The Loads and Boundary Conditions form will appear when the Loads/BCs toggle, located on the Patran main form, is chosen. When creating a load and boundary condition there are several option menus. The selections made on the Loads and Boundary Conditions menu will determine which load and boundary conditions form appears, and ultimately, which MD Nastran loads and boundary conditions will be created.

The following pages give an introduction to the Loads and Boundary Conditions form and details of all the loads and boundary conditions supported by the Patran MD Nastran Analysts Preference.

This form appears when Loads/BCs is selected on the main menu. The Loads and Boundary Conditions form is used to provide options to create the various MD Nastran loads and boundary conditions. For a definition of full functionality, see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual. Options for defining slide line contact are also accessed from this main Loads and Boundary Conditions form. For more information see Defining Contact Regions, 242.

The following table outlines the options when Create is the selected Action.

* For SOL 700 only.

This subordinate form appears when the Input Data button is selected on the Loads and Boundary Conditions form and the Current Load Case Type is Static. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 219. The information on the Input Data form will vary depending on the selected Object. Defined below is the standard information found on this form.

This subordinate form appears when the Input Data button is selected on the Loads and Boundary Condition form and the Current Load Case Type is Time Dependent. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 219 and Load Cases, 241. The information on the Input Data form will vary, depending on the selected Object. Defined below is the standard information found on this form.

These are areas on the static and transient input data forms where the load data values are defined. The data fields that appear depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. The following Object Tables outline and define the various input data that pertains to a specific selected object:

Creates MD Nastran SPC1 and SPCD Bulk Data for Displacement entries. All non blank entries will cause an SPC1 entry to be created. If the specified value is not 0.0, an SCPD entry will also be created to define the non zero enforced displacement or rotation. Phase angle specifications will create DPHASE entries for all corresponding non blank translational or rotational data in frequency response analysis. Displacement, Velocity and Acceleration LBCs used in frequency response / dynamic analysis also define the RLOAD1 entries with DISP, VELOC, and ACCEL keywords, respectively. For frequency response analysis, the LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this. Values given via this option are total enforced values. For relative enforced values used in SOL 400, see the description for the Relative Displacement option below.

Applies a zero or nonzero total displacement boundary condition to the face of solid elements. The primary use of this boundary condition is to apply constraints to p-elements; but it may also be used for standard solid elements. If applied to a p-element solid, the appropriate FEFACE and GMBC entries are created. If applied to a standard solid element, the appropriate SPC1 and SPCD entries are created. In frequency response analysis, the phase angles are written as DPHASE entries. See comments above for nodal displacements.

Applies a zero or nonzero relative displacement boundary condition as opposed to a total magnitude. This is used in SOL 400 only with multiple steps and not applicable to other solution sequences. This LBC will be ignored if present in a referenced load case for solution sequences other than SOL 400. The appropriate SPC1 and SPCR entries are created. For example, if a DOF is specified on a SPCR with 0.0 for step 2, the relative displacement of this DOF for step 2 with respective to step 1 is 0.0. The total displacement of step 2 is 0.2 if the solution of step 1 for this DOF is 0.2.

Creates MD Nastran FORCE and MOMENT Bulk Data entries. Creates the DPHASE entries in frequency response analysis when specifying phase angles for out-of-phase loading. RLOAD1 entries are created for dynamic analysis and reference the appropriate FORCE entries. For frequency response analysis, the force LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this.

Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries.

Creates MD Nastran PLOAD4 Bulk Data entries.

Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries.

Creates MD Nastran PLOAD4 Bulk Data entries.

Creates MD Nastran TEMP Bulk Data entries.

Writes the TEMPP1 entry. For 2D Target Elements, T1/T2 or TBAR/TPRIME are written to the TEMPP1 entry but not both. For Equivalent Section shell properties or shell properties that have Z1/Z2 defined, T1/T2 is written and TBAR/TPRIME left blank on the TEMPP1 entry. Nastran determines the correct TPRIME. For all other shell properties TBAR/TPRIME are written and T1/T2 left blank. TBAR/TPRIME are computed by Patran from T1/T2 using the thickness property value. This is for Element Variable Temperature LBCs. For Element Uniform Temperature LBC, only TBAR is written or necessary. All others fields are left blank.

Creates MD Nastran TEMPRB Bulk Data entries.

Creates MD Nastran TEMPP1 Bulk Data entries.

Creates MD Nastran TEMPRB Bulk Data entries.

Creates MD Nastran TEMPP1 Bulk Data entries.

This option applies only to the P-formulation elements. A TEMPF and DEQATN entry are created for the constant temperature case. A TEMPF and TABLE3D entry are created for the case when a spatial field is referenced. Writes the TEMPP1 entry. For 2D Target Elements, T1/T2 or TBAR/TPRIME are written to the TEMPP1 entry but not both. For Equivalent Section shell properties or shell properties that have Z1/Z2 defined, T1/T2 is written and TBAR/TPRIME left blank on the TEMPP1 entry. Nastran determines the correct TPRIME. For all other shell properties TBAR/TPRIME are written and T1/T2 left blank. TBAR/TPRIME are computed by Patran from T1/T2 using the thickness property value. This is for Element Variable Temperature LBCs. For Element Uniform Temperature LBC, only TBAR is written or necessary. All others fields are left blank.

Creates MD Nastran GRAV and RFORCE Bulk Data entries.

The acceleration and velocity vectors are defined with respect to the input analysis coordinate frame. The origin of the rotational vectors is the origin of the analysis coordinate frame. Note that rotational velocity and rotational acceleration cannot be defined together in the same set.In generating the GRAV and RFORCE entries, the interface produces one GRAV and/or RFORCE entry image for each Patran load set.

Creates a set of MD Nastran TIC Bulk Data entries.

Creates a set of MD Nastran TIC Bulk Data entries.

Defines distributed force or moment loading along beam elements using MD Nastran PLOAD1 entries. The coordinate system in which the load is applied is defined by the beam axis and the Bar Orientation element property. The Bar Orientation must be defined before this Distributed Load can be created. If the Bar Orientation is subsequently changed, the Distributed Load must be updated manually if necessary.

For the element variable type, a field reference is evaluated at each end of the beam to define a linear load variation.

Defines a distributed force or moment load along the edges of 2D elements. The coordinate system for the load is defined by the surface or element edge and normal. The x direction is along the edge. Positive x is determined by the element corner node connectivity. See Patran Element Library (p. 345) in the Reference Manual - Part III. For example, if the element is a CQUAD4, with node connectivity of 1, 2, 3, 4. The positive x directions for each edge would be from nodes 1 to 2, 2 to 3, 3 to 4, and 4 to 1. The z direction is normal to the surface or element. Positive z is in the direction of the element normal. The y direction is normal to x and z. Positive y is determined by the cross product of the z and x axes and always points into the element. The MD Nastran entries generated, depend on the element type.

For the element variable type, a field reference is evaluated at all element nodes lying on the edge.

This form is used to define certain data for the MD Nastran contact entries. Other data entries for contact are defined under the Analysis Application when setting up a job for nonlinear static or nonlinear transient dynamic analysis. A contact table 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 subform in the Analysis Application when creating a Load Step.

Note that contact bodies (BCBODY entry) are written to the MD Nastran input deck in alphanumeric order, deformable bodies first followed by rigid bodies. The only way to control the order in which bodies are written to the input deck is to name them alphanumerically in the order you wish them to be written..

After defining the Input Properties you can use the Preview Rigid Body Motion to check the movement of the rigid bodies in place. This is an effective tool for verifying the directions for LBCs.

 

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 optionally be meshed with beam elements prior to translation) and used in 2D problems. Two dimensional rigid surfaces must be defined as Quad/4 or Tri/3 elements, or as surfaces (which may optionally be meshed with Quad/4 or Tri/3 elements prior to translation) and are used in 3D problems. The elements will be translated as 4-node patches if meshed or as NURB surfaces if not meshed.

Two different planar rigid wall options exist:

These are seen as options at the top of the Input Data form. The user must select which wall will be used. Both wall’s position and orientation are defined by selecting a coordinate system which has its origin on the plane and the local z axis as the outward normal from the contact surface. This defines a WALL Bulk Data entry. There are only parameters associated with the penalty based planar rigid wall.

Defines a velocity field of grid points consisting of a rotation and a traslation specification.

Creates a TIC3 Bulk Data entry.