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Parametric dimensions

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.

Can dimensions be changed after a feature is created?

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.

How are units determined?

Units are determined when you choose a template or set one up with custom units.

How can parametric dimensions be specified?

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.

How do dimensions work with adaptive features?

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 you place a part with adaptive features in an assembly, the undimensioned geometry in the feature can change size and shape when you constrain it to fixed components.

After you place a component in an assembly, you can edit its dimensions or change its parameters. This capability lets you maintain a family of similar parts that must be different sizes in multiple assemblies.

Procedures

 On the ribbon, click Sketch tab Constrain panel Dimension to add dimensions to a 2D or 3D sketch. Dimensions control the size of a part and can be expressed as numeric constants, as variables in an equation, or in parameter files. In 3D sketches, you can add only linear and angular dimensions. Radial dimensions are created only when you create bends.

In 2D sketches, diametric dimensions are created by default if a centerline is included in the dimension.

Dimensions control the size of a part. You can express them as numeric constants, variables in an equation, or in parameter files.

 On the ribbon, click Sketch tabConstrain panel Dimension. In the graphics window, click the geometry and drag to display the dimension. To add: A linear dimension for a curve, click to select the curve. A linear dimension between two points, two curves, or a curve and a point, click to select each point or curve. In a 3D sketch, you can also constrain the distance between a point and plane or planar face. A radial or diametric dimension, click to select the arc or circle. Right-click and select Radius for an arc or circle, or Linear for a centerline. An angular dimension: In a 2D sketch, select two curves or three points. In a 3D sketch, select two points, one of which can be a work axis. Click to place the dimension. In a 3D sketch, the dimension text is parallel to a plane created by the two selections. Click the dimension text and drag to reposition if needed. In a 3D sketch, you can drag the dimension text on the placement plane only. If the dimension overconstrains the sketch, you can accept it or cancel the dimension. If you accept the dimension, it is saved as a reference parameter. Double-click the dimension value to open the Edit Dimension box. Specify a value, use an equation to calculate the value, or click the arrow to measure the value, show dimensions, or set a tolerance. TipYou can also enter or edit an expression that defines a parameter. For example, enter HGHT = 5mm. The expression is parsed to create the parameter HGHT and assign it a value of 5 mm.

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.

Dimensions calculated by equations (where, for example, d5=d2) are displayed with a prefix of "fx."

NoteClick Options to access the Application Options dialog box, and then click the Sketch tab to set preferences for placing overconstrained dimensions and editing a dimension when it is placed.

Show Me how to add and edit dimensions

Show Me how to use driven dimensions

Edit sketch dimensions

 You can edit sketch dimensions before or after a sketch becomes part of a feature. If a sketch has not been consumed 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.
NoteDimensions 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 and updates in response to changes in normal dimensions.

Edit dimensions on unconsumed sketch geometry

1. Open the Edit Dimension box one of these ways:
• If the Dimension command is active, click the dimension to change.
• If the Select command is active, double-click the dimension to change.
2. Enter a new value or click the arrow and select Measure, Show Dimensions, or one of the listed values.
TipYou can also enter or edit an expression that defines a parameter. For example, enter HGHT = 5mm. The expression is parsed to create the parameter HGHT and assign it a value of 5 mm.

To make the current dimension equal to another dimension, enter a dimension number. Dimensions calculated by equations (where, for example, d5=d2) are displayed with a prefix of "fx."

3. Click the check mark to accept the new dimension.

Show Me how to edit a dimension

NoteTo automatically edit the dimension value when you place a dimension, click Options to access the Application Options dialog box and click the Sketch tab. Select the Edit Dimensions When Created check box.

Edit feature sketch dimensions

1. In the browser, right-click a sketched feature, and select Edit Sketch. The feature sketch is displayed.
2. Double-click the dimension to change.
3. Enter a new value or click the arrow and select Measure, Show Dimensions, Tolerance, or one of the listed values.
TipYou can also enter or edit an expression that defines a parameter. For example, enter HGHT = 5mm. The expression is parsed to create the parameter HGHT and assign it a value of 5 mm.
4. Click the check mark to accept the new dimension.
5. Right-click and select Finish Sketch to update the feature with the new dimension.
TipOnly normal dimensions can be edited. To convert driven dimension to normal dimensions, select the dimension(s), and then click Sketch tabFormat panel Driven Dimension to switch off the Driven dimension option. In an overconstrained sketch, you may have to first convert other dimensions to driven (reference) parameters, or remove some dimensions or constraints, before you can convert driven dimension to normal dimensions.

Delete sketch dimensions

You can remove dimensional constraints from a sketch, and allow the sketch to resize as needed. Parts with adaptive features resize in assemblies when they are constrained to fixed geometry.

 On the Quick Access toolbar, click Select Sketch Features.Right-click the dimension in the graphics window.Select Delete from the menu.
NoteIf the sketch is part of a feature, click Update after you delete dimensions.

Automatically apply sketch dimensions and constraints

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 remembers which dimensions and constraints you added and which are calculated by the system, so that the specific values you need are not replaced.

To begin, use commands on the Sketch tab to create sketch geometry. If desired, use the Dimension command to apply critical dimensions.

 On the ribbon, click Sketch tabConstrain panel Automatic Dimensions and Constraints.The Auto Dimension dialog box shows the number of dimensions and constraints required to fully constrain the sketch.Accept the default settings to add both Dimensions and Constraints or clear a check mark to prevent application of the associated items.Click Curves, then individually or multi-select geometry.If you prefer, click and hold the left mouse button, then drag to enclose desired geometry in a selection window, then click to select.Click Apply to add dimensions and constraints to selected geometry.To automatically dimension and constrain the entire sketch, click Apply with no geometry selected.If desired, click Remove to delete the automatically added dimensions and constraints from the sketch geometry. The Dimensions and Constraints check boxes must be selected for the Remove command to delete the dimensions and constraints, respectively.When finished, click Done.

Show Me how to use Automatic Dimensions and Constraints

Show dimensions

Use Show Dimensions to display feature and sketch dimensions. When dimensions are displayed, you can edit the values.

1. Right-click a feature in the browser or graphics window and select Show Dimensions.
2. If desired, do one or more of the following:
• Double-click a dimension and edit its value.
• Double-click a dimension and change its value to a parameter.
• Delete a dimension.
3. To hide dimensions, click in the graphics window or select another command.
4. On the Quick Access toolbar, click Update to incorporate changed values, if necessary.
NoteUndimensioned ( underconstrained ) geometry can be designated as adaptive . Its size changes when it is constrained to fixed geometry in an assembly. Right-click a feature with undimensioned geometry and select Make Adaptive.

Change the display style of dimension values

You can show parametric dimensions as nominal values, parameter names, expressions, with tolerances, and precise value. Setting the dimension display style applies to all dimensions in the document.

1. In an active sketch, right-click in the graphics window.
2. Click Dimension Display.
3. Select a dimension display style.

Value displays the nominal dimension.

Name displays dimension as a parameter name.

Expression displays the dimension as an expression.

Tolerance displays the tolerance for dimensions.

Precise Value displays the dimension value, ignoring any precision setting.

NoteDimensions that are based on equations are preceded by the letters "fx." For example, if d0 is the value for another dimension (so that its size is equal to d0), the dimension displays as fx:d5 = d0 for a dimension expression or fx:90 for a nominal dimension.

References

Automatic Dimensions and Constraints

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 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.

 Access: Ribbon: Sketch tab Constrain panel Automatic Dimensions and Constraints
 Automatically applies missing dimensions and constraints to selected sketch geometry. Curves Selects geometry to dimension. Dimensions Default is On. Applies automatic dimensions to selected geometry. Clear check mark to exclude dimensions. Constraints Default is On. Applies automatic constraints to selected geometry. Clear check mark to exclude constraints. Dimensions Required 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. Apply Applies dimensions and constraints to selected geometry. Remove Removes dimensions and constraints, if the associated check box is selected, from the sketch geometry. Done Closes dialog box.

Sketch dimensions

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

 Access: Ribbon: Sketch tab Constrain panel Dimension
 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. Radial dimension. Diameter dimension.

Dimension properties - Document settings tab

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.

 Access: 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.

Modeling 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.

 Value Shows the nominal dimension. Show Name Shows the dimension as a parameter name. Show Expression Shows the dimension as an expression. Show Tolerance Shows the tolerance for the dimensions. Show Precise Value Shows the dimension value, ignoring any precision setting.

Linear Dimension Display Precision

Controls the number of decimal places to the right of the decimal in linear dimensions.

Angular Dimension Display Precision

Controls the number of decimal places to the right of the decimal in angular dimensions.

Use Standard Tolerancing Values

Select check box to use the precision and tolerance values set on this tab when creating dimensions.

 Linear Applies a linear tolerance setting to a dimension of a specific precision. Angular Applies an angular tolerance setting to a dimension of a specific precision.

Export Standard Tolerance Values

Select check box to export dimensions to drawings using the precision and tolerance values set on the Default Tolerance tab.