Loads and Boundary Conditions

Marc > Building A Model > Loads and Boundary Conditions - Contact

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Loads and Boundary Conditions - Contact

The Loads and Boundary Conditions application controls which loads and boundaries and contact information will be created in the Marc input file. For more information, see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual.

The following table lists the supported loads and boundary condition types:


Object	Analysis Type	Type	Element Dimension
• Acceleration	• Structural, Coupled	Nodal
• Displacement	• Structural, Coupled	Nodal
• Release	• Structural, Coupled	Nodal
• Force	• Structural, Coupled	Nodal
• Pressure	• Structural, Coupled	• Element Uniform • Element Variable	• 2D 3D • 2D 3D
• 1D Pressure	• Structural, Coupled	Element Uniform	• 1D
• Temperature	• Structural, Thermal, Coupled	• Nodal • Element Uniform • Element Variable	• 1D 2D 3D • 2D
• Inertial Load	• Structural, Coupled	Element Uniform	• 1D 2D 3D
• Initial Displacement	• Structural, Coupled	Nodal
• Initial Velocity	• Structural, Coupled	Nodal
• Initial Temperature	• Structural, Thermal, Coupled	• Nodal • Element Variable	• 2D
• CID Distributed Load	• Structural, Coupled	Element Uniform	1D 2D 3D
• Contact	• Structural, Thermal, Coupled	Element Uniform	1D 2D 3D
• Convection	• Thermal, Coupled	• Element Uniform • Element Variable	• 2D 3D • 2D 3D
• Heat Flux	• Thermal, Coupled	• Element Uniform • Element Variable	• 2D 3D • 2D 3D
• Volumetric Flux	• Thermal, Coupled	Element Uniform	• 1D 2D 3D
• Heat Source	• Thermal, Coupled	• Nodal • Element Uniform • Element Variable	• 2D 3D • 2D
• Radiation	• Thermal, Coupled	Element Uniform	• 2D 3D
• Convective Velocity	• Thermal, Coupled	Nodal
• Potential	• Coupled	• Nodal • Element Variable	• 2D
• Charge	• Coupled	• Nodal • Element Uniform • Element Variable	• 2D 3D • 2D
• Voltage	• Coupled	Nodal
• Current	• Coupled	• Nodal • Element Uniform • Element Variable	• 2D 3D • 2D
• Magnetization	• Coupled	• Element Uniform

Loads and boundary conditions can be placed directly on geometric or finite element entities. In both cases the loads and boundary conditions are written to the Marc input file and associated with finite element entities, either nodes or elements. Geometric entities in Patran are evaluated to determine the associated finite element entities. However, in Marc 2003 and greater, geometric entities can be written to the input file and the loads and boundary conditions associated directly to them. This is advantageous for adaptive remeshing. See Loads on Geometry for more details.


Note:	The load magnitudes specified for any of the above load types should always be given as total loads for any given step or load case. The Marc Preference always writes loads to the Marc input file as total loads (not incremental loads) by using the parameter FOLLOW FOR,,1 in the input file. This has nothing to do with follower forces even though the flag is on this parameter. If the Use Tables toggle is ON, then this parameter is NOT written to specify total loads as total loads are assumed in this case.

Static Load Case Input

This subordinate form appears when the Input Data button is selected and Static is the load case type. The load case type is set under the Load Cases application. See Load Cases. The information contained on this form will vary according to the selected Object. However, defined below is information that remains standard to this form.


Note:	It is not advisable to mix both static and time dependent load cases together in a single analysis. Use either all static or all time dependent loading.

Time Dependent Load Case Input

This subordinate form appears when the Input Data button is selected in the Loads and Boundary Conditions application and the load case is Time Dependent. The load case type is set under the Load Cases application. See Load Cases. The information contained on this form will vary according to the selected Object. However, defined below is information that remains standard to this form.

Object Tables

On the Static and Transient Input Data forms, these are areas where the load data values are defined. The data fields presented depend on the selected Object and Type. In some cases, the data fields also depend on the selected target element type. These object tables list and define the various input data which pertain to a specific selected object.


Note:	The Analysis Type set on the Loads and BCs application form will determine which Objects are available to you. You can switch between Analysis Types without affecting any analysis setup or recognition of already defined LBCs.

Acceleration

This input data creates the FIXED ACCE and the ACC CHANGE keyword options. All non-blank entries will generate prescribed accelerations with the FIXED ACCE option. Time dependent fields create multiple ACC CHANGE options. Currently the TABLE parameter and option in conjunction with a LOADCASE option for Marc 2003 or greater is not supported with the LBC.


Input Data	Type	Analysis	Description
Translations (A1,A2,A3)	Nodal	Structural Coupled	Defines the prescribed translational acceleration vector. Components of the vector are entered in model length units.
Rotations (R1,R2,R3)	Nodal	Structural Coupled	Defines the prescribed rotational acceleration vector.


Caution:	Read caution notes for Displacements below

Displacement

This input data creates the FIXED DISP and the DISP CHANGE keyword options. All non-blank entries will generate prescribed displacements with the FIXED DISP option. Time dependent fields create multiple DISP CHANGE options, or a TABLE parameter and option in conjunction with a LOADCASE option for Marc 2003 or greater.


Input Data	Type	Analysis	Description
Translations (T1,T2,T3)	Nodal	Structural Coupled	Defines the prescribed translational displacement vector. Components of the vector are entered in model length units. This vector is not transformed. The analysis coordinate frames of the nodes in the application region are changed to the analysis coordinate frame specified on this form.
Rotations (R1,R2,R3)	Nodal	Structural Coupled	Defines the prescribed rotational displacement vector. Components of the vector are entered in radians. This vector is not transformed. The analysis coordinate frames of the nodes in the application region are changed to the analysis coordinate frame specified on this form.
Use Sub. FORCDT	Nodal	Structural Coupled	If this toggle is ON, the FORCDT option is written. The list of nodes supplied in the 2nd data block of this option comes from the application regions list of nodes or associated nodes. For displacements, the FIXED DISP keyword is still written but with zero magnitudes for the specified degrees-of-freedom.


Caution:	Patran always assumes there are six (6) degrees-of-freedom per node regardless of the element type. You must be cognizant of the actual degrees-of-freedom valid for a particular Marc element you want to use. For example, an axisymmetric shell (1D element) has only three valid degrees-of-freedom (axial (Z), radial (R) and rotational) but in Patran these would map to degrees-of-freedom 1, 2, and 4 (T1, T2, and R1 respectively). Elements 49 and 72 have midside nodes with only a single rotational dof, which would be considered the 4th (R1) dof in Patran.

Release

This input data creates the RELEASE NODE keyword option. All non-blank entries will generate prescribed releases of previously prescribed displacements specified using the FIXED DISP option in a previous Load Step. Time dependent fields are not applicable. Release will also be ignored if included in a loadcase associated to the first Load Step. Only subsequent Load Steps can release node constraints. This option is not available when using the TABLE parameter (Use Tables is ON in the Job Parameters form) and option in conjunction with a LOADCASE option for Marc 2003 or greater. RELEASE NODE will not be written in this case. Instead, any releases should be done using the Select Load Case selection form.


Input Data	Type	Analysis	Description
Translations (T1,T2,T3)	Nodal	Structural Coupled	Defines the prescribed translational displacement vector that should be released. Any non-null value entered here will be used to indicate that that translational degree-of-freedom is to be released.
Rotations (R1,R2,R3)	Nodal	Structural Coupled	Defines the prescribed rotational displacement vector that should be released. Any non-null value entered here will be used to indicate that that rotational degree-of-freedom is to be released.


Caution:	The same caution as that for Displacement is applicable for Release also.

Force

This input data creates the POINT LOAD keyword option. Multiple POINT LOAD options are generated for the time dependent fields, or a TABLE parameter and option in conjunction with a LOADCASE option for Marc 2003 or greater.


Input Data	Type	Analysis	Description
Force (F1,F2,F3)	Nodal	Structural Coupled	Defines the applied translational force vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the POINT LOAD option.
Moment (M1,M2,M3)	Nodal	Structural Coupled	Defines the applied rotational force vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the POINT LOAD option.
Use Sub. FORCDT	Nodal	Structural Coupled	If this toggle is ON, the FORCDT option is written. The list of nodes supplied in the 2nd data block of this option comes from the application regions list of nodes or associated nodes. In this case, no POINT LOAD options are written, only the FORCDT option in the Model Definition section.


Caution:	Elements 49 and 72 have midside nodes with only a single rotational dof, which would be considered the 4th (M1) dof in Patran.

Pressure

This input data creates the DIST LOADS keyword option. Multiple DIST LOADS options are generated for the time dependent fields, or a TABLE parameter and option in conjunction with a LOADCASE option for Marc 2003 or greater. An exception to this is when the Element Variable type is chosen as described in the table below


Input Data	Type	Analysis	Description
Top Surface Pressure	Element Uniform	Structural/2D Coupled/2D	Defines the top surface pressure on shell and/or plate elements which is directed inward when positive. The IBODY data field of the DIST LOADS option is set to two.
Bot Surface Pressure	Element Uniform	Structural/2D Coupled/2D	Defines the bottom surface pressure on shell and/or plate elements which is directed inward when positive. This value is subtracted from the element’s top surface pressure and the difference is entered in the DIST LOADS option.
Edge Pressure	Element Uniform	Structural/2D Coupled/2D	Defines the edge pressure on 2D solid elements which is directed inward when positive. The IBODY data field of the DIST LOADS option varies based on the element edges chosen in the application region. Top and/or bottom surface pressures cannot be used in the same application region as edge pressure.
Pressure	Element Uniform / Variable	Structural/3D Coupled/3D	Defines the face pressure on solid elements which is directed inward when positive. The IBODY data field of the DIST LOADS option varies based on the element faces chosen in the application region.
Top, Bottom Surface or Edge Pressure or Pressure	Element Variable	Structural/2D Coupled/2D	This is used for superplastic forming. Putting a value in for Top or Bottom simply specifies the direction. The IBODY data field of the DIST LOADS option is set to the appropriate value for nonuniform loading in the normal direction for the given element type. The magnitude that you specify is arbitrary and should be used for visualization purposes only. The value written to the DIST LOADS option is zero.
Use Sub. FORCEM	Element Variable	Structural Coupled	If this toggle is ON, the FORCEM user subroutine is used by placing the appropriate nonuniform IBODY code in field 1 of the 3rd data block of the DIST LOADS option. The magnitude of the pressure will be written but may be ignored as the definition of the pressure load is the function of the FORCEM routine.


Note:	If the Use Sub. toggle is ON, it will flag the use of the user subroutine unless a superplastic forming analysis is detected, in which case it will be ignored.

Temperature / Temp (Thermal)

This input data creates the CHANGE STATE keyword option for element uniform conditions or the POINT TEMP for nodal conditions. Multiple CHANGE STATE or POINT TEMP options are generated for time dependent fields. Or this creates the FIXED TEMPERATURE and the TEMP CHANGE keyword options for thermal analysis.


Input Data	Type	Analysis	Description
Temperature	Element Uniform	Structural/1D Coupled/1D	Defines the temperature state variable for the axisymmetric shell, beam and truss elements. (INITIAL STATE / CHANGE STATE)
Temperature	Element Uniform	Structural/2D Coupled/2D	Defines the temperature state variable for the shell, plate, and 2D solid elements. (INITIAL STATE / CHANGE STATE)
Temperature	Element Uniform	Structural/3D Coupled/3D	Defines the temperature state variables for the solid elements. (INITIAL STATE / CHANGE STATE)
Temperature	Nodal	Structural	Defines the point temperature (POINT TEMP) values for nodes. The stress-free temperature value may be entered by using the Initial Temperature option. You may not define a reference temperature (in Material properties) if POINT TEMPs are defined.
Temperature	Nodal	Thermal Coupled	Defines the prescribed temperature value. Multiple TEMP CHANGE option are generated for the time dependent fields, or in Marc 2003 or greater, the TABLE and LOADCASE options are used instead. Note that a blank appication region will release all temperatures is subsequent Load Steps.
Top Bottom Middle Temperature	Element Variable	Thermal Coupled	Same as above except allows for definition of temperature for the various degrees of freedom in shell elements in 3D analysis.
Use Subs. INITSV/NEWSV	Element Uniform	Structural	If this toggle is ON, the INITSV/NEWSV routines are flagged by placing a 2 in the 2nd field of the 2nd data block of the INITIAL STATE and CHANGE STATE keywords. Data blocks 3 and 4 are then not used.
Use Sub. FORCDT	Nodal	Thermal Coupled	If this toggle is ON, the FORCDT option is written. The list of nodes supplied in the 2nd data block of this option comes from the application regions list of nodes or associated nodes. For temperatures, the FIXED TEMPERATURE keyword is still written.

Inertial Load

This input data creates the DIST LOADS and ROTATION A keyword option. Multiple DIST LOADS options are generated for the time dependent fields, or TABLE and LOADCASE options are used for Marc 2003 or greater. ROTATION A is written only if present in first Load Step for non-Table format.


Input Data	Type	Analysis	Description
Translational Acceleration (A1,A2,A3)	Element Uniform	Structural Coupled	Defines the gravitational acceleration vector with respect to the specified analysis coordinate frame. This vector is transformed into the global coordinate frame before it is written to the third card of the DIST LOADS option. The load type (field 1) on the same card is set to 102.
Rotational Velocity (w1,w2,w3)	Element Uniform	Structural Coupled	Defines the angular velocity vector in radians per unit of time in the analysis coordinate frame for centrifugal loading. The magnitude of this vector is squared and entered on the third card of the DIST LOADS option. The load type (field 1) on the same card is set to 100. The direction of the angular velocity vector and the origin of the analysis coordinate frame are respectively entered as the direction of and point along the rotation axis on the second card of the ROTATION A option.
Rotational Acceleration (a1,a2,a3)	Element Uniform	Structural Coupled	Not supported.

Initial Displacement

This input data creates the INITIAL DISP keyword option. Time dependent fields are ignored.


Input Data	Type	Analysis	Description
Translations (T1,T2,T3)	Nodal	Structural Coupled	Defines the initial translational displacement vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the INITIAL DISP option.
Rotations (R1,R2,R3)	Nodal	Structural Coupled	Defines the initial rotational displacement vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the INITIAL DISP option.
Use Sub. USINC	Nodal	Structural Coupled	If this toggle is ON, the use of the USINC routine is flagged by placing a -1 in the 1st field of the 2nd data block of the INITIAL DISP option. Data blocks 3/4 are not required if this is the case.

Initial Velocity

This input data creates the INITIAL VEL keyword option. Time dependent fields are ignored.


Input Data	Type	Analysis	Description
Translational Velocity (v1,v2,v3)	Nodal	Structural Coupled	Defines the initial translational velocity vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the INITIAL VEL option.
Rotational Velocity (w1,w2,w3)	Nodal	Structural Coupled	Defines the initial rotational velocity vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the third card of the INITIAL VEL option.
Use Sub. USINC	Nodal	Structural Coupled	If this toggle is ON, the use of the USINC routine is flagged by placing a -1 in the 1st field of the 2nd data block of the INITIAL VEL option. Data blocks 3/4 are not required if this is the case.

1D Pressure

This input data creates the DIST LOADS keyword option. Multiple DIST LOADS options are generated for the time dependent fields, or the TABLE and LOADCASE options are used for Marc 2003 or greater.


Input Data	Type	Analysis	Description
Pressure	Element Uniform	Structural / 1D Coupled / 1D	Defines pressure loading on 1D planar and axisymmetric shell elements using the DIST LOADS option.
			Element Types	1, 15, 89, 90 (axisymmetric shell) 5, 16, 45 (planar beam) IBODY = 0: Uniform in XY plane.


Note:	If the curves or elements on which this 1D (planar) Pressure is applied are not in the XY plane, an error will be issued. In order for the program to determine this, the orientation system must be supplied in the Element Properties application for the given entities. The element property must exist before the load is allowed.

CID Distributed Load

This input data creates the DIST LOADS or equivalent POINT LOAD keyword option. Multiple options are generated for the time dependent fields, or the TABLE and LOADCASE options are used for Marc 2003 or greater.


Input Data	Type	Analysis	Description
Distributed Force (F1,F2,F3)	Element Uniform	Structural / 1D Coupled / 1D	Defines the applied translational distributed force vector with respect to the specified analysis coordinate frame. In general this provides the magnitudes (for each component) of the uniform load per unit length for 1D elements on the DIST LOADS option. a) Types 15, 16, 45, 89, 90: IBODY = 1: Uniform in X. IBODY = 2: Uniform in Y. b) Types 9, 13, 14, 25, 52, 64, 76, 77, 78, 79, 98: IBODY = 0 or 1: Uniform in X. IBODY = 1 or 2: Uniform in Y. IBODY = 2 or 3: Uniform in Z.
Distributed Force (F1,F2,F3)	Element Uniform	Structural Coupled 1D/2D/3D	These types of loads are converted to equivalent POINT LOAD options along the line of application depending on the element type to which they are applied for 2D and 3D elements.

Patran converts the distributed loads to equivalent POINT LOADs distributed to the nodes of the geometric selection in the input file. This is accomplished in the following manner:

Let q(x) be the distributed load applied between x0 and xf. The resultant force Q is given as

The centroid xc of the distributed load between x0 and xf is given as

where M is the magnitude of the net moment around x0 given by

Consider the problem where there are n element edges. Treating each of the n element edges as separate beam problems, each resultant force is calculated and the centroid along each edge. Then each element edge is treated as a static beam problem with the nodes acting as pinned supports on each beam end. Sum the loads from each beam solution at all nodes except the 0th and nth nodes since each node is shared by two element edges (beams). As an example:

Consider the problem of a uniform load q(x) of 200 pounds/inches applied along n element edges, each one inch long. Then Q=200 pounds, M = 100 inch pounds, and x0 = 0.5 inch for each element edge. The static solution for each element edge (as a beam) is 100 pounds applied on each end node. This gives the expected solution of 100 pounds applied at the end nodes and 200 pounds applied at all internal nodes.

Similar calculations are done for two dimensional cases.

Convection

This input data creates the FILMS keyword options. Multiple FILMS options are generated for the time dependent fields.


Input Data	Type	Analysis	Description
Top Surf Convection	Element Uniform/ Variable	Thermal/2D Coupled/2D	Defines the top surface film coefficient on shell elements. The entry in the IBODY data field is set to five on the third card of the FILMS option.
Bot Surf Convection	Element Uniform/ Variable	Thermal/2D Coupled/2D	Defines the bottom surface film coefficient on shell elements. The entry in the IBODY data field is set to six on the third card of the FILMS option.
Edge Convection	Element Uniform/ Variable	Thermal/2D Coupled/2D	Defines the edge film coefficient on 2D solid elements. The entry in the IBODY data field of the FILMS option varies based on the element edges chosen in the application region. Top and/or bottom surface convections cannot be used in the same application region as edge convection.
Convection	Element Uniform/ Variable	Thermal/3D Coupled/3D	Defines the film coefficient on faces of solid elements. The entry in the IBODY data field of the FILMS option varies based on the element faces chosen in the application region.
Ambient Temperature	Element Uniform/ Variable	Thermal/2D/3D Coupled/2D/3D	Defines the sink temperature for the shell or 2D solid and 3D elements. This produces an entry on the third card in the FILMS option.

Heat Flux / Volumetric Flux

This input data creates the DIST FLUXES keyword options.


Input Data	Type	Analysis	Description
Top Surface Heat Flux	Element Uniform	Thermal/2D	Defines the top surface heat flux on shell elements. The IBODY data field of the DIST FLUXES option is set to five.
Bot Surface Heat Flux	Element Uniform	Thermal/2D	Defines the bottom surface heat flux on shell elements. The IBODY data field of the DIST FLUXES option is set to six.
Edge Heat Flux	Element Uniform	Thermal/2D	Defines the edge heat flux on 2D solid elements. The entry in the IBODY data field of the DIST FLUXES option varies based on the element edges chosen in the application region. Top and/or bottom surface heat fluxes cannot be used in the same application region as an edge heat flux.
Heat Flux	Element Uniform	Thermal/3D	Defines the heat flux on faces of solid elements or entire elements in the case of Volumetric Flux. The entry in the IBODY data field of the DIST FLUXES option varies based on the element faces chosen in the application region.
Top/Bottom Surface/Edge Heat Flux	Element Variable	Coupled 2D/3D	When doing a Coupled analysis, Marc generates internal heat due to plastic work hardening that will effect the results. This is done by placing 101 (IBODY) in the 1st field of the 3rd data block of the DIST FLUXES option. Only the Element Variable Heat Flux LBC will request this. The magnitude is arbitrary and should be entered as zero, but will be ignored by the analysis if provided.
Use Sub. FLUX	Element Variable	Thermal Coupled	If this toggle is ON, the FLUX user subroutine is used by placing the appropriate nonuniform IBODY code in field 1 of the 3rd data block of the DIST FLUXES option. The magnitude of the load will be written but may be ignored as the definition of the pressure load is the function of the FLUX routine.

Heat Source

This input data creates the POINT FLUX keyword options.


Input Data	Type	Analysis	Description
Heat Source	Nodal	Thermal Coupled	Defines the applied nodal heat source. Multiple POINT FLUX options are generated for the time dependent fields.
Top Bottom Middle Heat Source	Element Variable	Thermal Coupled	Same as above except allows for heat source definition at the various degrees of freedom for shell elements in 3D analysis.
Use Sub. FORCDT	Nodal	Thermal Coupled	If this toggle is ON, the FORCDT option is written. The list of nodes supplied in the 2nd data block of this option comes from the application regions list of nodes or associated nodes. In this case, no POINT FLUX options are written, only the FORCDT option in the Model Definition section.

Initial Temperature

This input data creates the INITIAL TEMP keyword options.


Input Data	Type	Analysis	Description
Temperature	Nodal	Structural Thermal Coupled	Defines the initial nodal temperature. Time dependent fields are ignored.
Top Bottom Middle Temperature	Element Variable	Structural Thermal Coupled	Same as previous except allows for temperature definition at the various degrees of freedom for shell elements in 3D analysis.
Use Sub. USINC	Nodal	Structural Thermal Coupled	If this toggle is ON, the use of the USINC routine is flagged by placing a -1 in the 1st field of the 2nd data block of the INITIAL TEMP option. Data blocks 3/4 are not required if this is the case.

Radiation

This LBC type produces no options in the Marc input file. However, radiation LBCs must be present in order to do view factor calculations (see Radiation Viewfactors). Once a view factor calculation has been done and the view factor file has been created through this operation, a radiation analysis can be flagged by referencing this file and submitted. Only the VIEW FACTOR option is included in the input file with this operation.


Input Data	Type	Analysis	Description
Temp. at Infinity (top)	Element Uniform	Thermal/2D Coupled/2D	Used as input to the view factor file only. Generally used on 3D shell elements. This is the ambient temperature at infinity.
Temp. at Infinity (bottom)	Element Uniform	Thermal/2D Coupled/2D	Used as input to the view factor file only. Generally used on 3D shell elements. This is the ambient temperature at infinity. For shell elements, you can have two different ambient temperatures as seen from the top or bottom.
Temp. at Infinity (edge)	Element Uniform	Thermal/2D Coupled/2D	Used as input to the view factor file only. Generally used on 2D solid elements such as axisymmetric or plane strain. This is the ambient temperature at infinity.
Temp. at Infinity	Element Uniform	Thermal/3D Coupled/3D	Used as input to the view factor file only on 3D solid elements. This is the ambient temperature at infinity.

Convective Velocity

This input data creates the VELOCITY and VELOCITY CHANGE keyword options. Multiple VELOCITY CHANGE options are generated for the time dependent fields.


Input Data	Type	Analysis	Description
Velocity (V1,V2,V3)	Nodal	Thermal Coupled	Defines the convective velocity on the specified nodes by writing the VELOCITY option.
Use Sub. UVELOC	Nodal	Structural Thermal Coupled	If this toggle is ON, the use of the UVELOC routine is flagged by placing a -1 in the 1st field of the 2nd data block of the VELOCITY or VELOCITY CHANGE options. Data blocks 3-5 are not required if this is the case.

Potential

This input data creates the FIXED EL-POT or FIXED MG-POT keyword option for electrostatic or magnetostatic analysis. This LBC is ignored if not applicable to the selected analysis type.


Input Data	Type	Analysis	Description
Potetnial	Nodal	Coupled	Defines the electrostatic potential.
Top Bottom Middle Potential	Element Variable	Coupled	Same as previous except allows for potential definition at the various degrees of freedom for shell elements in 3D analysis.

Charge

This input data creates the POINT CHARGE or DIST CHARGES keyword options for electrostatic analysis. This LBC is ignored if not applicable to the selected analysis type.


Input Data	Type	Analysis	Description
Charge	Nodal Element Uniform	Coupled	Defines the electrostatic charge. Nodal definitions write the POINT CHARGE and Element Uniform definitions write the DIST CHARGES option.
Top Bottom Middle Charge	Element Variable	Coupled	Same as previous except allows for charge definition at the various degrees of freedom for shell elements in 3D analysis. Writes the POINT CHARGE option.

Voltage

This input data creates the FIXED VOLTAGE keyword option for thermal-electrodynamic (Joule heating) analysis. This LBC is ignored if not applicable to the selected analysis type.


Input Data	Type	Analysis	Description
Voltage	Nodal	Coupled	Defines the applied voltage.
Top Bottom Middle Voltage	Element Variable	Coupled	Same as previous except allows for voltage definition at the various degrees of freedom for shell elements in 3D analysis.

Current

This input data creates the POINT CURRENT or DIST CURRENT keyword options thermal-electrodynamic (Joule heating) and other applicable analyses. This LBC is ignored if not applicable to the selected analysis type.


Input Data	Type	Analysis	Description
Current	Nodal Element Uniform	Coupled	Defines the applied current.
Top Bottom Middle Current	Element Variable	Coupled	Same as previous except allows for current definition at the various degrees of freedom for shell elements in 3D analysis.

Magnetization

Creates the PERMANENT option in magnetostatic analysis.


Input Data	Type	Analysis	Description
Remenance	Element Uniform	Coupled	Defines a permanent magnet for magnetostatic analysis (vector input).

Contact

Defines deformable and rigid contact bodies, and creates certain data entries in the CONTACT and MOTION CHANGE keyword options. Other data entries in the CONTACT option are defined under the Analysis application when setting up a job for nonlinear static or nonlinear transient dynamic analysis. A CONTACT TABLE option is also supported; by default, all contact bodies initially have the potential to interact with all other contact bodies and themselves. This default behavior can be modified under the Contact Table form, located on the Solution Parameters form in the Analysis application when creating a Load Step. See Contact Parameters and Contact Table.


Note:	For pure heat transfer analysis, the THERMAL CONTACT options is used instead of CONTACT.

The Application Region form for contact is used to select the contact bodies whether they be deformable or rigid. Deformable contact bodies are always defined as a list of elements or a list of elements associated to a geometric entity, the boundary of which defines the contact surface. Rigid bodies are translated as ruled surfaces or 3-noded patches (2D) or straight line segments (1D) if a mesh or geometry with an associated mesh is selected. Otherwise, if no mesh is associated with the selected geometry, the contact definition will be written as geometric NURB surfaces during translation. 2D meshed surfaces can use 4 or 8 noded quads, or 3 or 6 noded tri elements, however the mid-side nodes are unnecessary and ignored for the higher order elements.


Caution:	The line segments of a meshed rigid body will be translated only if they form a continuous sequence of 1D elements (i.e. no branches, and common nodes between adjoining elements). And the sequence of nodes must be open (i.e., the first node should be distinct from the last one). Note that a mesh of a closed loop composed of a single curve should not be equivalenced so as to make an open sequence of nodes. However, if the mesh used two curves, only one pair of common nodes should be equivalenced.

Deformable Body

These input properties are defined for each deformable body defined on the CONTACT keyword option. They can be overridden if defined with non-zero values in the CONTACT TABLE. Also the SPLINE option for representing a deformable body with an analytical surface to improve accuracy is defined here


Input Data	Type	Analysis	Description
Structural Properties:
Friction Coefficient (MU)	Element Uniform	Structural Coupled	Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients, the average value is used. Only available for Structural and Coupled analysis.
Thermal Properties:
Heat Transfer Coefficient to Environment	Element Uniform	Thermal Coupled	Heat transfer coefficient (film) to environment. This is only allowed for thermal or coupled analysis.
Environment Sink Temperature	Element Uniform	Thermal Coupled	Environment sink temperature. This is only allowed for thermal or coupled analysis.
Contact Heat Transfer Coefficient	Element Uniform	Thermal Coupled	Contact heat transfer coefficient (film). This is only allowed for thermal or coupled analysis.
Near Contact Heat Transfer Coefficient	Element Uniform	Thermal Coupled	Near Contact heat transfer coefficient (film). This is only allowed for thermal or coupled analysis. Requires that a tolerance distance be defined in the Contact Table. Heat fluxes have components of convection and radiation which are defined in the next properties.
Natural Convection Coefficient	Element Uniform	Thermal Coupled	Natural convetion coefficient used with near thermal contact. This is only allowed for thermal or coupled analysis.
Natural Convection Exponent	Element Uniform	Thermal Coupled	Natural convetion exponent used with near thermal contact. This is only allowed for thermal or coupled analysis.
Surface Emissivity	Element Uniform	Thermal Coupled	Surface emissivity used with near thermal contact radiation component. This is only allowed for thermal or coupled analysis.
Distance Dependent Heat Transfer Coefficient	Element Uniform	Thermal Coupled	Distance dependent heat transfer coefficient used with near thermal contact. This is only allowed for thermal or coupled analysis.
Electrical Properties (only written in TABLE format):
Conductivity	Element Uniform	Coupled	Electrical transfer coefficient to environment. Only used in Coupled analysis (Joule Heating).
Sink Voltage	Element Uniform	Coupled	Environment sink voltage. Only used in Coupled analysis (Joule Heating).
Contact Conductivity	Element Uniform	Coupled	Electrical transfer coefficient to environment. Only used in Coupled analysis (Joule Heating).
Near Contact Conductivity	Element Uniform	Coupled	Electrical transfer coefficient for near field behavior. Only used in Coupled analysis (Joule Heating).
Distance Dependent Conductivity	Element Uniform	Coupled	Separation distance dependent electrical transfer coefficient. Only used in Coupled analysis (Joule Heating).
Analytical Contact Definition:
Boundary Type	Element Uniform	Structural Thermal Coupled	By default a deformable contact body boundary is defined by its elements (Discrete). However, you can use an Analytic surface to represent the deformable body. This improves the accuracy for deformable-deformable contact analysis by describing the outer surface of a contact body by a spline (2D) or Coons surface (3D) description. This writes a SPLINE option to the input file.
MFD Increment	Element Uniform	Structural Thermal Coupled	This places the number specified in the 2nd field of the 2nd data block of the SPLINE option. An MFD file will be written every n increments as specified by this number. This file can be viewed my Marc Mentat to ensure the spline or coon surface data is being properly generated to define the proper discontinuities.
Select Discontinuities	Element Uniform	Structural Thermal Coupled	This is an optional input. The Analytic surface of a deformable body can be described by a spline (2D) or Coons surface (3D) and by default the entire outer surface will be included unless an Exclusion Region is selected. The exclusion region is a region of discontinuity where you don’t want a spline or coons surface fit. You may select either Geometry or FEM entities of the contact body to define these regions. For 2D analysis, the exlusion region consists of nodes that describe vertices through which a spline should not be fit. You select either individual nodes or geometric entities from which the associated nodes are extracted. For 3D analysis, the exlusion region consists of element edges across which a coons surface should not be fit. You select individual element edges or geometric curves/edges of surfaces/solids from which the associated element edges are extracted. You can set the Detect Discontinuities and give a feature angle if you wish the program to automatically detect these exclusion regions. Once the entities are determined, you may edit them as necessary.
Auto Detect Discontinuities Feature Angle	Element Uniform	Structural Coupled	You can indicate for the Marc analysis to automatically detect the discontinuities by turning this toggle on and using the specified Feature Angle. This Feature Angle is also used by Patran if you click on the Detect Discontinuities button if you wish to view the discontinuity selection manually before submitting the job.
Contact Area Definition:
Select Contact Area	Element Uniform	Structural Coupled	You may define the nodes that are most likely to come into contact to speed up the compute time of the analysis when using contact. This writes the CONTACT NODE option to the input deck. The nodes associated to the entities selected are written. A node not included in this list that is part of the contact body may penetrate other bodies.
Exclusion Region:
Select Exclusion Region	Element Uniform	Structural Coupled	For certain contact problems, you might wish to influence the decision regarding the deformable segment a node contacts. You can specify element edges for 2D and surfaces for 3D analysis to be excluded from the contacted bodies. This writes the EXLUDE option to the input deck. The segments to be excluded are written by extracting the nodes that define the edge or surface.
Rigid Body Motion Properties:
Treat as Rigid	Element Uniform	Coupled	A deformable body in Coupled analysis can be treated as a simple rigid heat transfer body. In this case, many of the rigid body attributes, such as motion control can also be applied. See the input properties for Rigid Bodies below.

Rigid Body

These input properties are defined for each rigid body defined on the CONTACT keyword option. The input data form differs for 1D and 2D rigid bodies. One dimensional rigid surfaces are defined as beam elements, or as curves (which may be meshed with beam elements prior to translation) and used in 2D problems. The lines or beams must be in the global X-Y plane. Two dimensional rigid surfaces must be defined as Quad/4 or Tri/3 elements, or as surfaces (which may be meshed with Quad/4 or Tri/3 elements prior to translation) and are used in 3D problems. The elements will be translated as ruled surfaces if meshed or as NURB surfaces if not meshed in the Marc input file


Input Data	Type	Analysis	Description
Flip Contact Side	Element Uniform	Structural Coupled 1D/2D	Upon defining each rigid body, Patran displays normal vectors or tic marks. These should point inward to the rigid body. In other words, the side opposite the side with the vectors is the side of contact. Generally, the vector points away from the body in which it wants to contact. If it does not point inward, then UNDO the definition of the rigid surface, turn this toggle ON, and create the rigid surface again. The direction of the inward normal will be reversed.
Symmetry Plane	Element Uniform	Structural Coupled 1D/2D	This specifies that the surface or body is a symmetry plane. This places a one (1) in the 3rd field of the 4th data block of the CONTACT option. It is OFF by default.
Motion Control:
Null Initial Motion	Element Uniform	Structural Coupled 1D/2D	This toggle is enabled only for Velocity and Position type of Motion Control. If it is ON, the intitial velocity, position, and angular velocity/rotation are set to zero in the CONTACT option regardless of their settings here (for increment zero).
Motion Control	Element Uniform	Structural Coupled 1D/2D	Motion of rigid bodies can be controlled in a number of different ways: velocity, position (displacement), or forces/moments.
Velocity (vector)	Element Uniform	Structural Coupled 1D/2D	For velocity controlled rigid bodies, define the X and Y velocity components for 2D problems or X, Y, and Z for 3D problems. Data is placed on MOTION CHANGE option.
Angular Velocity (rad/time)	Element Uniform	Structural Coupled 1D/2D	For velocity controlled rigid bodies, if the rigid body rotates, give its angular velocity in radians per time (seconds usually) about the center of rotation (global Z axis for 2D problems) or axis of rotation (for 3D problems). Data is placed on MOTION CHANGE option.
Velocity vs Time Field	Element Uniform	Structural Coupled 1D/2D	If a rigid body velocity changes with time, its time definition may be defined through a non-spatial field, which can then be selected via this widget. It will be scaled by the vector definition of the velocity as defined in the Velocity widget. The Angular Velocity will also be scaled by this time field. See the explanation below in Rigid Body Motion.
Displacement (vector)	Element Uniform	Structural Coupled 1D/2D	For position controlled rigid bodies, define the final X and Y position in global coordinates for 2D problems or X, Y, and Z for 3D problems. Data is placed on MOTION CHANGE option.
Angular Position (radians)	Element Uniform	Structural Coupled 1D/2D	For position controlled rigid bodies, if the rigid body rotates, give its final angular position in radians about the center of rotation (global Z axis for 2D problems) or axis of rotation (for 3D problems). Data is placed on MOTION CHANGE option.
Displacement vs Time Field	Element Uniform	Structural Coupled 1D/2D	If a rigid body position changes with time, its time definition may be defined through a non-spatial field, which can then be selected via this widget. It will be scaled by the vector definition of the position as defined in the Displacement widget. The Angular Position will also be scaled by this time field. See the explanation below in Rigid Body Motion.
Rotation Reference Point	Element Uniform	Structural Coupled 1D/2D	This is a point or node that defines the center of rotation of the rigid body. If left blank the rotation reference point will default to the origin. This is placed on the 5th data block of the CONTACT option. For Force/Moment driven bodies, this is the First Control Node.
Axis of Rotation	Element Uniform	Structural/2D Coupled/2D	For 2D rigid surfaces in a 3D problem, aside from the rotation reference point, if you wish to define rotation you must also specify the axis in the form of a vector. This is placed in the 6th data block of the CONTACT option. (Z-axis is the default: <0., 0., 1.>)
First Control Node	Element Uniform	Structural Coupled 1D/2D	This is for Force controlled rigid motion. It is the node to which the force is applied. A separate LBC must be defined for the force, but the application node must also be specified here. If both force and moment are specified, they must use different control nodes even if they are coincident. The node number is placed in the 6th field of the 4th data block of the CONTACT option. This node also acts as the center of rotation (Rotation Reference Point).
Second Control Node	Element Uniform	Structural Coupled 1D/2D	This is for Moment controlled rigid motion. It is the node to which the moment is applied, sometimes called the auxiliary node. A separate LBC must be defined for the moment, but the application node must also be specified here. If both force and moment are specified, they must use different control nodes even if they are coincident. The node number is placed in the 7th field of the 4th data block of the CONTACT option. The moment acts around the Rotation Reference Point, which is the First Control Node.
Approach Velocity	Element Uniform	Structural Coupled	This defines the approach velocity of rigid bodies to position them in contact before the analysis proceeds. This is useful mostly when using load controlled rigid bodies. This is generally written to the 6th data block of the CONTACT option for VERSION, 10 formated files and is only valid for MSC.Marc 2003 or greater.
Approach Angular Velocity	Element Uniform	Thermal Coupled	See Approach Velocity.
Number of Subdivision	Element Uniform	Structural Thermal Coupled	In the NURB definition portion of the CONTACT option, these data specify the number of subdivision in the U, V directions for surface data and the number of subdivisions for curves or trimming curves.
Structural Properties:
Friction Coefficient (MU)	Element Uniform	Structural Coupled 1D/2D	Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients the average value is used. This is placed in the 5th, 6th, or 7th data block of the CONTACT option depending on the dimensionality of the problem.
Thermal Properties:
Heat Transfer Coefficients, Convection, Emissivity	Element Uniform	Thermal/ Coupled 1D/2D	All of these heat transfer properties are the same as defined for deformable bodies above.
Body Temperature	Element Uniform	Thermal/ Coupled 1D/2D	Body temperature. Only necessary for coupled analysis. This is placed in the 5th, 6th, or 7th data block of the CONTACT option depending on the dimensionality of the problem.
Electrical Properties (only written in TABLE format):
Body Voltage	Element Uniform	Coupled	Rigid body voltage. Only used in Coupled analysis (Joule Heating).
Contact Conductivity	Element Uniform	Coupled	Electrical transfer coefficient to environment. Only used in Coupled analysis (Joule Heating).
Near Contact Conductivity	Element Uniform	Coupled	Electrical transfer coefficient for near field behavior. Only used in Coupled analysis (Joule Heating).
Distance Dependent Conductivity	Element Uniform	Coupled	Separation distance dependent electrical transfer coefficient. Only used in Coupled analysis (Joule Heating).


Note:	The order in which you see rigid and deformable bodies in the contact table and written to the Marc input file is by alphabetical order with deformable bodies listed first and not in the order in which they were created. If you need to reorder them, you can do so by renaming them under the Modify action in the Loads/BCs application.

Rigid Body Motion

The motion of rigid bodies is defined under this contact LBC. The motion can be specified as velocity driven, position driven, or force/moment driven. In the latter case, you must define your force and/or moment via the appropriate LBC and apply it to a node which is then referenced as the control node when defining the rigid body. The first control node is for force and the second is for moment. These nodes must be different.

For velocity or position driven rigid bodies, you define a vector describing the velocity or position. Each rigid body can only reference a single vector to describe this motion plus another scalar value describing the angular velocity or position (in radians/sec. or radians, respectively). It is possible to describe the velocity or position via a time varying field. You may use two different field dimensionalities to describe this motion. A one dimensional nonspatial field may be selected in which case all components of the velocity or position vector are scaled by this time varying field, including the angular velocity/position. This does not allow separate control of each component and is limited in this respect.

If you must have separate time varying control for all components of the velocity or position, then you must use a 2D nonspatial field where the independent variables are time(t) and velocity(v) or time(t) and displacement(u). This allows you to define time in the first column, the v1,v2,v3 or u1,u2,u3 in the 2nd through 3rd columns and the angular velocity/position in the 4th column. If a particular component does not move, you must leave that column of the field blank. The header values of the velocity or position columns must be input in increasing values, however these values are ignored. Please see Non-Spatial Fields for an example.


Note:	You can preview the motion with the Preview Motion button on the main form. If this toggle is ON, the selected rigid body will move according to the motion definition. This is useful to determine that the motion control has been defined properly. This works with time dependent fields also.

The Preview Motion as mentioned in the note above issues this PCL command:

lbc_animate_rb_motion( lbc_name, start_time, end_time, num_frames, time_delay)

where:


lbc_name	Name of the contact body in double quotes, e.g., “rigid_body”
start_time	Time you wish motion to start. If not defined by a time dependent field, this should be set to zero.
end_time	Time you wish motion to end. If not defined by a time dependent field, this should get set to one.
num_frames	The number of frames you wish to see animated. The more you specify the smoother the animation will look but the longer it will take.
time_delay	The time delay between dispaly of individual frames in milliseconds.