Mechanical Tab

Boundary Condition Type

Notes

Displacement

Specifies the displacement constraint.

Select the directions to constrain the displacement and enter the values.

If 0 is entered in a direction, there will be no displacement in that direction. For the forced displacement, enter the displacement value.

If [Constrain the freedom of shells] is selected on the analysis condition, the rotation can be constrained too.

Select [Use distribution data] to define the distribution.
See "Options for Mechanical Boundary Condition" below

Normal Displacement

Sets the displacement normal to the set face.

It sets the normal displacement without constraining the displacement in the inward direction of the face.

To fix a displacement, enter 0. For the forced displacement, enter the displacement value.

Rotational Displacement

Specifies the rotation angle around the specified axis.

The axis is defined by Coordinates on Axis and Vector of Axis.

For the positive angle, the rotational direction is clockwise with reference to the axial vector. It is counter-clockwise for the negative angle.

Displacement in the rotation axis direction and radius direction are not constrained.

Like torque load, the load is observed only in the rotational direction.

The trace may not become arc as the displacement in the radius direction is not constrained.

If [Rotate at constant radius] is selected,
the trace will always become arc.
Here, constraint in the radius direction will occur and it will create the load in the radius direction.

If [Constrain displacement in axis direction] is selected,
displacement in the rotation axis direction is constrained.

• If the rotation angle is 0, the rotation can be constrained.

Acceleration

Sets the acceleration vector on the set face.

If [Constrain the normal displacement] is selected,
the normal displacement to the set vector will be constrained, and its acceleration will be 0.

• This can be used in the harmonic and transient analyses of the stress, and the harmonic analysis of the piezoelectricity.
  

Lumped Vertex Load

Applies the lumped load on a vertex

If [Constrain the freedom of shells] is selected in the [Analysis Condition Setting] dialog box, rotational force or moment can be applied.

• If this is applied on a face or an edge, all the nodes on the face or the edge will be given this load.
  That means the total load is smaller for the coarse meshes
  and bigger for the fine meshes.
  

• It cannot be selected in resonant analysis. It will be ignored.
  

Distributed Edge Load

Sets the distributed edge load by the load per unit length [N/m] in any direction.

Alternatively you may select "Set the total load" and enter the total load [N] instead of the load per unit length.

The total load will be distributed evenly to all the edges selected for the boundary.

• This can be set only on the edge topologies of solid bodies. This cannot be set on the vertex/face topologies or sheet bodies.

• Not allowed in the resonant analysis. It will be ignored.

Distributed Face Load

Sets the distributed face load by the load per unit area [N/m2] in any direction.

Alternatively you may select [Set the total load] and enter the total load [N] instead of the load per unit length.

The total load will be distributed evenly to all the faces selected for the boundary.

The list below indicates the possible topologies and how the total load is distributed when selected.

If [Set the total load] is deselected, you can define the distribution by selecting [Use distribution data].
See [Options for Mechanical Boundary Condition] below

If [Constrain the freedom of shells] is selected in the [Analysis Condition Setting] dialog box, rotational force or moment can be applied.

• It cannot be selected in resonant analysis. It will be ignored.

Pressure

Sets the pressure on the face (or edge in 2D). The normal and inward direction onto the face (edge)

is defined positive as shown below.

Alternatively you may select [Set the total load] and enter the total load [N] instead of the load per unit length. The load will be distributed evenly to all the faces selected for the boundary.

If [Set the total load] is deselected, you can define the distribution by selecting [Use distribution data].

See "Options for Mechanical Boundary Condition" below

• Not allowed to apply on vertex. It will be ignored.

• Not allowed in the resonant analysis. It will be ignored.
  Exceptionally, selectable only if [Initial Stress] > [Specify static load for boundary condition] is selected.

Torque Load

Specifies the torque load around the specified axis. If the torque is positive, its direction is clockwise with reference to the axial vector. If the torque is negative, the direction is counter-clockwise.

The axis is defined by Coordinates on Axis and Vector of Axis.

The torque can be applied on vertex, edge or face.

The same-name torque can be applied on multiple number of vertices, edges or faces. In that case, the average distance from the rotation axis is calculated, and

the load [N] is the torque [Nm] divided by the average distance.

The same-name torque can be used for the same type of topologies.

Joint Load

Sets the attractive load or the repulsive load to the joint load boundary pair.

The joint load boundary conditions are paired on the [Boundary Pair] of [Analysis] to set the joint load value.

See [Joint Load Boundary] for the [Constrain except axial direction] option, which simulates the actual constraint imposed by a bolt.

• The joint load boundary condition for pairing must have a different name.

• Allowed to set to any of the vertex, edge, and face topologies. However, the same-name joint load boundary can be set to the same type of topologies only.

• Not available in the piezoelectric analysis.
  

Simple Contact

Analyzes the behaviors of two bodies meeting on a face (or on an edge in 2D).

There are 6 types of contacts.

In the simple contact, slip, off contact, and automatic judgment (1.coefficient of friction: zero, no peeling, 2.with friction, 3.with peeling) are selectable.

Bond requires no setting. It is equivalent to the state with no boundary condition (no constraint).

Specify the right one for your analysis.

Bond * No specific setting required.	The faces are completely bonded.
Slip	The faces slip each other in the tangent direction. They stay in contact and are not separated.
Off Contact	The faces are off contact completely. They don't interact each other. One might penetrate the other depending on the loading direction.
Automatic Judgment (with coefficient of friction of zero, and no peeling taken into account)	The stress on the face is calculated and automatically judged. It will be "Slip" for the compressive stress. It will be "Off contact" for the tensile stress. Off contact (tensile stress) Slip (compressive stress)
Automatic Judgment (with friction)	The friction is taken into account if the coefficient (u) is non-zero.   The stress on the face is calculated and automatically judged . In the case of the compressive stress: Given the normal force N and the tangent force F, if F < uN, it will be "Bond" = static friction if F > uN, it will be "Slip" = kinetic friction   It will be "Off contact" for the tensile stress.   Off contact (tensile stress) Bond (F < μN) Slip (F＜μN)
Automatic Judgment (with peeling)	If the tensile peel strength is selected, the normal stress σ on the face is calculated and judged as follows.   σ is smaller than the tensile peel strength: "Bond" σ is larger than the tensile peel strength: "Off contact"     If the shear peel strength is selected, the shear stress on the face is calculated and judged as follows. τ is smaller than the shear peel strength: "Bond" τ is larger than the shear peel strength: "Off contact"   if it is larger than the peeling strength, it is automatically judged as "off contact".   Off contact (stress at boundary > peel strength) Bond (compressive stress) Bond (stress at boundary < peel strength)

• The simple contact can be set only on the faces where two bodies are in contact beforehand.
  (Select the contact surface to analyze the situation where the bodies originally separated are going to contact.)
  

• Multiple number of iterative calculations will be required to settle all the status of faces under the automatic judgment.

• The iterative calculations might not converge in the automatic judgment with coefficient of friction of zero and no peeling taken into account.
  The following could be effective to solve it:
  1) Set the near-zero coefficient of friction.
  2) Set "bond", "slip", or "off contact" individually, if necessary.
  

• Coefficient of friction and peel strength cannot be taken into account simultaneously for the automatic judgment.
  

• It cannot be selected in resonant analysis. No calculation will be done.

• Calculation is not executed if the shell elements exist in the model.

• The "off contact" condition can be achieved by selecting "Discontinuous" on the Symmetry/Continuity tab too.

• If the simple contact is used in the piezoelectric analysis, the contacting face is calculated with the relative permittivity of 1.0. The electric field which pass through the contacting face cannot be taken into account.
  

• In the analysis with peeling taken into account, if the portion that has peeled once comes into contact again, the contact is treated as slip.

Contact Surface

Specifies the faces subject to the contact analysis as contact surface.

It will be either the contactor surface or the contactee surface.

If one is designated as contactor, the other should be contactee.

Their boundary conditions need to be paired on the the Boundary Pair dialog.

When the friction is taken into account, set the coefficient of friction during the pairing.

• The contactor surface could be face, edge or vertex for 3D, and edge or vertex for 2D.

• The contactee surface is required to be face for 3D or edge for 2D.

• See the technical note for the detail.

Spring Connection

Generates the spring force according to the relative deflection of the spring connection boundary pair.

The spring connection boundary conditions are paired on the [Boundary Pair] dialog box of [Analysis] to set the spring constant type and the values of the components.

• The spring connection boundary conditions for pairing must have different names.

• Allowed to set to any of the vertex, edge, and face topologies. However, the same-name spring connection boundary can be set to the same type of topologies only.

• Not available in the piezoelectric analysis.
  

Remote Load

Takes into account the distributed load and the torque load between the remote point and the boundary.

Its results are equivalent to those of the distributed load and torque load combined.

Contributes to simplifying the analysis model.

Requires the setting of the coordinates of the remote point and the setting of the load.

• The axisymmetric analysis is not supported.

Acoustic Impedance

Takes into account the influence of the surrounding medium such as air and water. Refer to Terminology in Acoustic and Piezoelectric Analysis.

Requires to be set so that the results of analysis and experiment match. Alternatively, a method in Example 23: Air Damping of Cantilever can be used as well.

Available in the piezoelectric solver, but ignored in the static analysis.

Not allowed to use unless the piezoelectric-transient analysis or the transient analysis using resonant mode is selected.

Used to analyze the resonant mode if the piezoelectric-transient analysis or the transient analysis using resonant mode is selected.

Not available in the stress analysis..

Open Boundary

Available for the piezoelectric analysis. See Open Boundary Tab.

Also see Example 16 of Piezoelectric Analysis and a technical note [PML].

Not available in the stress analysis..

Free

Mechanically no constraint at all.

Setting Items

Notes

Time Dependency

Selectable in the stress analysis if

the transient analysis or

the static analysis is selected for [Analysis type], and [Multi step/Multi-step thermal load analysis] is selected on the Step/Thermal Load tab.

Select Time Dependency and click Weight Function. [Time-Weight] table
(or [Step-Weight] table if time is not set) will appear. Fill in the table to set the variation over time.

Transient analysis is available in an optional package.

Set ON/OFF

Selectable in the stress analysis if

[Analysis type] is static analysis, and [Multi step/Multi-step thermal load analysis] is selected on the Step/Thermal Load tab.

It can be set if the boundary condition type is displacement, normal displacement, rotational displacement,
lumped vertex load, distributed edge load, distributed face load, pressure, or torque load.

It can set or remove boundary condition at the specific step in the multi-step analysis/multi-step thermal load analysis.

Select Set ON/OFF, and click ON/OFF List.
Time Table window (Boundary Condition ON/OFF tab and the weight function tab) will show up.

You can confirm time, step, Initial temperature and reached temperature.

Also, you can confirm the weight function which is created by the setting at ON/OFF setting.

If the boundary condition type is displacement, normal displacement, or rotational displacement,
when switched from OFF to ON, the specified value is reached in one step.
when switched from ON to OFF, the constraint is lifted the first substep.

If the boundary condition types are lumped vertex load, distributed edge load, distributed face load, pressure, or torque load,
when switched from OFF to ON, the specified value is reached in one step.
when switched from ON to OFF, the value reaches zero in one step.

It can be used together with the setting of time dependency (weight function).

Uniform Displacement

Sets the boundary to have the uniform displacement.

It can be set in UX, UY and UZ directions individually.

The faces having the same boundary condition are to have the same displacement even if they are physically separated.

If "Constrain the freedom of shells" is selected on the analysis condition,
the rotation (RX, RY, RZ) of shell elements will be the same.

This is applicable, for example, for the boundary where a very hard material is pressed.

• An example is on Example 21 of Stress Analysis.

Rigid Face

Select the rigid face boundary condition.

If selected, it allows all the selected faces to belong to the same rigid body, resulting in zero relative displacement.

The rigid body attribute serves in a similar way. For the details, please refer to the Analysis Domain tab.

• See Example 73 of the stress analysis for the usage.
  

• It is not supported in the piezoelectric analysis.
  

Use Distribution Data
(Distribution Data)

Selectable for Displacement, Distributed face load (total load deselected), and Pressure.

In the case of Displacement

Use distribution data
sets the distributed displacement.

In the case of Distributed face load

Use distribution data
sets the distributed face load.

In the case of Pressure

Use distribution data
sets the distributed pressure.

Click the Distribution Data button to open the dialog box.
See [How to Set Distributed Boundary Condition and Body Attribute] for the detail.