Autodesk WikiHelp Product help with community knowledge

Product
Language
Release

Community Scoring

Was this page helpful?

Tag Tags0

This page has no tags

Page statistics

2514 views, 1 edit(s), 14205 characters(s) Page last modified 21:46, 9 Feb 2012 by adsk_arutherford

How to add your knowledge

Create new page
Edit page
Upload video
- Upload video
- Video overview

Body Constraints

1. Create body constraints
2. Constraints in the browser
3. Special behavior and limitations

Inventor Fusion uses direct modeling, which allows you to change model geometry without impacting other features. This behavior makes it easy to create and modify models, but you can also make unintended changes to the model. Define the geometry relationships as the model matures so that you can lock down the shape of the model.

Overview of body constraints

Use body constraints to make planar faces coplanar, parallel, or perpendicular, and to make cylinders concentric. Body constraints create relationships between the faces, but do not control the size or location in the model.

NoteDefining the relationships between geometry is also called capturing design intent. For example, a motor has mounting feet that are bolted onto a flat surface. Adding coplanar constraints to the mounting feet captures the design intent for mounting the motor.

Body constraints are added to a Constraints folder in the browser. The faces are highlighted when you click on a constraint. You can delete a constraint, but you cannot edit it to change the type or the face selections.

Body constraints are used with model dimensions to define the model and capture relationships. Use body constraints to create relationships between geometry, such as making two cylinders concentric. Use dimensions to locate and define the size of geometry and features, such as the diameter and location of a hole. See the Working With Model Dimensions and Body Constraints section for more information.

Body constraints create relationships between geometry in a single component. Use assembly constraints to position components and create constraints between them. See the Position and Constrain Components topic for more information.

Create body constraints

Use body constraints to constrain faces and edges within a single component. Body constraints cause the body to maintain it’s shape as changes are made. For example, if you make two faces parallel, both faces update if one of them is moved to a different angle.

Body constraints define relationships between model geometry in a single component. You cannot create body constraints between components. Use Assemble to create geometric constraints between components.

Body constraints do not display in the graphics window, but they are added to a Constraints folder in the browser. Click on a constraint to highlight it in the graphics window.

The following types of Body constraints can be created:

Coplanar: Two planar faces are in the same plane
Center: Two cylindrical faces are aligned along the same axis.
Parallel: Two planar faces are parallel
Perpendicular: Two planar faces are perpendicular

Start Body Constraint from the Constrain & Dimension panel.
Select the Constraint Type. The face selections are filtered based on the constraint type.
1. Only planar faces can be selected for Coplanar, Parallel, and Perpendicular constraints.
2. Only cylindrical faces can be selected for Center constraints.
If desired, change the constraint type before you apply the constraint. The faces are deselected if they are not valid for the new constraint type.
The first face that you select is marked with the Anchor glyph, and the second face is marked with the Non-anchor glyph. When you apply a constraint, the anchored face remains where it is and the other face moves.
You can switch the anchored and non-anchored faces by pressing the Tab key, or clicking one of the anchor glyphs.

NoteThe anchored state is temporary. After you create the constraint, either face can move to satisfy the constraints.


The filleted end was selected first, so the hole moves to become concentric.

The hole was selected first, so the model is shortened to make the filleted end concentric.

Constraints in the browser

Body constraints are added to a Constraints folder in the browser. The faces highlight when you pause the cursor over a constraint. You can rename constraints to make it easier to identify them. You cannot edit a constraint; you can only delete it from the browser and create a new one.

Special behavior and limitations

If a modeling change divides a face, only one of the new faces keeps the constraints. It is not possible to predict or specify which face will keep the constraint.
Only the DWG format supports body constraints.
The Draft command overrides body constraints. Any conflicting constraints are deleted.
Using a face to create some features, like Revolve, will delete the original face. Any constraints to that face are also deleted.

Work with body constraints and model dimensions

Use a combination of body constraints and model dimensions to control the size and shape of a model. Body constraints define geometric relationships between faces and edges within a single component. Model Dimensions define the size and location of model edges, both within a component and between components.

Body constraints:

Make model geometry coplanar, concentric, parallel, or perpendicular.
Do not define the size or location of faces or edges.
Cannot be created between components.

Model Dimensions:

Define the size of or distance between edges.
Do not control geometric relationships between faces.
Can be created between components.

When the model is changed, Inventor Fusion analyzes the body constraints and model dimensions to maintain the shape of the model and the size of features. The body constraints are solved first, and then the model dimensions. An error displays if there is a conflict.

For more information on using dimensions to define the size and location of model edges, see the Model Dimensions and Annotations topic.

For information using assembly constraints to position components relative to each other, see the Position and Constrain Components.

Inventor Fusion