ZW3D Base | ||
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Input Options Index | ||
You can right-click the mouse during any command that is prompting you for input. Doing so may display a menu of the Input Options for that command prompt. The options that appear are command sensitive and will vary depending on the situation. The table below lists many of the more common input options. Many of the point and directional input options function within the context of an assembly. Components and sub-assemblies as well as the active part can be referenced directly without additional external reference commands.
2 Lines
2 Planes
3 Points Angular Specify the included angle between four points as input. The first and second points define the first direction while the third and fourth points define the second direction. The two directions define the included angle.
-X axis
Directional Select the world -X axis as directional input. -Y axis Directional Select the world -Y axis as directional input. -Z axis Directional Select the world -Z axis as directional input. 1 Line Angular Specify the angle between a vector and the X axis as angular input.
2D Sheet
Command
Create a new 2D Sheet and add it to the active file. The object name will be "file_name_2D" where "file_name" is the name of the active file. After selecting the command, a list of drawing templates are available to choose from.
0 degrees Angular Specify 0 degrees as the angular input. 30 degrees Angular Specify 30 degrees as the angular input. 45 degrees Angular Specify 45 degrees as the angular input. 60 degrees Angular Specify 60 degrees as the angular input. 90 degrees Angular Specify 90 degrees as the angular input. 180 degrees Angular Specify 180 degrees as the angular input. 270 degrees Angular Specify 270 degrees as the angular input. 360 degrees Angular Specify 360 degrees as the angular input. A Absolute Point Specify absolute X,Y,Z coordinates as point. The coordinates are measured from the world coordinate frame of the active part. All Dimensions Show all dimensions in the active part. This option is available when you are prompted to select a dimension. Along Point Select a point along a specified line, arc, circle, curve, or edge. The location can be a percentage or a distance along the curve. Angle Point Select a point on an arc or circle that is at a CCW angle from a selected point on the arc or circle. Angular Dim. Selection During the Quick Dimension command, use this input option to change to Angular Dim. mode from Default Dim. mode.
Attributes
Entity
For any entity that contains editable attributes such as points, lines, text, tables, etc., this option displays the appropriate attributes form to easily modify its attributes. The changes will only apply to that entities attributes.
B Between Point Specify a point defined by the Percent or Distance between two other points. The point is located in a linear direction from the first point to the second. An Options Form is provided. Between Crv Points Point Specify a point defined by the mid point between to points on a curve. Select two points on a curve. Boundary Face Location Use this input option to limit the effect of an operation. An example of using Boundary Face during the Extrude Shape command would be extruding to a pipe shape. That is, a hollow cylinder. Starting outside the cylinder and extruding to the outside of the cylinder (the boundary face) would not gouge the inside of the cylinder. The boundary face option (a "bounded boolean") ensures that it does not. Without this option, it would be generally impossible to extrude to the pipe without penetrating to the interior unless the pipe wall were very thick and the profile small. Browse Operational Make the Object Browser or the History Manager appear for selection. Browse Variables Operational Display the Variable Browser when prompted to enter a variable name. C Center Point Select a point at the arc center of an arc, circle, or curve. If a curve is selected, the arc center is calculated from the selected point on the curve.
CAM Plan
Command
Create a new CAM Plan and add it to the active file. The object name will be "file_name_CAM" where "file_name" is the name of the active file. After selecting the command, a list of CAM templates are available to choose from.
Center line Directional Specify the center line of a cylindrical face as directional input.
Center of Curvature
Point
Select the center of an arc when Critical Point picking fails to recognize the arc as an arc.
Component Dimensions Show all dimensions specific to a component. Critical Point Have the cursor highlight critical points (e.g., endpoints, midpoints, datum plane origins, etc.) of lines, edges, curves, and datum planes during point input. Curve Normal Directional Specify the normal direction of a curve at a point on the curve as directional input. Curve Tangent Directional Constrain directional input tangent to a curve at a point and direction. Cv-Cv Intersection Point At the Part Level, select the intersection of 2 curves to specify a point. Cv-Sf Intersection Point Select the intersection of a curve and face to specify a point. D Datum Dimensions Show datum plane dimensions. Default Point Switch back to the Default point selection mode from other modes such as Relative, Critical, or Tangent. Default mode is the absolute point you pick or the coordinates you enter. Also use Default mode to snap to grid points that are in close proximity with other Critical points. Default Dim. Selection During the Quick Dimension command, use this input option to change back to Default Dim. mode from the Angular Dim. mode. Dimension Value Location Enter a relative location based on a dimension value. E Editor Operational Display the Text & Dimension Editor for entering text. Entity Selection Select an entity as input. Expression Value Enter an expression using the Expression Input Form when prompted for a value. See also Equations and Expressions. F Face Normal Directional Specify the normal direction of a face at a selected point on the face as directional input. Face Normal Direction Offset Directional Used during the Modify Face Control Points command. Offsets the control points a specified distance determined from the projection location of the control point onto the face. If more than one control point is selected, the barycenter of the control points is used.
Face-Vector Point Select a point defined by the projection of a vector onto a face. Feature Dimensions Show all dimensions that define a feature. File Browser Selection Display the File Browser. Focus Selection While editing a sketch, use this input option to have the constraint manager change the Focus of Smart Pick from one entity to another. From 2 Lines Point Select a point that is a specified distance from 2 lines. G Grid Point Constrain the cursor to select points on the active sketch grid. I Insert Curve List Selection Create a curve list from a selection of curves connected end to end. This allows multiple curves to be combined into a single selection for use during drive curve loft, bi-rail loft, threads, sweeps, surface mesh tools and base, boss, and cut feature tools. The curves are not physically combined (concatenated) or otherwise modified. You can also make a curve list using the Define Curve List command. Insert Datum Selection Executes the Insert Datum Plane command and then automatically assigns the new datum as input to the command.
Insert Reference Plane
Selection
Executes the
Reference a Datum Plane/Face (3D) command and then automatically assigns the new datum as input to the command.
Insert Sketch
Selection
Executes the
Insert Sketch command and then automatically assigns the new datum as input to the command.
Intersection
Point Select the intersection of two curves to specify a point. This option will select "implicit" intersections. If you move the cursor over the intersection of the two curves, the point will highlight automatically. L Length Value Enter a length. M
Measure
Angle
Angular
Measure Arc
Measure DistanceAngular Specify an angle subtended by an arc as input.
Distance
Executes the
Inquire Distance (3D) command and then automatically assigns the new datum as input to the command.
Measure Face Dihedral
Angular Specify an angle defined by a face dihedral. Face dihedral refers to the angle between two adjacent faces/planes at a point along a shared edge. For input, select the shared edge at the point where you want to measure the face dihedral for. O Object List Operational Make the Object Browser appear for selection. Offset Point Select a point that is offset relative to a point in the X, Y, (sketch/Drawing Sheet Level) and Z (part level) directions. First select a reference point. Then enter the offset values. At the part level, you can also select an alternate datum plane that the offsets will be relative to or you can middle-click for the default world origin.
Offset Distance
However, if the filter is set to ALL, edges have priority over the faces that they border and vertices have priority over all of the edges that meet at that vertex. If your command allows a point to be picked on a face, you need to set the Pick Filter to Face.
In wireframe mode, faces are pickable even if the cursor is not over an edge or isoline. In shaded mode, hidden faces cannot be picked.
P Pick All Selection Select all entities in the active object of the specified type. If you want to pick all of a certain type of entities, use the Pick All option in conjunction with a pick filter instead of using Window Pick. In general a Pick All will regenerate much more quickly than the entity list created by a Window Pick.
Pick Curves
Proj to Cv or Sf Point Use this input option to project a point onto a curve or face to specify a point. The point is projected normal to the curve or face. Projected Cv-Cv Intersection Point Specify a point at the intersection of two curves projected onto a plane.
Q
Quick Chain Pick Selection This Input Option performs the same task as Chain Pick, but does not require the SHIFT KEY. It selects all lines, arcs, curves, or edges that are connected end to end. It is now available as an RMB (Right Mouse Button) selection when curves are accepted as input. Selecting the option toggles it on & off. Chain Pick, on the other hand, is activated by holding down the SHIFT KEY while picking. See Other Keys & Mouse Combos for more about Chain Pick. IMPORTANT NOTE: Selections made using Quick Chain Pick ARE NOT re-evaluated during part history regenerations. For this added functionality, use the Pick Curves input option. Quadrant of Curvature Point Select a quadrant point of the arc, circle or arc/circle edge as the input. The center point is the coordinate origin. R Relative Point Select a point by entering an X,Y,Z coordinate value that is relative to the last point selected. S Show All Dimen Selection Shows all dimensions in the active part. Show Datum Dimen Selection Shows all dimensions that locate datum planes. Show Feature Dimen Selection Shows all dimensions that drive features Show Label Selection Use this input option to show the temporary label of an entity as they are highlighted by the cursor. These labels are only good until the next regeneration of the active part. They can be used to pick an entity (by text input), but can potentially change when the part is regenerated. If the part topology does not change, then the labels will likely remain the same. These labels are generated for curves (#), faces (f#), edges (e#) and shells (s#). The number embedded in the label is a simple counter assigned to each entity in the order it is generated. If the order of creation changes during a regeneration, the labels will change. Show Sketch Selection Show the sketch related to a selected feature if one exists. This function is logged to the active parts history. Sketch Selection Use this option during selection of a list of points in part edit mode. It will prompt you to select a sketch. The coordinates of all point entities of the sketch will be input to the active point input list. This is useful for controlling the number and placement of holes in a part using a sketch. Snap Pick Off Selection Turn off Smart Pick. More details see Enable "Snap Pick" on Configuration dialog. Snap Pick On Selection Turn on Smart Pick. More details see Enable "Snap Pick" on Configuration dialog. T Tangent Point Select a point that is tangent to a line, arc, circle, or curve. Through All Location Constrain the depth of a feature to pass completely through the part. To Curve Location Enter a relative location based on a curve or edge. For example, during the Trim/Extend Wireframe Curve command, you can select a curve or edge to extend to. To Face Location Enter a relative location based on a face. For example, during the Trim/Extend Wireframe Curve command, you can select a face to extend to. To Point Location Enter a relative location based on a point. U Unpick All Selection Unselect all previously selected entities. Unpick Last Selection Unselect the last entity selected or to delete the current entry in the Text Input Window.
ZW3D Manager
Command
Displays/Hides the ZW3D Data Manager.
W Window Pick Selection Select entities contained within a window defined by two diagonal points. Entities passing outside the defined window will not be selected. If you want to pick all of a certain type of entities, use the Pick All option in conjunction with a pick filter instead of using Window Pick. In general a Pick All will regenerate much more quickly than the entity list created by a Window Pick. X X axis Directional Select the world X axis (positive) of the active part. Y Y axis Directional Select the world Y axis (positive) of the active part. Z Z axis Directional Select the world Z axis (positive) of the active part. |
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