Sets options for dimensions placed with the Smart Dimension command. Not all options on the command bar are available when using the Smart Dimension command. The options that are available depend upon the element you select and the type of dimension you are placing.
For dimension value editing controls in the modeling environments, see the Help topic, Dimension value edit controls.
Format group options
Dimension Style Mapping
Specifies that the setting on the Dimension Style page of the Options dialog box determines the dimension style. When you set this option, Dimension Style is unavailable.
Dimension Style
Lists and applies the available dimension styles. This option is unavailable when Dimension Style Mapping is enabled.
Text Scale
Applies a scale value to the current text height. The default is 1.0.
Round-Off
Sets the round-off for the value. This option is sensitive to the unit setting (decimal or fractional) and contains values as appropriate for the unit. This option is also sensitive to the dimension being placed and contains values as appropriate for the dimension.
Advanced Round-off
Displays the Round-off dialog box for you to specify all round-off options in one location.
Driving
Changes the state of the selected dimension between driving (locked) and driven (unlocked). If you want to set this option before you place a dimension, you must first select the Maintain Relationships command.
Properties group options
Dimension Axis
Not available when using the Smart Dimension command.
Orientation
The Orientation options are not available when using the Smart Dimension command. However, when placing a dimension between two elements, you can alter the default orientation of the dimension using the following keys.
If a selected line is horizontal or vertical, then the dimension that is created is Horizontal/Vertical to the line.
If a selected line is not horizontal or vertical, then the dimension that is created is placed By 2 Points.
Before you click to place the dimension, you can hold the Shift key to change the orientation of the dimension from By 2 Points to Horizontal/Vertical.
To learn about all of the available keyboard options, refer to the table, below.
Length
Places a linear dimension for the following:
The length of a line.
The arc length of an arc.
The horizontal or vertical distance between the end points of a line.
Note:
Before you place the dimension, and depending upon the number of elements selected, you can use the following keys to affect the dimension that is created:
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Keyboard options |
Result |
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A |
Changes between a linear dimension and an angular dimension. |
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B |
For PMI, changes the dimension orientation back to the previous dimension plane in sequence. |
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D |
Changes between a radial dimension and a diameter dimension. |
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I |
For PMI, selects an intersection point. |
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N |
For PMI, changes the dimension orientation to the next dimension plane in sequence. |
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Shift |
Alternates between:
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Alt |
For a radial or diameter dimension, adds a projection line extension to the dimension.
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Q |
Turns automatic locate off and on so you can select a different element to dimension to. |
Angle
Places an angular dimension for the angle of a line or the sweep angle of an arc.
Radius
Places a radial dimension for the following:
Arc
Circle
Ellipse
Curve
Note:
Before you click to place the dimension, you can use the D key to change from a radial dimension to a diameter dimension, and from a diameter dimension to a radial dimension.
After placing a radial dimension inside an arc or circle, you can drag the edit handle on the extension line to lengthen or shorten it.
Diameter
Places a diameter dimension for an arc or circle.
Diameter Normal
Measures the diameter of elements in the normal plane. This option is available when placing PMI dimensions.
Tangent
Specifies that you want to place the dimension tangent to the selected elements. When you place a tangent dimension, the tangent point on the element closest to the selected point is used.
If you select only one of two elements for a tangent dimension, the dimension is placed from the keypoint of the non-tangent element to the tangent of the element closest to where you click.
If you select both elements for tangent dimensions, the dimension is placed from the tangent point closest to where you click each element. In either case, if necessary, Solid Edge extends the element to preserve this relationship.
If you select two keypoints with the Tangent button depressed, the keypoints take precedence and a tangent dimension is not placed.
Note:
You can use the T key on the keyboard to activate the Tangent option.
Counterclockwise
Changes the dimension from a clockwise to a counterclockwise measurement from the origin. This option is available for angular coordinate dimensions only.
Major/Minor
Displays only the major (A) and minor (B) angles when set.
When this option is cleared, you can choose between four placement options (quadrants) for angular dimensions.
This option is disabled for chained and stacked dimensions.
Jog
Places a jogged projection line on a radial or diameter dimension.
When editing a selected dimension line or dimension projection line with jogs in it, removes all jogs at once.
Note:
You can add jogs to the parallel projection lines on linear dimensions, symmetrical diameter dimensions, and circular diameter dimensions, using Alt+click.
See the Dimensioning overview.
Diameter-Half/Full
For diameter or symmetric diameter dimensions, changes the display between half and full.
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Half |
Full |
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Note: For a Half diameter display, you can use the Extension option in the Projection Line section of the Lines and Coordinate tab (Dimension Style and Dimension Properties dialog box to specify the initial amount that the dimension line extends beyond the center of the circle. |
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Tolerance group options
Dimension Type
Specifies the dimension type. You can choose from the following dimension types.
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Nominal |
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Tolerance (unit) |
Enter a numeric tolerance value in specified units. Example:
Note:
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Tolerance (alpha) |
Enter an alphanumeric string.
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Class |
Note: You can type the tolerance values in the Upper Tolerance and Lower Tolerance boxes. |
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Limit |
Note: You can type the tolerance values in the upper and lower boxes, and use the + and - buttons to specify that the values are positive or negative.
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Basic |
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Reference |
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Feature Callout |
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Blank |
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Inspection
Adds an inspection bubble around the dimension text.
Prefix 
Opens the Dimension Prefix dialog box for specifying prefix, suffix, superfix, and subfix information.
Enable Prefix 
When selected, displays the dimension text specified in the Dimension Prefix dialog box on the next dimension you place or on a dimension you are editing.
When cleared, hides the prefix content.
Upper Tolerance
Sets the primary upper tolerance value. This option is available for tolerance, class, and limit dimension types.
Lower Tolerance
Sets the primary lower tolerance value. This option is available for tolerance, class, and limit dimension types.
Upper Tolerance Sign (+)/Lower Tolerance Sign (-)
By default, the Upper Tolerance box displays the positive upper tolerance value, and the Lower Tolerance box displays the negative lower tolerance value.
You can use the Upper Tolerance Sign (+) button and the Lower Tolerance Sign (-) button to specify whether the tolerance value in the box is a positive value or a negative value. Selecting either button changes it from + to -, and from - to +.
Another way to change the values from positive to negative is to type a - or + in the box and then use the Tab or Enter key to update the dimension value. This does not change the state of the button on the command bar.
You can format the unit tolerance values using the options on the Units tab and the Secondary Units tab in the Dimension Properties dialog box.
Type
Specifies the class type when the Class dimension type is selected. You can choose from the following options.
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Fit |
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Fit, tolerance only |
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Fit with tolerance |
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Fit with limits |
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Fit Hole/Shaft only |
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Fit Hole/Shaft, tolerance only |
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Fit Hole/Shaft with tolerance |
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User-defined (Any user-defined text is valid) |
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For more information, see Class fit dimensions.
Class (Fit)
Sets the tolerance class for user-defined, class fit dimensions. You can type any text in the box.
This option is available only when the Dimension Type is set to Class, and the Class Type is set to User-defined.
Hole
Sets the tolerance class for a hole. This option is not available for the Class Type: User-defined.
Shaft
Sets the tolerance class for a shaft. This option is not available for the Class Type: User-defined.
Note:
You can change the formatting of class fit type dimensions and tolerance type dimensions using the options in the Tolerance Text section of the Text tab (Dimension Style and Dimension Properties) dialog box. For example, you can specify a slash or a horizontal separator; how to align the numbers (to the + or - sign or the decimal point); and whether to use a degree symbol.
Other group options
Set dimension plane
Sets the active dimension plane for the creation of PMI dimensions and annotations. The dimension plane controls how dimension values are calculated and how the dimension text is displayed.
Lock dimension plane (F3 to unlock)
Lets you specify a dimension plane by clicking a planar face or reference plane. The plane remains locked until you unlock it by pressing F3.
Keypoints
When placing a PMI model dimension, you can select the type of keypoint to dimension to. The default 3D keypoint filter option, 
, selects only the centers of circles and arcs or endpoints of edges. Use this option to place a dimension that you want to use to change the model.
Activate part
Makes a part in an assembly available for selection and for dimensioning and annotating. This option is only available in assembly models.
Place a locked dimension on a drawing
