Manufacturing > Manufacturing > Manufacturing Process > Operations > Operation Tab
Operation Tab
Set elements for creating an operation using the following tabs.
• Clearance—Provide values for the following optional retract fields on this tab.
Retract—Specify the retract style for the cutting tool.
◦ Type—Specify the retract type for the operation. The retract type may be a Plane, Cylinder, Sphere, Surface, or None. Here, None indicates that a retract type is not defined.
◦ Reference—Specify a reference to use as the origin for the retract type. The reference varies depending on the retract type. It may be a plane, surface, axis, coordinate system or copied from an existing operation. The following options are available on the shortcut menu of this option.
▪ Default Reference—Select to replace the selected reference with the orientation coordinate system.
▪ Information—Select to view the information of the selected reference.
◦ Tolerance—Controls maximum deviation of the tool when it moves along a non-planar retract surface. The default is 0.1" (in English units) or 1 mm (in metric units).
◦ Select Always use Operation Retract to use the operation retract at the end of every step. If you do not select this option, the tool moves to the operation retract only when the tool axis changes.
Alternatively, right-click the graphics window and select Retract, from the shortcut menu.
If you have set up a Mill-Turn or Lathe work center with two spindles, the retract options Type, Reference, and Value are available under the following sections:
◦ Main spindle retract
◦ Sub spindle retract
• Home Point—Specify the start and end positions of the tool. If the work center associated with the operation has four heads, you can set up separate From and Home points for each head. These options appear in the Head 1, Head 2, Head 3, and Head 4 sections of the tab.
◦ From—Create or select a datum point to specify the start position of the cutting tool for the operation.
◦ Home—Create or select a datum point to specify the end position of the cutting tool for the operation.
* 
You can set up separate From and Home points to specify the start and end position for the operation. A From motion will be created between the From point and the first point of the first NC sequence. A Home motion will be created from the last point of the last NC sequence to the Home point.
Alternatively, right-click the graphics window and select, Head 1 Home point, Head 1 From point, Head 2 Home point, and Head 2 From point, Head 3 Home point, Head 3 From point, Head 4 Home point, and Head 4 From point from the shortcut menu.
• Parameters—Provide values for the following optional fields on this tab:
◦ PARTNO—Displays the default part name. You can type another name if required. The part name, is output with the PARTNO command using PPRINT. Right-click, and select Default to set it back to the system default (the name of the manufacturing assembly for Assembly machining, and the name of the workpiece for Part machining).
◦ Startup File—Type the name of the file you want to be included at the very beginning of the operation CL file (after the PARTNO, MACHIN, and UNITS commands). The file must be located in your current working directory and have the extension ".ncl".
◦ Shutdown File— Type the name of the file you want to be included at the very end of the operation CL file. The file must be located in your current working directory and have the extension ".ncl".
◦ CL Output—Select Main Spindle Program Zero to output all steps in the operation using the main spindle program zero or select Per Spindle Program Zero to output all steps in the operation using the sub spindle program zero.
* 
This list is available only if you have a work center with two spindles any you have selected a coordinate system for the sub spindle.
◦ Output File—Displays the default name for the operation cutter location (CL) data file. You can type any name. Right-click, and select Default to set it back to the system default.
* 
The operation CL file is located at the path specified using the pro_mf_cl_dir configuration option.
• Options—Provide values for the following optional fields on this tab:
◦ Stock Material—Select a name of the stock material. Click New to add a new stock material name.
* 
You have to set up the material directory structure first; otherwise, the only option available in the Stock Material drop-down list is Unspecified.
◦ Use Rotary Clearance—This option is available for 4-axis machines only. It allows you to define a safe Z-level retract height for cutting tools, to ensure safety of table rotations. The Clearance value specifies the minimum distance by which the reference model, workpiece, and fixture components will be cleared during table rotations. The default value is 2" (in English units) or 50 mm (in metric units). You can type any positive value. In addition, you can specify a Safe Point for tools that are too long to be retracted to the Rotation Clearance level. Type the X, Y, and Z coordinate values in the Safe Point text boxes. In order for a tool to use the Safe Rotary Point instead of Rotation Clearance, you have to mark it as "long" in the Tool Manager, by selecting the Long Tool checkbox on the Settings tabbed page of the Tool Setup dialog box.
• Fixture Setup—Optionally, define a fixture setup as an element of the operation. A list of all fixture setups defined for the operation are displayed in the drop-down list. Select the required fixture setup from the drop-down list. If you do not require a fixture setup, select the No Setup option in the drop-down list.
This tab also contains the following icons for creating, modifying, and deleting fixture components:
◦ —Optionally, click to insert a fixture component.
Alternatively, right-click the graphics window and select Assemble.
◦ —Click to open the Select Feature dialog box containing a list of fixture setups. Select a fixture from the list and click OK.
• On the Properties tab, optionally specify the operation name or comments. The operation name identifies the operation within the manufacturing process. The default operation names have the format OP010 [MILL01], OP020 [MILLTURN02], where the number gets automatically incremented by the system and the text in brackets denotes the workcenter.
• Select one of the following options depending on your requirement:
◦ Click to save the changes.
◦ Click to pause the process of creating the operation and use one of the asynchronous tools. Click to resume.
◦ Click to cancel the changes.