Create a Profile Contouring Operation
Between a Curve and Surfaces

	This task shows how to insert a 'Between Curve and Surfaces' Profile Contouring operation in the program. To create the operation you must define: the Contouring mode as Between Curve and Surfaces the geometry to be machined the tool that will be used the parameters of the machining strategy the feedrates and spindle speeds the macros (transition paths) .
	Open the PrismaticMilling02.CATPart document, then select the desired `Machining` workbench from the `Start` menu. Make the Manufacturing Program current in the specification tree.
	1.	Select `Profile Contouring` . The Profile Contouring dialog box appears directly at the Geometry tab page . This page includes a sensitive icon to help you specify the geometry to be machined. Set the Contouring mode to `Between Curve and Surfaces`.
		The top guiding curve and part bottom in the icon are colored red indicating that this geometry is required for defining the operation. All other geometry is optional.
	2.	Click the red bottom in the icon, then select the bottom surface of the part in the 3D window.
	3.	Click the top guiding curve in the icon, then select the top edge of the part in the 3D window.
	4.	Click the first relimiting element in the icon, then select a vertical edge at one end of the part in the 3D window.
	5.	Click the second relimiting element in the icon, then select the vertical edge at the other end of the part in the 3D window.
	6.	If needed, set offsets on the geometric elements.
		The guide and limit elements of the icon are now colored green indicating that this geometry is now defined. These are also indicated on the part.

	7.	Select the Strategy tab page and choose the desired tool path style. You can then use the tabs to set parameters for: Machining such as machining tolerance Stepover (see example below) Finishing High Speed Milling.
		A tool is proposed by default when you want to create a machining operation. If the proposed tool is not suitable, just select the Tool tab page to specify the tool you want to use. This is described in Edit the Tool of an Operation.
	8.	Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
	9.	Check the validity of the operation by replaying the tool path.
		You can add approach and retract motions to the operation in the Macros tab page . This is described in Define Macros of an Operation. When macros are used, the surface selected as bottom is checked for collisions.
	10.	Click OK to create the operation.
	More About Profile Contouring Operations Multi-Edition You can modify the parameters of two or more Profile Contouring operations in one shot by means of the `Selected Objects > Definition...` contextual command. See Editing Parameters of Several Profile Contouring Operations. Collision Checking A Collision Checking capability is available in the Geometry tab page, which allows collision checking between the tool and guide elements during macro motions. See Reference section for more information.