Product help with community knowledge

Page statistics

0 views0 edit(s)0 characters(s) Page last modified 13:09, 19 Oct 2012 by henderh

Prepare for Analysis

Version as of 17:02, 18 Jun 2013

to this version.

View current version

When considering a part or assembly for analysis, there are considerations worth making. Among them is model preparation. To prepare an assembly model for analysis, evaluate the types of components. In a part model, evaluate the part features. Then you can remove low impact parts or features from the analysis, and improve performance with relatively little difference in the analysis result.

The actions that prepare a part or assembly for analysis are:

Simplify the model

Why simplify an assembly?

When you analyze assemblies, you can exclude small parts whose functionality is simulated by constraints or forces. Simplifying an assembly, where possible, helps reduce simulation times.

Why simplify part features?

When you conduct simulation analyses, you can tailor portions of a model to allow for a more efficient analysis. This tailoring involves suppressing geometrically small features that are not subject to stress concentrations. An example is outer convex rounds. They can complicate mesh creation, without significant effects to the final result.

Why simplify your model containing thin bodies?

Your model can often contain components that are comprised of very thin wall bodies relative to the overall dimensions or size of the model, so can be very thin (for example sheet metal or frame structures). Therefore an analysis of such components using solid elements based FEA leads to long meshing/solution times and numerical instabilities in the results. When you simplify components containing thin wall bodies to shells you may dramatically reduce computational resources required for your simulation.

You may inspect your model to see if there are thin bodies which are good candidates for shell feature by clicking the Find Thin Bodies command on the Prepare panel.

Bodies that meet the thin component criteria are found within your model automatically. Then you can decide to simplify the solid geometry and generate mid-surfaces defining shell structure using Midsurface command or Offset command.

What are the limits for using the thin parts commands in Stress Analysis?

L/D ratio = Length /Thickness

where:

Length = overall length of the body

Thickness = thickness of the body

Consider a thin square plate whose length and width are 100 with a thickness of 1. The L/D ratio of such a plate is 100/1 = 100. We compute the L/D ratio of the input body and compare it with the thin square plate’s L/D ratio.

• If the L/D ratio is below 100, the body is considered as thick (or solid), and we recommend to analyze it as solid to perform accurate analysis using solid elements.
• If the L/D ratio of the input body is above 100, then the body is considered as a thin component, and is highlighted as such after you click the Find Thin Bodies command.
• If the L/D ratio is above 100 and you perform the analysis without converting them to a Shell using either Midsurface or, Offsett, a message displays recommending using the Find Thin Bodies command to perform more accurate analysis.
• If the L/D ratio is above 250, and the body is being analyzed as a thick solid, a warning message displays indicating that results of analysis are very likely to be inaccurate and not precise.
NoteSpecific details on how the L/D ratio is computed and compared are not covered here. Autodesk Inventor makes only a suggestion of which body should be considered as a thin. The chosen criteria are not absolute, so they may not be applicable in to some specific circumstances. You can override results of the command.

Structural constraints restrict or limit the displacement of the model. For static simulations, remove all rigid body modes (free translational and rotational movement of the bodies). To do so, fix a face, for example, or combine partial constraints on faces, edges, or vertices.

NoteOver or under constraining can substantially change the model behavior. Therefore, considerable attention must be given to assigning a proper set of constraints to reflect the real model environment.

Types of structural constraints are:

 Fixed Removes all degrees of freedom. Frictionless Prevents movement normal to the surface. Pin Isolates degrees of freedom to radial, axial, or tangential.

To display the reaction force information, run the simulation and then right-click a constraint in the Simulation browser, select Reaction Forces.

NoteYou can apply loads and boundary conditions to the same entity as long as they are compatible. You can apply incompatible load and boundary conditions by mistake to the same entity. An example is a fix face in Z direction, and a load applied in Z direction to the same face. Then the fixed boundary conditions override the forces.

Structural loads are forces applied to a part or assembly during operation. Such loads cause stresses, deformations, and displacements in components.

In product design, it is important to know how your product reacts under normal and excessive working conditions. Know how to determine the response your product has to these loads, and build in an appropriate safety factor. Important aspects of your design include load magnitude, frequency of occurrence, distribution, and nature (static or dynamic). If you can visualize how your product responds to loads, you can control your designs better.

The types of structural loads available are:

• Force (N or lbforce)
• Pressure (MPa or psi)
• Bearing Load (N or lbforce)
• Moment (N*m or lbforce in)
• Remote Force (N or lb)

Apply structural loads Normal to the face where the force is perpendicular to the face. Apply structural loads Directional to the face with a magnitude specified in each direction. You can apply moments to solid faces. Use remote force to:

• Apply a force at a specific point outside or inside of the model.
• Be transformed as an equivalent force and moment on a given face.

You can apply Bearing load to cylindrical faces only.

NoteIf you apply loads to faces that are involved in contacts, use Pressure rather than Force.

A body load is a load acting on the entire volume or mass of a component. Examples of body loads include, but are not limited to:

• Gravitational force

Body loads created through the application of:

• Linear acceleration
• Angular velocity and acceleration

If the model experiences the effect of outside forces, define gravitational or body loads. You can define up to one gravitational and one body load per simulation.

Specify Materials

Material properties define the structural characteristics of each part of a model for a simulation. Each simulation can have a different set of materials for any component.

Styles and Standards

The Inventor materials are managed with the Styles and Standards Editor. You can modify existing materials or create new ones. When you create or modify materials, be careful to assign the correct material characteristics.

Material definitions

When a new part is started, the component material is set to whatever the document template uses. With Inventor, as shipped, the document templates for part and assembly use a material called Default. The Default material is not defined for use in the simulation environment. As a result, if the material for any component is assigned the Default, override the material. There are several ways to correct the material assignment:

• Edit the part. In the iProperties, specify a material that is properly defined for simulation use. This solution is the recommended.
• Override the Inventor default material with another properly defined material.
• Modify the Default material to make it usable for simulations. Use caution if you modify the template file to redefine the Default material. Other documents sometimes depend on the original definition.

There are two ways in which a material can be invalid for a simulation.

• The assigned part model material is not fully defined. It is missing critical information to satisfy the simulation requirements. In this case, you receive a warning message about the material. You can override the material with one suited for analysis or modify the existing material before running the simulation.
• The override material is not fully defined. It is missing critical information to satisfy the simulation requirements. The override material node in the browser is decorated with the information icon. You can override the material with one suited for analysis or modify the existing material before running the simulation.

Simulation Browser

In the simulation browser, there is a Materials folder in which you find a list of all materials that override other materials. For example, if you have a Copper component, and override the Copper with Steel, there is a unique node for Steel. The Steel node contains nodes for each part using that material.

The following are assumptions about the behavior of materials:

 Constant All structural material properties do not change with respect to temperature and time. Homogeneous Material properties do not change throughout the volume of the part. Linear Structural Stress is directly proportional to strain.

If a simulation material is better suited to your design needs, promote the material assignment to the model as a CAD edit.

Specify Contact Conditions

There are two methods for adding contact conditions to the simulation:

 Automatic Contacts Software assigned contacts based on the settings in the Edit Simulation Properties dialog box. Automatic contacts can be edited at any time in the process. Manual Contact Contacts you assign through use of the command. Manual contacts can be edited at any time in the process.

Other considerations:

Warning icons at parent browser nodes

State icons display next to parent nodes in the Stress Analysis browser to indicate a node is out-of-date, or issues exist for the child nodes. Initially, the Update Required icon displays next to the parent node. If the Warning icon appears after the node is updated, then an issue exists for one or more child nodes.

Procedures

Simplify parts and assemblies for analysis

Simplifying the model or part contributes to expediting the analysis. You can exclude parts whose purpose is simulated by a constraint and whose structural significance is otherwise small.

To help expedite analyses, you can suppress part features, such as rounds, that are either cosmetic or used to break sharp edges.

NoteAssembly component and part feature exclusions are simulation-specific. As a result, exclusions you make in one simulation do not affect your other simulations.

Exclude Components to Simplify Assemblies

Exclude a part or assembly from analysis:

1. Expand the assembly browser nodes to the level where you see the component to exclude.
2. Right-click the component and select Exclude From Simulation. Alternatively, right-click the component in the graphics region and click Exclude From Simulation.

The display of an excluded component changes to transparent while in the simulation environment.

Exclude Features to Simplify Parts and Assemblies

Suppressing features for analysis can speed up the meshing process. To exclude a part feature in the graphics window from your stress analysis:

1. Change the select filter to Select Features .
2. In the graphics window, select features to exclude, either individually or with multi-select.
3. Right-click and select Exclude From Simulation.

The features become invisible in the graphics window. In the browser, the features are unavailable and show with the Exclude icon . Dependent features are also made invisible and unavailable in the browser.

NoteThe excluded features are suppressed for your stress analysis, but the suppression is ignored when you return to the Part or Assembly modeling environment. Also, you cannot exclude features already suppressed in the modeling environment.

Alternatively, you can select features in the browser to exclude:

1. Expand the part browser node to the level where you see the features you want to exclude.
2. Right-click the feature and select Exclude From Simulation.

If there is an error while creating the finite element mesh, an error dialog box displays. The potentially problematic geometry object highlights, and the mesh creation stops.

Analyze parts or assemblies containing thin wall bodies

To detect thin wall bodies, click Find Thin Bodies in the Prepare panel. If your model contain components that meet thin wall bodies criteria, a message box displays with an option to automatically create midsurfaces from detected thin wall bodies.

If you click OK, Midsurface dialog box opens. Click OK to evaluate the model and create midsurfaces. You can also click the Offset command to manually select face or faces to be analyzed for thin bodies criteria.

All midsurfaces and offsets are listed under Shells node in the browser.

Add a structural ( fixed, frictionless, or pin) constraint:

1. On the ribbon, click the constraint command for the type of constraint to add.
NoteYou can also right-click the Constraints node in the browser and select the appropriate constraint type from the context menu.
2. In the dialog box, the select command is active, so you can immediately select the constraint location. Select the appropriate input for the constraint type. If you select more than one input, the selections must be of the same type: such as face, edge, or vertex. The input type is based on the constraint type.
3. Optionally, you can use the (More) command to expand the dialog box for access to other constraint parameters. The available parameters are based on the constraint type.
4. Click OK to add the constraint and close the dialog box. Alternatively, click Apply to add the constraint and keep the dialog box open.

You can edit or suppress constraints after you run the simulation, then rerun the simulation and see the effect of changing or suppressing the constraint.

NoteYou cannot exclude part-part contact areas from constraints applied to faces containing the contact. Avoid applying improper constraints to contacting faces.

Apply a fixed constraint with non-zero displacement

You can apply a displacement in addition to a fixed constraint. To specify the displacement, do the following:

1. In the Fixed Constraint dialog box, click the (More) button. The dialog box expands to provide access to additional settings.
2. Select Use Vector Components.
3. Select the x, y, or z vector components appropriate for defining your displacement vector.
4. Enter the appropriate displacement magnitudes for each vector component.
5. Click OK to apply the constraint.

Loads are part of the boundary conditions you define for the simulation. There are various load types available to apply:

Access Load Type Inputs Used to...

Force

Faces, edges, and vertices.

When selecting more than one input, all inputs must be the same entity type.

Apply a force of the specified magnitude to the selected faces, edges, or vertices.

By default, Force is applied:

• Normal to the selected face.
• Parallel with the selected edge.
• Using the vector components in the expanded section of the dialog box.

Pressure Face

Apply a pressure of the specified magnitude to the selected faces.

• Pressure is uniform
• Applied Normal to the selected face.

Apply a load of the specified magnitude to the selected face. Forces are predominantly

• Perpendicular to axis (moment)

Moment

Face

Edges (shells only) When selecting more than one input, all inputs must be the same entity type.

Apply a load of the specified magnitude around the axis and perpendicular to the face.

Linear: Face or edge

Angular: Face or edge

Location: Vertex

Apply linear acceleration or angular velocity and acceleration of the specified magnitude to the model.

Linear

Loads are applied perpendicular to the face with the magnitude value. Positive values are applied into the face. Loads are applied parallel to edge selections.

Flip reverses directions.

Angular

Apply angular velocity and acceleration of the specified magnitude normal to a face or parallel to an edge.

Flip reverses directions.

Location

Specifies an alternate location for the body loads. The location is shared between velocity and acceleration.

Gravity Face or Edge

Apply gravity of the specified magnitude normal to the selected face or parallel with the selected edge.

Flip reverses gravity direction.

Vector components define the magnitude and direction of gravity.

Remote Force

Face

Apply a force of the specified magnitude to the selected face.

By default, Force is applied:

• Normal to the selected face.
• Click Flip Direction to change directions.
• Use coordinates to specify the force location.

1. In the Loads panel, click the load type to apply. The applicable load dialog box displays.
NoteYou can also right-click the Loads node in the browser and select the appropriate load type from the context menu.
2. The selector command is active, and you can select inputs in the graphic region immediately. Based on the load type, make the corresponding selection.
3. The selection displays a glyph indicating the direction in which the load is applied. To change the load direction, use the vector components in the expanded section (for applicable load types) to describe the direction.
4. The More section of the dialog box also provides the glyph settings for that load. Adjust the glyph settings, if necessary.
NoteWhen it is appropriate to create multiple loads of the same type, define the load conditions, pick the geometry, and click Apply. The dialog box remains open and you are ready to create the next load. The Apply button is not available for Body and Gravity loads, as a simulation can have only one of each of these load types.

In many applications, different locations on a component surface are subject to different loads. An example is a rotating shaft supported at both ends by bearings. The middle section of the shaft is under a moment, while the ends of the shaft see bearing loads

When you assign bearing loads to components, such as a shaft, you can split faces to create bearing contact locations.

Another example is the application of loads to simulate two individuals seated on a park bench. Split the top bench surface to create locations where you can apply the weight of the individuals.

Override material assignments

Generally, materials are assigned at the Part model level in the components iProperties. There, the Physical Properties tab describes the fundamental aspects of the material. Stress analysis simulations use this information.

One aspect of analysis is to allow comparison of different materials for the design solution. Thus, in each simulation you are able to override the assigned material for a given part or assembly. The override occurs only for the specific simulation and does not affect the assembly model unless you promote changes to the model.

If an override material becomes inadequately defined for simulation purposes, the material node indicates an issue to resolve.

Override the assigned material:

1. Click Stress Analysis tab Material panel Assign to display a dialog box with components and their material assignments.
NoteYou can also double-click the parent Material browser node or right-click the node and select Assign Materials.
2. In the Override Material column, click the cell that matches the component whose material you want to change. The row and associated component browser node and the component in the graphics window, highlight to reflect the selection.
3. Click the pull-down arrow to display the list of materials, and select the desired material. All occurrences of that component receive the material override. Thus, if you have 16 occurrences of a bolt, and override material for one bolt, the action results in overriding material for all 16 bolt occurrences.
NoteYou can copy and paste material overrides. Right-click an Override Material cell and select copy. Then, right-click an Override Material cell and select paste.
4. Specify the material overrides for as many components as you want, then click OK to apply the material changes.
NoteIf the material you want to use is not available in the provided materials, you can define new ones or modify existing ones. See Add a New Material or Edit Materials.

Show all material assignments

View all material assignments in the browser:

1. Right-click the Material parent node and select Show All Materials.
2. Expand the browser material nodes to view component material assignments made at the Part model level , and component material overrides .

Warning icons display in the browser in the following situations:

• Show All Materials is selected and your part has an undefined default material without an override in place.

The icon displays, as some material properties required for your simulation are missing. To eliminate the warning, update the default material at the Part model level or apply a material override.

• Material properties are invalid.

The icon displays if a property is outside the limits for the simulation. For example, if you change the material density to zero, the icon displays for that material. To eliminate the warning, update the material properties, assign a different material, or apply a material override.

• Material is missing.

The icon displays if the assigned material is missing from the Inventor material list. To eliminate the warning, update the material list, assign a different material, or apply a material override.

Work with multiple component materials

You can multi-select rows in the Assign Materials dialog box:

1. Open the Assign Materials dialog box.
2. Click a row on the dialog box.
3. To select multiple rows, press and hold CTRL, and select rows.
4. To multi-select contiguous rows, use SHIFT.
NoteThe selected rows and associated component browser nodes highlight, as do the components in the graphics window.

Assign override materials to your selections:

1. With rows selected, click one of the selected cells in the Override Material column.
2. On the drop-down menu, click the appropriate material selection. All selected rows inherit the same override material.

Copy and paste an override material:

1. Right-click a row and select Copy. The override material associated with the row is copied.
2. Individually select or multi-select the target rows for the override material.
3. Right-click a highlighted row and select Paste. All rows inherit the copied override material.

Delete a material override

For a single component, you can right-click the component node and click Delete Materials. The component and material nodes are removed from the override list. The component material reverts to the previous material.

For a material, right-click the Material node and click Delete Materials. All overrides of that material are removed and the component material reverts to the previous material.

Remove redundant overrides

Removes redundant overrides and aggregates the components under the common override. The command is available in the context menus of the Material node and all its child nodes.

Right-click the node level at which you wish to perform the operation and click Remove Redundant Overrides.

Apply automatic contacts

Automatic contacts are detected during the simulation, without your taking direct action to detect them. If you want to see them before running the simulation or evaluate any that are detected, run the Automatic Contacts command.

To detect contacts, click Automatic Contacts in the Contacts panel.

The model is evaluated and contacts added. The faces must satisfy two criteria:

• The distance between the faces must not exceed the Tolerance value as expressed in the Simulation Properties.
• The angle between the faces must be within 15 degrees of being parallel.

When automatic contacts are generated, geometry decoration for mixed (solid + shell) and pure shell displays in browser indicating the type of contact. There are 3 possible types:

[E-E] Edge-Edge, contact created between two edges

[E-F] Edge-Face, contact created between an edge and a face

[F-F] Face-Face, contact created between two faces

Access to the Tolerance value and contact type is provided in the Simulation Properties on a per simulation basis. The angle requirement is fixed.

You can change the contact type by editing individual contacts or multi-select contacts and change the selection to another contact type.

When necessary, you can manually specify the contact types and components participating in the contact. You can specify the separation tolerance, but cannot change the 15 degree limit.

For example, use a Separation contact type in a weldment where:

• The components form a T shape.
• The vertical component contact face does not bond ideally.

All contacts are listed under the contact node in the browser. The type and participating components display next to the browser node name. Contacts are also listed in the browser as children of the components participating in the contact.

Add contact conditions manually between component faces:

1. First activate the Automatic Contacts command to gather all inferred contacts.
2. Activate the Manual Contact command.
NoteYou can activate Manual Contact from the ribbon, or right-click the Contacts node in the browser and select Manual Contact from the context menu.
3. Select the first component or component face where contact occurs.
NoteTo enhance selection capability, check the filter reference check box. Select the component first, and then specify the contact face.
4. Select the second component or component face where contact occurs. The selected components or faces are colored differently to distinguish the selection order.
5. Specify the contact type. You can specify the contact type before you select the inputs.

Contact type lists applicable contacts for the particular simulation type. Static analysis lists all contact types. Modal analysis lists only Bonded and Spring contact types.

Normal and Tangential Stiffness are values reserved and enabled only for spring contacts.

As you set up your simulation, changes you make to the model can require your attention. In such cases, the parent node of the affected child node displays the Update Required icon . Right-click the parent node and select the applicable Update command. The update is performed and the Warning icon displays next to the parent node when issues still exist. Expand the parent node to view the affected child node as indicated by the Warning icon.

For example, the following is a potential workflow associated with the stress analysis of a bracket assembly.

1. Create a simulation.
2. On the ribbon, click Stress Analysis tab Contacts panel Automatic Contacts
3. Click Manual Contact and add a minimum of one manual contact to the model.
4. Return to the Assembly environment and delete a component involved in a manual contact.
5. Enter the Stress Analysis environment. Note the presence of the Update Required icon next to the Contacts node. Expand all nodes under Contacts and view the Warning icons.
6. Right-click the Contacts node and select Update Automatic Contacts. The solver re-evaluates the interfaces and makes appropriate contact changes.

Since the component involved in the manual contact was deleted, the manual contact cannot be resolved. The Warning icon remains next to this manual contact and the Contacts node also shows a Warning icon.

In general, the Warning icon at the parent note indicates that at least one unsuppressed child node has a warning. If all child nodes with warnings are suppressed, the parent node is treated as healthy and no Warning icon displays.

Find thin bodies

When performing the analysis of parts and assemblies you can simplify you models containing thin bodies.

Prepare thin wall models for analysis:

1. Open a part or assembly file.
2. Click Stress Analysis on the Environments tab.
3. Create a new simulation.
4. On the Prepare panel:
• Click Find Thin Bodies . Solid bodies that meet the thin component criteria are highlighted in the browser. To learn more about thin parts criteria, read the concept chapter above (Simplify the model section).
• Click OK in the message box. Midsurface dialog box opens.
• Click OK in the Midsurface dialog box to generate midsurface from selected solid body components.
• Alternatively, click Offset to manually select faces to create thin shell components.

Important: Loads and Constraints applied to solid components become sick when converted to shell elements. We recommend applying them after you convert the model.

1. Solve the simulation, and view desired results.

How to convert parts back from shells to solids?

In the browser, select the Midsurface or Offset node, right-click and select Delete.

How to view midsurface or offset thickness?

1. In the browser, select the desired Midsurface or Offset node.
2. Right-click, and select Edit Shell. In parametric simulations, the base configuration thickness is displayed.

In parametric simulations, right-click and select Show Thickness. An averaged thickness for particular configuration is displayed.

For midsurfaces, you can only view the body thickness but you are not able to edit it. For offsets, you can edit only the Thickness value which is twice as the Distance value.

How to delete multiple instances of midsurface or offset at once?

1. In the browser, right-click the Shells folder.
2. Click Expand All Children.
3. Select first middle surface (Midsurface:1), or first Offset (Offset:1).
4. Hold the Shift key, and select the last midsurface, or offset.
5. Click Delete.

How to view multiple connectors of midsurface at once?

1. In the browser, right-click the Shells folder.
2. Click Expand All Children.
3. Select first connector (Connector:1).
4. Hold the Shift key, and select the last connector, to check if all the gaps are connected with connectors, or not.

Create thin components (shells) from selected faces

1. In Stress Analysis environment, create a new simulation.
2. On Prepare panel, click Offset .
3. Select a desired face.
4. In the Offset dialog box, specify the thickness. Distance is automatically calculated as half the thickness, and cannot be edited.
5. Click OK.

Generate midsurfaces from thin bodies components

Use Midsurface command to generate midsurface from selected shell component. Only components that meet the shell criteria can be converted to midsurface. A message displays informing you when midsurface cannot be created.

1. In Stress Analysis environment, create a new simulation.
2. On Prepare panel, click Midsurface .
3. Select a body.
4. Click OK in the Midsurface dialog box.

We recommend using Find Thin Bodies command first. If any thin bodies are found, a message box displays. Click OK to open the Midsurface dialog box automatically.

References

Exclude from simulation

Simplifies the assembly for simulation purposes. Excludes component from the Simulation. The setting applies on a per simulation basis.

 Access: Simulation browser Component browser node Context menu

There are distinct differences between excluding a component and suppressing a component.

 Exclude From Simulation Component is removed from the list of components participating in the simulation. Any component can be excluded in any simulation. Excluded components are still witnessed in the assembly and can be seen if you change environments to the assembly environments. Suppress component Are not witnessed in the assembly or other environments including simulation. Cannot be used in any simulation.

Fixed Constraint

Applies a fixed constraint on selected faces, edges, or vertices. The fixed constraint removes all degrees of freedom. That is, the fixed constraint prevents the face, edge, or vertex from moving or deforming.

You can also specify a displacement to apply with the fixed constraint.

 Access: Ribbon: Stress Analysis tab Constraints panel Fixed Alternatively, right-click the Constraints node in the browser and select Fixed Constraint.
 Location The Select command is active when the dialog box is displayed. Select the face, edge, or vertex to designate the constraint location. OK Create the constraint and close the dialog box. Cancel Close the dialog box without creating the constraint. Apply Create the constraint and keep the dialog box open. More Expands the dialog box to reveal additional controls pertinent to the command. Use Vector Components Select to apply a displacement along with the fixed constraint. You define the displacement using vector components. Vector Component x - select and enter the appropriate displacement magnitude along the x-axis. y - select and enter the appropriate displacement magnitude along the y-axis. z - select and enter the appropriate displacement magnitude along the z-axis. Display Glyph Turns on the visibility of the constraint vector glyph. Scale Specifies the glyph scale in model units. Specifies the glyph color. Name Constraint name - a default is provided, but you can give the constraint a more meaningful name for future or presentation reference.

 Edit Fixed Constraint Displays the Edit Fixed Constraint dialog box where you modify the values originally placed on the constraint. Reaction Forces Displays the Reaction Forces dialog box with the Reaction force and Reaction moment values. The values display zero until results of a simulation are available. Suppress Suppresses the selected constraint. When a constraint is suppressed, some other context menu entries are not available. Copy Copies the selected constraint. Select the Constraints folder and use the context menu Paste command to apply the copied constraint. Delete Deletes the selected constraint.

Pin Constraint

Applies a rotational constraint on the selected combination of cylindrical faces.

 Access: Ribbon: Stress Analysis tab Constraints panelPin Alternatively, right-click the Constraints node in the browser and select Pin Constraint.
 Location The Select command is active when the dialog box is displayed. Select cylindrical faces on which to apply the constraint. OK Create the constraint and close the dialog box. Cancel Close the dialog box without creating the constraint. Apply Create the constraint and keep the dialog box open. More Expands the dialog box to reveal additional controls pertinent to the command. Fix Radial Direction Cylindrical surfaces cannot move, rotate, or deform radially to the cylinder. Fix Axial Direction Cylindrical surfaces cannot move, rotate, or deform axially to the cylinder. Fix Tangential Direction Cylindrical surfaces cannot move, rotate, or deform tangentially to the cylinder. Name Constraint name - a default is provided, but you can give the constraint a more meaningful name for future or presentation reference.

 Edit Pin Constraint Displays the Edit Pin Constraint dialog box where you modify the values originally placed on the constraint. Reaction Forces Displays the Reaction Forces dialog box with the Reaction force and Reaction moment values. The values display zero until results of a simulation are available. Suppress Suppresses the selected constraint. When a constraint is suppressed, some other context menu entries are not available. Copy Copies the selected constraint. Select the Constraints folder and use the context menu Paste command to apply the copied constraint. Delete Deletes the selected constraint.

Frictionless Constraint

Applies a frictionless constraint on selected faces. A frictionless constraint prevents the surface from moving or deforming in the normal direction relative to the surface. The surface is free to rotate, move, or deform in a tangential direction to the applied frictionless constraint.

 Access: Ribbon: Stress Analysis tab Constraints panelFrictionless Alternatively, right-click the Constraints node in the browser and select Frictionless Constraint.
 Location The Select command is active when the dialog box is displayed. Select a face to designate the constraint location. OK Create the constraint and close the dialog box. Cancel Close the dialog box without creating the constraint. Apply Create the constraint and keep the dialog box open. More Expands the dialog box to reveal additional controls pertinent to the command. Name Constraint name - a default is provided, but you can give the constraint a more meaningful name for future or presentation reference.

 Edit Frictionless Constraint Displays the Edit Frictionless Constraint dialog box where you modify the values originally placed on the constraint. Reaction Forces Displays the Reaction Forces dialog box with the Reaction force and Reaction moment values. The values display zero until results of a simulation are available. Suppress Suppresses the selected constraint. When a constraint is suppressed, some other context menu entries are not available. Copy Copies the selected constraint. Select the Constraints folder and use the context menu Paste command to apply the copied constraint. Delete Deletes the selected constraint.

Force

Applies a force of the specified magnitude to the selected faces, edges, or vertices. When selecting multiple entities, the selection is limited to the same type as your first selection.

 Access: Ribbon: Stress Analysis tabLoads panelForce Alternatively, right-click the Loads node in the browser and select Force Load.
 Location Specifies the face, edge, or vertex on which to apply the load. Direction Specifies the force direction. The default direction is normal to the selected face and with the magnitude value. Magnitudes are applied into the face.   The Direction Selector is automatically active allowing you to select geometry to define a different load direction.   The Direction Reverse command inverts the direction of the selected vector. Magnitude Specifies the force magnitude. OK Create the force and close the dialog box. Cancel Close the dialog box without creating the force. Apply Create the force and keep the dialog box open. (More) Expands the dialog box to reveal additional controls for specifying the force vector and controlling glyph display. Use Vector Components Enables vector controls so that you can define more explicitly the force load vector. Specify the magnitude for the appropriate vector components for: Vector Components Fx = X component Fy = Y component Fz = Z component Display Glyph When checked, displays the force glyph in the graphics region. Scale Specifies scale of the force glyph. You can increase or decrease the glyph size. Specifies the force glyph color. Name Specifies a name for the load. The name you specify is displayed in the browser.

Pressure

 Access: Ribbon: Stress Analysis tabLoads panelPressure Alternatively, right-click the Loads node in the browser and select Pressure Load.
 Faces Specifies a face to which the pressure load is applied. Magnitude Specifies the magnitude of the pressure load. OK Create the pressure load and close the dialog box. Cancel Close the dialog box without creating the pressure load. Apply Create the pressure load and keep the dialog box open. (More) Expands the dialog box to reveal glyph display controls. Display Glyph When checked, displays the pressure load glyph in the graphics region. Scale Specifies scale of the pressure load glyph. You can increase or decrease the glyph size. Specifies the pressure load glyph color. Name Specifies a name for the load. The name you specify is displayed in the browser.

Bearings loads vary greatly over the size and directions of forces that they can support. Forces can be predominately axial (thrust bearings) or radial.

Moment

 Access: Ribbon: Stress Analysis tabLoads panelMoment . Alternatively, right-click the Loads node in the browser and select Moment Load.
 Location Specifies the face or faces to which the moment is applied. Direction Moment loads are applied around the axis and perpendicular to the face. OK Create the moment and close the dialog box. Cancel Close the dialog box without creating the moment. Apply Create the moment and keep the dialog box open. (More) Expands the dialog box to reveal additional controls for specifying the moment load vector. Use Vector Components Enables vector controls so that you can define more explicitly the moment vector. Specify the magnitude for the appropriate vector components for: Vector Components Mx = X component My = Y component Mz = Z component Display Glyph When checked, displays the moment load glyph in the graphics region. Scale Specifies scale of the moment load glyph. You can increase or decrease the glyph size. Specifies the moment load glyph color. Name Specifies a name for the moment load. The name you specify is displayed in the browser.

Defines linear acceleration for the model.

 Access: Ribbon: Stress Analysis tabLoads panelBody - Linear tab Alternatively, right-click the Loads node in the browser and select Body Load. Then, select the Linear tab in the dialog box.
 Linear Enable Linear Acceleration Enables the controls for specifying the linear acceleration parameters. Valid selections are face or edge. Direction Specifies the acceleration vector. A Normal vector is applied perpendicular to the face and with the magnitude value. When an edge is selected, the loads are applied parallel to the selected edge. The Direction Selector is automatically active allowing you to select geometry to define the vector. The Direction Reverse command inverts the direction of the specified vector. Magnitude Specifies the linear acceleration magnitude. OK Create the body load and close the dialog box. Cancel Close the dialog box without creating the body load. (More) Expands the dialog box to reveal additional controls for specifying the Body Loads vector. Use Vector Components Enables vector controls so that you can define more explicitly the body loads vector. Specify the magnitude for the appropriate vector components for: Location X = X component Y = Y component Z = Z component Display Glyph When checked, displays the load glyph in the graphics region. Scale Specifies scale of the load glyph. You can increase or decrease the glyph size.

Defines angular velocity or angular acceleration for the model.

 Access: Ribbon: Stress Analysis tabLoads panelBody - Angular tab Alternatively, right-click the Loads node in the browser and select Body Load. Then, select the Angular tab in the dialog box.

Based on the options you can select, there are three cases possible:

• Velocity and Acceleration have the same rotation axis. The location point is unspecified. The solver chooses a point along the axis.
• Velocity and Acceleration have a different rotation axis. The location point is unspecified. The solver chooses a point on the Velocity rotation axis. Acceleration is transformed to the location point on the Velocity rotation axis.
• Velocity and Acceleration have a different rotation axis. The location point is specified. This case is the same as when you define the point with the vector components.
 Angular Enable Angular Velocity and Acceleration Enables the controls for specifying angular velocity and acceleration. Valid selections are faces and edges. Velocity Direction Specifies the direction of angular velocity. A Normal vector is applied perpendicular to the face and with the magnitude value. When an edge is selected, the loads are applied parallel to the selected edge. The Direction Selector is automatically active allowing you to select geometry to define the load direction. The Direction Reverse command inverts the direction of the selected vector. Magnitude Specifies the angular velocity magnitude. Acceleration Direction Specifies the direction of angular acceleration. A Normal vector is applied perpendicular to the face and with the magnitude value. When an edge is selected, the loads are applied parallel to the selected edge. The Direction Selector is automatically active allowing you to select geometry to define the vector. The Direction Reverse command inverts the direction of the specified vector. Magnitude Specifies the angular acceleration magnitude. Location Allows you to change the location of the initial Velocity and/or Acceleration selection while maintaining the specified orientation. Select a vertex and the location you choose is common to both the Velocity and Acceleration selections. OK Create the body load and close the dialog box. Cancel Close the dialog box without creating the body load. (More) Expands the dialog box to reveal additional controls for specifying the angular velocity and acceleration vector. Use Vector Components Enables vector controls so that you can define more explicitly the body load vector and magnitude. Specify the magnitude for the appropriate vector components and the applicable location for: Velocity X component Y component Z component Acceleration X component Y component Z component Location X component Y component Z component Display Glyph When checked, displays the load glyph in the graphics region. Scale Specifies scale of the load glyph. You can increase or decrease the glyph size.

Gravity

 Access: Ribbon: Stress Analysis tabLoads panelGravity Alternatively, right-click the Loads node in the browser and select Gravity Load.
 Direction Specifies the direction of gravity. This direction can be normal (perpendicular) to the face and with the magnitude value. When an edge is selected, the loads are applied parallel to the selected edge. The Direction Selector is automatically active allowing you to select geometry to define the load direction. The Direction Reverse command inverts the direction of the selected vector. Magnitude Specifies the acceleration applied to the assembly in the context of the simulation. OK Create the gravity load and close the dialog box. Cancel Close the dialog box without creating the gravity load. (More) Expands the dialog box to reveal additional controls for specifying the gravity vector. Use Vector Components Enables vector controls so that you can define more explicitly the gravity vector. Specify the magnitude for the appropriate vector components for: Vector Components g[X] = X component g[Y] = Y component g[Z] = Z component Display Glyph When checked, displays the gravity load glyph in the graphics region. Scale Specifies scale of the gravity load glyph. You can increase or decrease the glyph size.

Remote Force

 Access: Ribbon: Stress Analysis tabLoads panel Remote Force Alternatively, right-click the Loads node in the browser and select Remote Force Load.
 Location Specifies the face on which to apply the remote load. Direction Specifies either a Normal or directional force. A Normal force is applied perpendicular to the face and with the amplitude value. The Direction Selector is automatically active allowing you to select geometry to define the load direction. The Direction Reverse command inverts the direction of the selected vector. Magnitude Specifies the force magnitude. Remote Point Specifies the X, Y, and Z components of the remote force location OK Create the remote force and close the dialog box. Cancel Close the dialog box without creating the remote force. Apply Create the remote force and keep the dialog box open. (More) Expands the dialog box to reveal additional controls for specifying the force vector. Use Vector Components Enables vector controls so that you can define more explicitly the remote force vector. Specify the magnitude for the appropriate vector components for: Vector Components Fx = X component Fy = Y component Fz = Z component Display Glyph When checked, displays the force glyph in the graphics region. Scale Specifies scale of the force glyph. You can increase or decrease the glyph size. Specifies the force glyph color. Click to display the color selector and specify a different color. Name Specifies a name for the load. The name you specify is displayed in the browser.

Assign Materials

The Assign Materials dialog box lists the assembly and components in hierarchical order. Each component can use either the originally assigned material, or you can override the material selection with another from the Material Library list provided. Material overrides are applied per simulation, thus one component can have several material assignments each in a different simulation within the same assembly document.

If appropriate, you can work with multiple component material rows simultaneously (See Work with multiple component materials under Prepare for Analysis.)

 Access: Ribbon: Stress Analysis tabMaterial panel Assign Alternatively, you can double-click the parent Material browser node or right-click the node and select Assign Materials.

To define a new material or modify an existing one, see Add a New Material or Edit Materials.

When assigning an override material to a component with more than one instance in the assembly, all instances update to reflect that material. Material overrides are listed in two places in the simulation browser. In the Materials folder, they display by material. The components using that material display as child nodes.

When you assign material overrides, the dialog box presents the following information and options:

 Component Hierarchical list of components in the assembly. All instances of components are displayed. Original Material The material currently assigned to a specific component. Override Material The material you assign to analyze a different material. Safety Factor Specifies whether to use Yield Strength or Ultimate Tensile Strength when determining the Safety Factor. The default setting is Yield Strength. The setting affects the component material for that simulation.   For ductile materials, select Yield Strength. For brittle materials, select Ultimate Tensile Strength.

Edit Material Overrides

There are two ways to edit material overrides:

 Delete Materials Removes the material override. The command is accessed only through the context menu of either the material or component nodes. Right-click the material node and click Delete Materials. Override material node is removed from the browser. Components using the material override revert to the assigned material of their component. To remove the material override from one component and not all components using it, expand the override material node, locate the component. Right-click the component node and click Delete. The material override is removed from that component alone. The component material is reverted to its previous setting. Remove Redundant Overrides Inspects the overrides of component nodes and deletes redundant material overrides. The command is available in the context menus for the Material node and all child nodes.

Modify Material Properties

When you add or modify materials for use with simulation, define the following properties carefully:

• Young’s modulus must be greater than zero.
• Density and Yield Strength must be greater than zero.
• Poisson’s ratio must be between 0 and 0.5, but not equal to 0.5.

Promote Materials

 Promote materials to model Accessed from the component browser node context menu, this command promotes the override material into the component file. The component file is edited and the material is changed to the promoted material. The override cell updates to display As Defined. Other simulations using the override are not updated. Use the Remove Redundant Overrides command to update each simulation. For each component whose material is promoted, that component is removed from the Material browser folders. When no materials exist in a node, the node is removed. NoteWith Show All Materials active, the component is not removed from the Material browser folder. Only the icon is changed to reflect that the material is no longer an override.

Automatic Contacts

 Access: Ribbon: Stress Analysis tabContacts panelAutomatic Alternatively, right-click the Contacts node in the browser and select Automatic Contacts.

The command executes immediately when clicked.

The default contact type, bonded, is specified in the Stress Analysis Settings.

Also, you specify the contact tolerance, the maximum distance within which a contact is deemed inferred and a contact is assigned.

Manual Contact

Adds manual contact conditions to selected geometry elements.

 Access: Ribbon: Stress Analysis tabContacts panelManual Alternatively, right-click the Contacts node in the browser and select Manual Contact.
 Contact type Select the contact type from the choices in the pull down list. Available contact types differ based on the simulation type. Selections Specify the first contact edge or face. Specify the second contact edge or face. Specifies that you want to pick the part first, before the contact face. This command is useful when one or more parts lie atop one another and graphic selection is tedious.

Available Contact Types

Contact type Behavior
Bonded

Bonds contact faces to each other rigidly.

Separation

Separates contact faces partially or fully while sliding

Sliding / No Separation

Bonds contact faces in normal to face direction while sliding under deformation.

Separation / No Sliding

Separates contact faces partially or fully without their sliding against each other.

Shrink Fit / Sliding

Provides conditions like 'Separation' with initial parts overlapping. The initial distance between the contact faces is negative

Shrink Fit / No Sliding

Provides conditions of Separation/no sliding with initial parts overlapping, meaning negative initial distance

Spring

Creates equivalent springs between the two faces. You define total Normal and/or Tangential stiffness.

Normal Stiffness Specifies the equivalent normal stiffness value. Applicable to Spring contact only.
Tangential Stiffness Specifies the equivalent tangential stiffness value. Applicable to Spring contact only.
NoteNormal and tangential directionality is based on the best approximation between the two faces that follow each other in a parallel way. Examples are parallel planes, concentric cylinders, and so on. Otherwise it can be ambiguous.

The following two options are accessible from the context menu for Contacts:

 Edit Contact Displays the Edit (Type) Contact dialog box so you can edit the contact type. Suppress Suppresses the select contact.

Convergence Settings

Result convergence criteria consists of a collection of entities, the results type you want, the number of refinements, Stop Criteria, and the refinement threshold. The goal of convergence criteria is to specify the result type and maximum number of h refinements desired to reach convergence. Convergence can occur in fewer refinements than requested in the settings dialog box. The resulting Convergence Plot displays:

This information is specified in the Convergence Settings dialog box.

 Access: Ribbon: Stress Analysis tabMesh panelConvergence Settings

To set convergence criteria, click the Convergence Settings command, and in the dialog box that displays specify the preferred settings.

Convergence Settings - Static Simulations

 Maximum Number of h Refinements Specifies the maximum number of h refinement cycles for convergence. Default is 0. For values higher than 2, a dialog box displays. Increasing the number of refinements could decrease performance. Value increment is 1. If the Stop Criteria is met, the refinements can cease before the maximum number is reached. Stop Criteria (%) Ceases refinement when the difference between the last two results is less than the specified (%) value. Value increment is 1. The refinement can also cease when the maximum number of refinements is reached, regardless of whether Stop Criteria is met. h Refinement Threshold (0 to 1) Specifies the refinement threshold (between 0 to 1). A zero setting means include all the elements in the set as candidates for refinement. The results are the maximum refinement per cycle. 1 means exclude all elements in the set from refinement, as in no refinement. The default is .75, which means, of the elements with equivalent errors at the top, 25% are subject to refinements. Not applicable to Modal analysis. Value increment is 0.1. Results to Converge Von Mises Stress Specifies Von Mises Stress as the result component. 1st Principal Stress Specifies 1st Principal Stress as the result component. 3rd Principal Stress Specifies 3rd Principal Stress as the result component. Displacement Specifies Displacement as the result component. Geometry Selections All Geometry Specifies that all geometry is considered for the convergence criteria. Include Selected Geometry Specifies that only the items in the list are included as the set in the convergence criteria. Exclude Selected Geometry Specifies that the items in the list are excluded from the set in the convergence criteria. Bodies Filters the list to display only bodies. Faces Filters the list to display only faces.

Convergence Settings - Modal Simulations

 Maximum Number of h Refinements Specifies the maximum number of h refinement cycles for convergence. Default is 0. For values higher than 2, a dialog box displays. Increasing the number of refinements could decrease performance. Stop Criteria (%) Ceases refinement when the difference between the last two results is less than the specified (%) value. Results to Converge Frequency Mode Specifies the mode number for results convergence.

Midsurface

Inspects the selected bodies, and if they meet the shell feature criteria, converts them to shell features defined by midsurface.

 Access: Ribbon: Stress Analysis tabPrepare panelMidsurface

A dialog box opens automatically when you compute the Find Thin Bodies command first, and any thin bodies are detected within your component. In the displayed message box, click OK.

 Solid Bodies Select a solid body from which you want to create a midsurface.

Offset

Inspects the selected bodies, and if they meet the shell feature criteria, creates a shell component from selected faces.

 Access: Ribbon: Stress Analysis tabPrepare panelOffset
 Faces Specifies a face to which create an offset. Automatic Face Chain Select the check box to create a chain of selected face. Thickness Specify the thickness. This value is independent of distance, and cannot be a zero value. Distance Distance value is automatically calculated as half the thickness, and cannot be edited. Enable/Disable Feature Preview Select the check box to preview the shell before it is created.

Shell Thickness

 Access: Simulation browser Midsurface or Offset browser node Context menu (Show Thickness)
NoteContext menu option is only available in parametric simulations.
 Thickness Displays the averaged thickness for particular configuration in a parametric dimension simulation. This averaged thickness is sent to solver for analysis.