths) .
	Open the PrismaticMilling01.CATPart document, then select `Machining > Prismatic Machining`from the Start menu. Make the Manufacturing Program current in the specification tree.
	1.	Select `Facing` . A Facing entity along with a default tool is added to the program. The Facing dialog box appears directly at the Geometry tab page . This tab page includes a sensitive icon to help you specify the geometry to be machined.
		The part bottom and flanks in the icon are colored red indicating that this geometry is required for defining the operation. All other geometry is optional.
	2.	Right click the red Bottom in the icon and select `Contour Detection` from the contextual menu. Click the red Bottom then select the underside of the part in the 3D window. The part boundary is automatically deduced thanks to the Contour Detection option. This is indicated by the highlighted Drive elements.
		The bottom and flanks of the icon are now colored green indicating that this geometry is now defined.
	3.	Select the Strategy tab page and choose the desired tool path style: Inward helical, Back and forth, or One way. You can then use the tab pages to set parameters for: Machining such as machining tolerance Radial strategy (see example) Axial strategy (number of levels = 1, for example) Finishing High speed milling (for Inward helical tool path style only).
	4.	Select the Tool tab page to replace the default tool by a more suitable one.
	5.	Select the `Face Mill` icon. A 50mm diameter face mill is proposed. You can adjust the parameters as required. See Edit the Tool of an Operation for more information about selecting tools.
	6.	Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
	7.	Select the Macros tab page to specify a return macro, which is necessary for the One Way mode. In the Macro Management frame, right-click the `Return in a Level Retract` line and select the `Activate` contextual command. In the Current Macro Toolbox frame, select the Axial mode. A sensitive icon representing this retract motion is displayed. Double click the distance parameter in the sensitive icon and enter the desired value in the pop-up dialog box. Select the Return in a Level Approach line, the repeat the procedure to specify the approach motion. See Define Macros of an Operation for another example of specifying transition paths on a machining operation.
		Before accepting the operation, you should check its validity by replaying the tool path.
	8.	Click OK to create the operation.
		In this scenario the operation used the default start point (that is, the origin of the absolute axis system). If you want to define a different start point, you can click the start point symbol in the sensitive icon then select a point. Please note that the exact position of operation's start point may be different from your selected point. The program will choose the nearest point from a number of possible start positions.

Create a Facing Operation