On this page:
7.3.1 Cubit Boundary Conditions
7.3.2 Using CFD Boundary Conditions
7.3.3 Using Constraints
7.3.4 Using Contact Surfaces
7.3.5 Cubit Initial Conditions
7.3.6 Using Loads
7.3.7 Miscellaneous Boundary Condition Commands
7.3.8 Using Restraints
7.3.9 Boundary Condition Sets
2021.11

7.3 Non Exodus

7.3.1 Cubit Boundary Conditions

 

In Cubit, boundary conditions are applied to sidesets or nodesets.  Sidesets and nodesets can contain geometry or mesh.  This means that models can be remeshed without worrying about losing boundary condition data if the boundary condition is applied to a geometry-based sideset/nodeset. The sideset/nodeset used by a boundary condition will be visible to the user, and the user can modify the sideset/nodeset separately from the boundary condition.  Sidesets/nodesets can be assigned to (or removed from) a boundary condition at any time. Boundary conditions are broken into four groups: Restraints, loads, contact, and cfd. Each restraint that is created will belong to a restraint set, each load will belong to a load set, and each contact definition will belong to a contact set. A boundary condition set consists of any number of restraints, contact pairs, and loads. CFD boundary conditions do not belong to boundary condition sets.


Overview of boundary condition entities available in Cubit

Entity

Description and scope

FEA Boundary Conditions

Acceleration

Creates an acceleration boundary condition (acts on a body, volume, surface, curve, or vertex)

Velocity

Creates a velocity boundary condition (acts on a body, volume, surface, curve, or vertex)

Boundary Condition Set

Creates a BC set (contains restraint, load and contact sets)

Contact Region

Creates a contact region between two surfaces or two curves

Contact Pair

Creates a contact pair between two previously defined contact regions

Convection

Creates a convection boundary condition (acts on 2d elements)

Displacement

Creates a displacement boundary condition (acts on a body, volume, surface, curve or vertex)

Temperature

Create a temperature boundary condition (acts on a surface, curve or vertex)

Force

Creates a force boundary condition (acts on a surface, curve or vertex)

Pressure

Creates a pressure boundary condition (acts on a surface or curve)

Heat flux

Creates a heat flux boundary condition (acts on a surface or curve)

CFD Boundary Conditions

Inlet Velocity

Creates an inlet velocity boundary condition

Inlet Pressure

Creates an inlet pressure boundary condition

Inlet Massflow

Creates an inlet massflow boundary condition

Outlet Pressure

Creates an outlet pressure boundary condition

Farfield Pressure

Creates a farfield pressure boundary condition

Axis

Creates an axis boundary condition

Exhaust Fan

Creates an exhaust fan boundary condition

Fan

Creates an fan boundary condition

Inlet Vent

Creates an inlet vent boundary condition

Intake Fan

Creates an intake fan boundary condition

Interface

Creates an interface boundary condition

Interior

Creates an interior boundary condition

Mass Flow Inlet

Creates an mass flow inlet boundary condition

Outflow

Creates an outflow boundary condition

Outlet Vent

Creates an outlet vent boundary condition

Periodic

Creates an periodic boundary condition

Periodic Shadow

Creates an periodic shadow boundary condition

Porous Jump

Creates an porous jump boundary condition

Radiator

Creates an radiator boundary condition

Symmetry

Creates a symmetry boundary condition (acts on a surface)

Wall

Creates an wall boundary condition

 

7.3.2 Using CFD Boundary Conditions

Cubit supports the following CFD boundary condition types. All use the same syntax and use the same command panel (shown below) to create and modify the boundary condition.

The GUI Command Panel for creating an Axis boundary condition is shown below.

Figure 481:

Cubit can export models to the Fluent mesh format and supports defining the above CFD boundary conditions. Only the region on which the BC acts can be defined in Cubit. The data associated with each boundary condition (pressure, velocity, mass values) is not defined within Cubit and must be assigned using a CFD model editor, such as Fluent. The following shows the commands for creating and modifying some sample CFD boundary conditions. To delete them, use the delete command (see Miscellaneous Commands).

7.3.2.1 Inlet Velocity

To create and modify inlet velocity

Create Inletvelocity [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Inletvelocity [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.2.2 Inlet Pressure

To create and modify inlet pressure

Create Inletpressure [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Inletpressure [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.2.3 Inlet Massflow

To create and modify inlet massflow

Create Inletmassflow [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Inletmassflow [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.2.4 Outlet Pressure

To create and modify outlet pressure

Create Outletpressure [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Outletpressure [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.2.5 Farfield Pressure

To create and modify farfield pressure

Create Farfieldpressure [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Farfieldpressure [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.2.6 Symmetry

To create and modify symmetry

Create Symmetry [id] [name <’name’>] [{Add|On {Surface} <entity_list>]}

Modify Symmetry [id] [name <’name’>] [{Add|Remove {Surface} <entity_list>]}

7.3.3 Using Constraints

Constraints couple the motion of a set of nodes to the motion of a reference node. Rigid bodies and kinematic constraints do exactly this for blocks and sidesets, respectively. A distributing constraint allows users to average the constrained motion of a sideset by using weight factors to control force transmission (to be specified outside of CUBIT). A tie constraint can be used to tie the elements of one sideset to the elements of another. Currently, only the Abaqus Exporter supports this type of constraint. Note that as of CUBIT 13.0, constraints are supported by the Abaqus Importer/Exporter only. Contact the CUBIT support team if support in additional file formats is needed. To create a constraint

  1. On the Command Panel, click on FEA Bcs and then contraint.

  2. Click on the create action button.

  3. Enter the appropriate settings for ID/name.

  4. Select kinematic, distributing, rigid body or tie for Constraint Type.

  5. Enter the appropriate settings.

  6. Select apply.

Create Constraint {Kinematic|Distributing} [name ’<name>’] [vertex|node] <id> sideset <id>

Create Constraint Rigidbody [name ’<name>’] [vertex|node] <id> block <id>

Create Constraint Tie [name ’<name>’] master sideset <id> slave sideset <id>

A constraint’s name, dependent object, and independent object can be changed using the following commands: To modify a constraint

  1. On the Command Panel, click on FEA Bcs and then contraint.

  2. Click on the modify action button.

  3. Enter the appropriate settings for ID/name.

  4. Select kinematic, distributing, rigid body or tie for Constraint Type.

  5. Enter the appropriate settings.

  6. Select apply.

Modify Constraint <id|name> [name ’<name>’] [vertex|node] <id> sideset <id>

Modify Constraint <id|name> [name ’<name>’] [vertex|node] <id> block <id>

Constraints can be listed or deleted using the following commands:

List Constraint <id_range>

Delete Constraint <id_range>

7.3.4 Using Contact Surfaces
7.3.4.1 The Contact Region

To define contact between two entities, Cubit requires each entity to be defined as a separate contact region. Each region can be made up of multiple 1D or 2D entities. To create a contact region

  1. On the Command Panel, click on FEA Bcs and then contact region.

  2. Click on the create action button.

  3. Specify ID(s)/Name settings.

  4. Select the contact region entity and specify the entity ID(s). This can also be done using the pick widget function.

  5. Click apply.

Create Contact Region [id] [Name <’name’>] [{Add|On {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]}

To modify a contact region

  1. On the Command Panel, click on FEA Bcs and then contact region.

  2. Click on the modify action button.

  3. Specify ID(s)/Name and optionally change name.

  4. Select add entities or remove entities.

  5. Select the contact region entity and specify the entity ID(s). This can also be done using the pick widget function.

  6. Click apply.

Modify Contact Region {id_list|’name’|All [Name <’name’>] [{Add|Remove} {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]}

7.3.4.2 The Contact Pair

To create or modify a contact pair

  1. On the Command Panel, click on FEA Bcs and then contact pair.

  2. Click on create or modify.

  3. Enter the appropriate settings.

  4. Click apply.

create contact pair [id] [name <’name’>] [master contact region <id|’name’>] [slave contact region <id|’name’>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior <on|OFF>]]

modify contact pair {id_list|’name’|all} [name <’name’>] [master contact region <id|’name’>] [slave contact region <id|’name’>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior <on|OFF>]]

A contact pair is composed of two contact regions. One region will be the ’master’ surface, and the other will be the ’slave.’ 2D contact regions can not be mixed with 1D contact regions. The friction coefficient can also be included. The tolerance keyword is currently unused. Use the tied keyword to specify that the contact is to define tied contact between the two contact regions, essentially "gluing" the parts together. Currently, this option is only available when using the Abaqus Exporter. The general keyword can be used to specify general (i.e. global) contact without specifying surfaces/curves to use as contact pairs. Currently, this keyword is only valid when exporting to Abaqus. If the exterior keyword is used with the general keyword, then Abaqus will consider all exterior surfaces when determining contact regions. If the Exterior keyword is omitted, then the user must provide a master contact region and/or a slave contact region.

7.3.4.3 Auto-Contact Tool

With the auto-contact tool, Cubit can search for contact pairs and automatically set up all of the necessary contact regions and contact pairs.

Create Contact Autoselect [{Volume|Surface|Curve <ids>] [Master Volume <id>] [Maxgap <value>] [Curve_Contact]}

The optional geometry list can be used to limit Cubit’s search to only a subset of entities. If this list is omitted, all bodies in the model will be searched. The optional master volume keyword can be used to tell Cubit which volume should be used as the master contact region. If this keyword is omitted, the user will not have control over which volume is the master region. The maxgap keyword can be used to control how Cubit searches for contact regions. This value is used as the maximum amount of gap that can exist between two surfaces and be identified as a contact region. If this keyword is omitted, the geometry tolerance is used. The curve_contact keyword can be used to indicate the model requires curve contact as opposed to surface contact.

7.3.5 Cubit Initial Conditions

In Cubit, initial conditions can be applied to nodesets. Cubit supports the following types of initial conditions: displacement, velocity, acceleration, temperature, and generic field. For now, initial conditions are only supported by Cubit’ Abaqus exporter. The commands to create an initial condition are:

Create initialcondition [id] type temperature [name <’name’>] [{add|on} nodeset <entity_list>] [value <val>]

Create initialcondition [id] type displacement [name <’name’>] [{add|on} nodeset <entity_list>] [dof {1|2|3|4|5|6} {value <value>|off}]

Create initialcondition [id] type velocity [name <’name’>] [{add|on} nodeset <entity_list>] [dof {1|2|3|4|5|6} {value <value>|off}]

Create initialcondition [id] type acceleration [name <’name’>] [{add|on} nodeset <entity_list>] [dof {1|2|3|4|5|6} {value <value>|off}]

Create initialcondition [id] type field [name <’name’>] [{add|on} nodeset <entity_list>] [variable <n> value <val>

For most of the initial conditions, only two pieces of data are required: a list of nodesets this IC is applied to, and an initial value. Optionally, a name can be specified for the initial condition. To modify an initial condition, replace the word "create" with the word "modify." If modifying an IC, the IC’s ID must be passed in so Cubit knows which IC you are modifying. Example:

Modify initialcondition 3 value 1.23

Use this command to list the information about a set of initial conditions:

List initialcondition <id_list>

Use this command to delete a set of initial conditions:

Delete initialcondition <id_list>

7.3.6 Using Loads
7.3.6.1 Forces

To create a force

  1. On the Command Panel, click on FEA Bcs and then force.

  2. Click on the create action button.

  3. Specify the ID/name,force entity and entity ID(s).

  4. Select or Deselect specify using vector and enter the appropriate settings.

  5. Click apply.

Create Force [id] [Name <’name’>] [ {Add|On {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [Force Value <val>] [Moment Value <val>] [Direction { direction_options}]}

Create Force [id] [Name <’name’>] [ {Add|On {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [ Vector <val> <val> <val> <val> <val> <val>]}

To modify a force

  1. On the Command Panel, click on FEA Bcs and then force.

  2. Click on the create action button.

  3. Specify the ID/name,force entity and entity ID(s).

  4. Select or Deselect specify using vector and enter the appropriate settings.

  5. Click apply.

Modify Force {id_list|’name’|all [Name <’name’>] [ {Add|Remove} {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [Force Value <val>] [Moment Value <val>] [Direction { direction_options}]}

Modify Force {id_list|’name’|all [Name <’name’>] [ {Add|Remove} {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [ Vector <val> <val> <val> <val> <val> <val>]}

A Cubit user has the ability to create forces on 0D, 1D, and 2D entities. A force can be created using the direction syntax (see Specifying Direction). If the vector keyword is used, the first three values are the force components, and the last three values are the moment components. The use of the force and moment keywords specify the type of load. If both a force and a moment are to be applied, first create one of them, then modify it to add the other. Note that every instance of a force or moment keyword must have an accompanying value keyword.

Regarding force and moment keywords, the following detail may be helpful: A user may create a force and moment at the same time, but can only specify a direction once. If the force and moment have the same unit vector, it will be successful. If a users wants to create a force in the direction 1,2,3 and a moment in the direction 1,0,0, the user will have to create one, then add the other by modifying it.

7.3.6.2 Using Pressure

To create or modify a pressure

  1. On the Command Panel, click on FEA Bcs and then pressure.

  2. Click on the create or modify action button.

  3. Specify the ID/name,force entity, entity ID(s) and magnitude value.

  4. Enter any other appropriate settings.

  5. Click apply.

Create Pressure [id] [Name <’name’>] [{Add|On {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Magnitude <value>] [TOP|Bottom] [PRESSURE|Totalforce]}

Modify Pressure {id_list|’name’|all [Name <’name’>] [{Add|Remove} {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Magnitude <value>] [TOP|Bottom] [PRESSURE|Totalforce]}

Cubit users can create pressure boundary conditions on 1D and 2D entities. Positive surface pressures acting on solid elements are defined as pointing into the face of the elements. Pressures are always normal to the face. For shells and independent surfaces, a ’left-hand-rule’ is employed. Point your left thumb at the surface in question. If the direction your fingers curl matches the direction of ascending vertex numbering, the direction of the pressure vectors will match the direction of your thumb.

7.3.6.2.1 Value

The value variable is the magnitude of the pressure boundary condition. If the user leaves this value blank, Cubit will assign the pressure magnitude to zero (possibly a trivial case) and issue a warning. Typing a negative value will not flip the direction of the pressure arrows on the display; instead, the pressure magnitude will be negative.

7.3.6.2.2 Pressure and Total Force

The pressure and totalforce keywords are used to modify the pressure boundary condition. The pressure keyword is the default. All pressures applied with this keyword present (or with both of these keywords absent from the command string) are pure pressures. If the user enters the totalforce keyword, the pressure magnitude is divided by the area of the surface the pressure is acting on (or the length of the curve, for a curve pressure). In effect, the user is entering a force that is treated and exported as a pressure.

7.3.6.2.3 Top and Bottom

The top keyword (default) indicates the pressure will occur on the top of a shell element. Specifying bottom will cause the pressure to be applied to the bottom of the element.

7.3.6.3 Using Heat Flux

To create or modify a heatflux

  1. On the Command Panel, click on FEA Bcs and then heatflux.

  2. Click on the create or modify action button.

  3. Specify ID/name, entity list and entity ID(s).

  4. Enter any other appropriate settings.

  5. Click apply.

Create Heatflux [id] [Name <’name’>] [{Add|On {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Value <value>]}

Create Heatflux [id] [Name <’name’>] [{Add|On {Sideset|Surface|Face|Tri} <entity_list>] [Top <value> Bottom <value>]}

Modify Heatflux {id_list|’name’|All [Name <’name’>] [{Add|Remove} {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Value <value>]}

Modify Heatflux {id_list|’name’|All [Name <’name’>] [{Add|Remove} {Sideset|Surface|Face|Tri} <entity_list>] [Top <value> Bottom <value>]}

A Cubit user may apply heat flux boundary conditions to 1D and 2D entities, including thin-shell elements.

7.3.6.3.1 Top and Bottom Values

Heat fluxes can be applied to thin-shell elements as well. The same rules apply to thin-shell heat fluxes as to thin-shell temperatures: thin-shell heat fluxes can only be applied to surfaces and heat flux boundary conditions cannot contain regular and thin-shell heat flux values (see journal below). However, thin-shell heat flux commands do not contain gradient or middle keyword options. Only top and bottom keywords are supported.

7.3.6.4 Using Convection

To create or modify a convection

  1. On the Command Panel, click on FEA Bcs and then convection.

  2. Click on the create or modify action button.

  3. Specify ID/name, entity list and entity ID(s).

  4. Enter any other appropriate settings.

  5. Click apply.

Create Convection [id] [Name <’name’>] [{Add|On {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Surrounding {<value>| Top <value> Bottom <value>} Coefficient {<value>| Top <value> Bottom <value>}]}

Modify Convection [id] [Name <’name’>] [{Add|On {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Surrounding {<value>| Top <value> Bottom <value>} Coefficient {<value>| Top <value> Bottom <value>}]}

A Cubit user can apply convection boundary conditions to 1D and 2D entities. Convection is a transport of thermal energy that is proportional to the difference between the surface temperature and the temperature of the surroundings.

7.3.6.4.1 Surrounding

The surrounding keyword specifies the temperature surrounding the entity with the convection boundary condition.

7.3.6.4.2 Coefficient

The coefficient keyword is a convection coefficient, in units of energy per length times time times temperature (i.e., [energy]/([length]*[time]*[temperature]) ).

7.3.7 Miscellaneous Boundary Condition Commands
7.3.7.1 Delete

The BC delete keyword combination is used to delete boundary conditions. The current list of all entities that can be deleted using this command were shown in Table 1. Cubit currently has no ’undo’ command to ’undelete’ a boundary condition deletion. To delete a boundary condition

  1. On the Command Panel, click on FEA Bcs or CFD Bcs.

  2. Click on any option from the Entity menu.

  3. Click on the delete action button.

  4. Enter the appropriate settings.

  5. Click apply.

delete {bc_type} [<id-range>|All]

delete boundary conditions

Every set (and boundary condition within them) can be deleted at once by typing delete boundary conditions. This command will delete all boundary conditions from your model.

7.3.7.2 List

The list keyword combination is used to list boundary conditions. The current list of all entities that can be listed using this command was shown in Table 1. Cubit’s parser can evaluate boundary conditions given the entities they act on. For example, "List pressure in surface 1" will list all pressures that act on Surface 1. To list boundary conditions

  1. On the Command Panel, click on FEA Bcs or CFD Bcs.

  2. Click on any option from the Entity menu except Contact Pair and Set.

  3. Click on the list action button.

  4. Enter the appropriate settings.

  5. Click apply.

list {bc_type} [<id-range>]

list boundary conditions

Every set (and boundary condition within them) may be listed at once by typing list boundary conditions. Cubit will list the number of sets and individual boundary conditions in your model. This command will list the total number of each type of set and boundary condition, including boundary conditions that are not a part of a BC set.

7.3.7.3 Draw

To draw boundary conditions

  1. On the Command Panel, click on FEA Bcs or CFD Bcs.

  2. Click on any option from the Entity menu except Contact Pair and Set.

  3. Click on the draw action button.

  4. Select draw.

  5. Enter the appropriate settings.

  6. Click apply.

draw {bc_type} {<id-range>|all}[Add]

The draw keyphrase allows a Cubit user to draw any type of boundary condition. This command will clear the graphics window of every part of the model except for the selected boundary condition. Using the add keyword will permit multiple boundary conditions to be drawn at the same time. Any combination of boundary conditions and entities that were valid for delete and list are also valid for draw.

7.3.7.4 Highlight

To Highlight boundary conditions

  1. On the Command Panel, click on FEA Bcs or CFD Bcs.

  2. Click on any option from the Entity menu except Contact Pair and Set.

  3. Click on the draw action button.

  4. Select highlight.

  5. Enter the appropriate settings.

  6. Click apply.

Highlight {bc_type {<id-range>|All}}

The highlight keyphrase allows a Cubit user to highlight any boundary condition. Highlighting a boundary condition will turn it bright orange and the vectors defining it will thicken. The highlight command is similar to the draw command.

7.3.8 Using Restraints
7.3.8.1 Displacements/Accelerations/Velocities

A Cubit user has the ability to create displacement boundary conditions on most geometric entities found within Cubit. To create a displacement

Create Displacement [id] [Name <’name’>] [{Add|On {Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}} Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]}

To modify a displacement

Modify Displacement {id_list|’name’|all [name <’name’>] [{Add|Remove} {Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}} {Fix <value>|Free}] [SmallestCombine|Average|LargestCombine|OVERWRITE]}

To create an acceleration

Create Acceleration [id] [Name <’name’>] [{Add|On {Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}} Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]}

To modify an acceleration

Modify Acceleration {id_list|’name’|all [name <’name’>] [{Add|Remove} {Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}} {Fix <value>|Free}] [SmallestCombine|Average|LargestCombine|OVERWRITE]}

To create a velocity

Create Velocity [id] [Name <’name’>] [{Add|On {Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}} Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]}

To modify a velocity

modify velocity {id_list|’name’|all [name <’name’>] [{add|remove} {nodeset|volume|surface|curve|vertex|hex|tet|face|tri|edge|node} <entity_list>] [dof {all|{[1][2][3][4][5][6]}} {fix <value>|free}] [smallestcombine|average|largestcombine|overwrite]}

A number of required and optional keywords make the BC create displacement command one of the more complicated of the boundary condition commands. These keywords will be examined individually in detail.

Degrees of Freedom The dof keyword is the heart of this command. It specifies how to constrain the entity in question. The keyword is an abbreviation for “degree of freedom”. Typing the optional keyword all tells Cubit that the entered command will encompass all six degrees of freedom. The degrees of freedom (1 - 6) are defined below.

Cubit definitions of the six degrees of freedom.

DOF

   

Physical analog

1

   

x-translation

2

   

y-translation

3

   

z-translation

4

   

x-rotation

5

   

y-rotation

6

   

z-rotation

Cubit will allow displacement commands to be applied upon between one and all six of the degrees of freedom. The degrees of freedom do not need to be entered in any order. The command strings “1 2 3 4 5 6” “2 6 1 4 3 5” and “all” will end with the same result.

7.3.8.1.1 Fixed or Free

The fix and free keywords tell Cubit whether an entity’s displacement defined by the dof keyword is to be enforced with a finite value or not. If the displacement is fixed, the entity will be constrained in the pre-specified degrees of freedom. A decimal number entered after the fix keyword will be the value of the enforced degree(s) of freedom. Cubit allows the user to leave this value blank if the enforced displacement is to be zero, for convenience. However, entering 0 is still permitted. If a user wishes to remove a displacement from an entity, he or she should just delete it rather than trying to set all of the degrees of freedom to free.

7.3.8.1.2 Displacement Combinations

The smallestcombine, average and largestcombine keywords deal with displacement combinations. These keywords only apply when a user is modifying an existing displacement boundary condition.

The smallestcombine keyword will compare the existing displacement values with the current (residing on the command line) displacement values. The keyword will modify the displacement to the match the displacements dictated by the boundary condition that has the smallest absolute value. If the boundary condition with the smallest absolute value is the existing value, the displacement boundary condition will be unchanged. If the current boundary condition has a smaller absolute value than the existing displacement, the displacement boundary condition will be changed to incorporate the new values.

The average keyword will average the existing displacement values with the current (residing on the command line) displacement values. Note that these averages are not continually updated (i.e., they are not weighted). If a user created a displacement boundary condition and constrained a degree of freedom to 10.0 and then constrained the same degree of freedom to 20.0 with the Average keyword, the new displacement value would be 15.0. But if a user constrained the same degree of freedom to 30.0, while using the Average keyword, the new displacement value would be 22.5 ([15+30]/2), not 20.0 ([10+20+30]/3).

The largestcombine keyword will compare the existing displacement values with the current (residing on the command line) displacement values. The keyword will modify the displacement to the match the displacements dictated by the boundary condition that has the largest absolute value. If the boundary condition with the largest absolute value is the existing value, the displacement boundary condition will be unchanged. If the current boundary condition has a larger absolute value than the existing displacement, the displacement boundary condition will be changed to incorporate the new values.

When none of these keywords are specified, Cubit will combine displacements in its default mode, Overwrite. The Overwrite keyword overwrites the entity’s previous displacement boundary condition(s) with the displacement values specified in the command.

7.3.8.2 Temperature

Cubit can create temperature boundary conditions on most geometric and mesh entities. The temperature boundary condition can also be applied to thin-shell elements.

To create a temperature

create temperature [id] [name <’name’>] [{add|on {nodeset|volume|surface|curve|vertex|hex|tet|face|tri|edge|node} <entity_list>] [value <val>]}

create temperature [id] [name <’name’>] [{add|on {nodeset|volume|surface|curve|vertex|hex|tet|face|tri|edge|node} <entity_list>] [{ top <val> bottom <val> | [middle <val>] [gradient <val>] } ]}

To modify a temperature

modify temperature {id_list|’name’|all [name <’name’>] [{add|remove} {nodeset|volume|surface|curve|vertex|hex|tet|face|tri|edge|node} <entity_list>] [value <val>]}

modify temperature {id_list|’name’|all [name <’name’>] [{add|remove} {nodeset|volume|surface|curve|vertex|hex|tet|face|tri|edge|node} <entity_list>] [{ top <val> bottom <val> | [middle <val>] [gradient <val>] } ]}

The value keyword defines the amplitude (temperature). The other command options are discussed below

7.3.8.2.1 Top, Gradient, Middle, Bottom

The above keywords are only used for thin-shell elements (i.e., 2D entities). The valid combinations are limited to: top and bottom, middle and gradient, only gradient or only middle. It should be noted that temperature boundary conditions cannot contain regular and thin-shell temperature values.

7.3.9 Boundary Condition Sets

To create boundary condition sets

  1. On the Command Panel, click on FEA Bcs and then set.

  2. Click on the create action button.

  3. Specify the settings for ID/name.

  4. Enter in the appropriate settings.

  5. Optionally select specify analysis type and/or specify modal max frequency and enter the appropriate settings.

  6. Click apply.

Create bcset [id] [name <’name’>] [After bcset <id>] [{Add|Remove} {bc_type} <id-range | <with name ’name’> >] [analysistype {STATIC|heat|dynamic|modal}] [modal_max_frequency <value>]

To modify boundary condition sets

  1. On the Command Panel, click on FEA Bcs and then set.

  2. Click on the modify action button.

  3. Enter in the appropriate settings.

  4. Optionally select specify analysis type and enter the appropriate settings.

  5. Click apply.

Modify bcset {id_list|’name’|all} [name <’name’>] [After bcset <id>] [{Add|Remove} {bc_type} <id-range | <with name ’name’> >] [analysistype {STATIC|heat|dynamic|modal}]

7.3.9.1 *** ABAQUS Parameters ***

Modify bcset {id_list|’name’|all} [max_step_increments <value>] [nonlinear_geometry <on|OFF>][perturbation <on|OFF>][stabilize <on|OFF>] [steadystate <on|OFF>][modal_max_frequency <value>]

Modify bcset {id_list|’name’|all} [initial_step_size <value>] [step_period <value>][min_step_size <value>] [max_step_size <value>][min_step_temperature_change <value>]

Modify bcset {id_list|’name’|all} [mass_scaling <on|OFF>] [mass_scaling_dt <value>][mass_scaling_factor <value>] [mass_scaling_type <’uniform’|’BELOW_MIN’|’set_equal_dt’>]

Modify bcset {id_list|’name’|all} [restart <on|OFF>][restart_overlay <on|OFF>] [{restart_frequency|restart_num_intervals} <value>]

Modify bcset {id_list|’name’|all} [output_field <on|OFF>] [output_field_frequency <value>] [output_history <on|OFF>] [output_history_frequency <value>]

Modify bcset {id_list|’name’|all} [el_file <on|OFF>][el_file_frequency <value>] [node_file <on|OFF>][node_file_frequency <value>]

Modify bcset {id_list|’name’|all} [el_print <on|OFF>][el_print_frequency <value>] [node_print <on|OFF>][node_print_frequency <value>]

7.3.9.2 *** NASTRAN Parameters ***

Modify bcset {id_list|’name’|all} {displacement_output <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> }}

Modify bcset {id_list|’name’|all} {oload <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> }}

Modify bcset {id_list|’name’|all} {mpcforces <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> }}

Modify bcset {id_list|’name’|all} {spcforces <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> }}

Modify bcset {id_list|’name’|all} {stress <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> } {CENTER|cubic|sgage|corner} {VONMISES|maxs}}

Modify bcset {id_list|’name’|all} {element_strain_energy <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>> } {AVERAGE|amplitude|peak}}

Cubit can create BC sets, which is a group of previously defined loads, restraints and contact pairs. A BCSet is used to define a load case (analysis step) when writing out 3rd party analysis decks. A BCSet can be a static analysis set, a thermal analysis set, a modal analysis set, or a dynamic analysis set by specifying the analysistype. The after keyword can be used to define the order that the BCSets will be written when the model is exported. Several solver-specific parameters can be set for a BCSet. For ABAQUS, parameters associated with *STEP, *STATIC, *DYNAMIC, *FREQUENCY, *HEAT TRANSFER, *MASS SCALING, *RESTART, *OUTPUT, *EL FILE, *NODE FILE, *EL PRINT, and *NODE PRINT can be modified. For Nastran, output requests can be defined for Displacement, Reaction Loads, MPC Forces, SPC Forces, Stress, and Element Strain Energy.