Parametric dimensions resize geometry when you change the dimension value. You can sketch freely without worrying whether or not the geometry is the correct size.
When you edit a sketch dimension, its position adjusts as the sketch geometry updates. When you rotate the view of your sketch, dimensions reorient so you can read them easily.
Parametric dimensions can be set to display parameter values, parameter names, or expressions.
As you sketch, the size of the geometry is automatically calculated. If it is acceptable, you can accept its size. Usually, you add dimensions to specify the correct size. You can sketch rough geometry and create a feature from it, then return later to edit the sketch and add dimensions to precisely size the feature.
Units are determined when you choose a template or set one up with custom units.
A powerful capability of parametric dimensions is your ability to control them. You can specify dimensions with parameters in a spreadsheet, control dimensions through equations to maintain proportions between geometric elements, or as constant values.
Dimensions constrain sketch size. Consider leaving geometry undimensioned if it changes size or is included in an iFeature that resizes when used in different parts.
If a dimension overconstrains the sketch, you can accept or cancel the dimension. If you accept the dimension, the dimension is saved as a reference parameter. Its value is enclosed in parentheses in the sketch, and updates in response to changes in driving dimensions.
Only normal dimensions can be edited. In an overconstrained sketch, you may have to convert other dimensions to driven (reference) parameters first or remove some dimensions or constraints before you can convert driven dimension to normal dimensions.
To take advantage of adaptive features, you can dimension elements to be a specific size or proportional to other geometry, while leaving other elements undimensioned. If your customer places a part with adaptive features into an assembly, the undimensioned geometry in the feature can change size and shape when constrained to fixed components.
In 3D sketches, you can add only linear and angular dimensions. Radial dimensions are created only when you create bends.
You can change the display style of dimensions. When a dimension is not selected, right-click in the graphics window, and select Dimension Display. Choose Value, Name, Expression, Tolerance, or Precise Value.
You can find sketch in browser using a sketch dimension. Select a 2D or 3D sketch dimension in the graphics window, right-click, and select Find in Browser. The related sketch is highlighted in the browser. Find in Browser is not available when multiple sketch dimensions are selected.
You can edit sketchbefore or after a sketch becomes part of a feature. If a sketch has not been by a feature, its dimensions are visible and can be edited. After a sketch is consumed by a feature, select the feature in the browser and activate the sketch for editing.
To change the dimension display style, right-click in the graphics window and select Dimension Display. Choose Value, Name, Expression, Tolerance, or Precise Value.
You can remove dimensional constraints from a sketch, and allow the sketch to resize as needed.
Use in addition to the Dimension and constraint commands on the Sketch tab, Constrain panel, to place critical dimensions. You can individually-select, multi-select, and window-select geometry to add or remove dimensions or constraints.
Use the Dimension command to add only the dimensions you need, then use the Automatic Dimensions and Constraints command to calculate all other sketch dimensions and constraints. Autodesk Inventor LT remembers which dimensions and constraints you added and which are calculated by the system, so that the specific values you need are not replaced.
Use Show Dimensions to display feature and sketch dimensions. When dimensions are displayed, you can edit the values.
Adds automatic dimensions and constraints to fully constrain a sketch. Use in addition to the Dimension and constraint commands on the Sketch tab, Constrain panel (to place critical dimensions). Autodesk Inventor LT remembers which dimensions you place with the Dimension and constraint commands and those placed by the Automatic Dimensions and Constraints command so that your added dimensions and constraints are not replaced.
Automatically applies missing dimensions and constraints to selected sketch geometry.
Selects geometry to dimension.
Default is On. Applies automatic dimensions to selected geometry. Clear check mark to exclude dimensions.
Default is On. Applies automatic constraints to selected geometry. Clear check mark to exclude constraints.
Shows number of constraints and dimensions required to fully constrain the sketch. If either Dimensions or Constraints are excluded from the solution, the number is removed from the total shown.
Applies dimensions and constraints to selected geometry.
Removes dimensions and constraints, if the associated check box is selected, from the sketch geometry.
Closes dialog box.
The Dimension command adds dimensions to a sketch. Dimensions control the size of a part. They can be expressed as numeric constants, as variables in an equation, or in parameter files.
Dimensions calculated by equations (where, for example, d5=d2) are displayed with a prefix of "fx."
Dimensions that overconstrain a sketch (driven) are enclosed in parentheses. They do not resize geometry, but update in response to changes to normal dimensions
Using the Dimension command, you can place the following types of dimensions:
Linear dimension from one element.
Linear dimension between two elements.
Aligned dimension between two elements.
Angular dimension between two edges.
Angular dimension between three points.
Angular dimension of an interior angle.
Angular dimension of an exterior angle.
Angular dimension from a reference line.
Changes settings that originate on the Units tab and Default Tolerances tab of the Document Settings dialog box. Settings affect all dimensions in the current document.
In the browser, right-click a feature and select Edit Sketch or Show Dimensions. Right-click a dimension, select Dimension Properties, and click the Document Settings tab.
Or, right-click in a sketch and select Dimension Display.
Changes the display type for model dimensions. Click the down arrow to choose an item, then click Apply to see its effect on dimensions.
Shows the nominal dimension.
Shows the dimension as a parameter name.
Shows the dimension as an expression.
Shows the tolerance for the dimensions.
Show Precise Value
Shows the dimension value, ignoring any precision setting.
Controls the number of decimal places to the right of the decimal in linear dimensions.
Controls the number of decimal places to the right of the decimal in angular dimensions.
Select check box to use the precision and tolerance values set on this tab when creating dimensions.
Applies a linear tolerance setting to a dimension of a specific precision.
Applies an angular tolerance setting to a dimension of a specific precision.
Select check box to export dimensions to drawings using the precision and tolerance values set on the Default Tolerance tab.