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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.
-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.
2 Lines
Angular
Specify the included angle between two lines, linear edges, or directional vectors as input.
2 Planes
Angular
Specify the included angle between two datum planes or planar faces. The datum plane or face normal direction will be used to calculate the included angle.
3 Points
Angular
Specify the included angle between three points as input. The first point defines the vertex of the angle. The remaining two points define the leg endpoints of the included angle.
30 degrees
Angular
Specify 30 degrees as the angular input.
4 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.
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.
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.
Arc
Angular
Specify an angle subtended by an arc as input.
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.
Centerline
Directional
Specify the centerline of a cylindrical face as directional input.
Centerline
Directional
Specify the centerline 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 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.
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
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 Distance
Distance
Executes the
Inquire Distance (3D) command and then automatically assigns the new datum as input to the command.
Middle
Point
Specify a point at the middle (midpoint) of a line, arc, curve, or edge.
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.
On Entity
Point
Use this input option to pick a point on an entity. The Pick Filter can be used to limit the pick to be on a particular type of entity. The front-most entity is always selected.
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.
Plane Axis
Directional
Select the X, Y, or Z axis of a datum plane, face, or sketch as input when prompted for a direction.
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.
 Required Inputs
- Place method
This specifies the method of projecting the two curves to determine the intersection point.
1st curve - Projects the intersection of the two curves onto the first curve.
2nd curve - Projects the intersection onto the second curve.
Half way - Projects the intersection right between the two curves.
Offset - Offsets the intersection from a projection plane. Specify the plane and offset below.
- 1st curve, 2nd curve
Select the two curves to determine a projected intersection for.
- Plane
Select a datum plane or planar face to project the curves onto.
- Offset
Select a distance to offset the plane that the two curves are projected onto. See Plane above.
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.
Smart Pick Off
Selection
Turn off Smart Pick. When Smart Pick is on, cursor movement will automatically detect and highlight fixed and relational pick points.
Smart Pick On
Selection
Turn on Smart Pick. When Smart Pick is on, cursor movement will automatically detect and highlight fixed and relational pick points.
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.
VX Manager
Command
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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