Object | Type |
• Displacement | • Nodal • Element Uniform • Element Variable |
• Force | • Nodal |
• Pressure | • Element Uniform • Element Variable |
• Nodal • Element Uniform • Element Variable | |
• Element Uniform | |
• Nodal | |
• Nodal | |
• Velocity | • Nodal |
• Acceleration | • Nodal |
• Element Uniform • Element Variable | |
• CID Distributed Load | • Element Uniform • Element Variable |
• Total Load | • Element Uniform |
• Contact | • Element Uniform |
• Initial Plastic Strain | • Element Uniform |
• Initial Stress | • Element Uniform |
• Initial Temperature | • Nodal |
• Planar Rigid Wall * | • Nodal |
• Init. Rotation Field * | • Nodal |
Object | Type | Analysis Type | Option |
Displacement Velocity Acceleration | Nodal | Structural | Standard |
Input Data | Description |
Translations (T1,T2,T3) | Defines the total enforced translational values. These are in model length units. |
Rotations (R1,R2,R3) | Defines the total enforced rotational values. These are in radians. |
Translational Phase Angles (Tth1,Tth2,Tth3) | Defines the phase angle for out-of-phase loading in frequency response analysis for the translational values. These are in degrees. |
Rotational Phase Angles (Rth1,Rth2,Rth3) | Defines the phase angle for out-of-phase loading in frequency response analysis for the rotational values. These are in degrees. |
Object | Type | Analysis Type | Dimension |
Displacement | Element Uniform Element Variable | Structural | 3D |
Input Data | Description |
Translations (T1,T2,T3) | Defines the enforced translational displacement values. These values are in model-length units. |
Translation Phases (Tth1,Tth2,Tth3) | Defines the phase angle for out-of-phase loading in frequency response analysis for the translational displacement values. These are in degrees. |
Object | Type | Analysis Type | Option |
Displacement | Nodal | Structural | Relative Displacement |
Input Data | Description |
Relative Translations (T1,T2,T3) | Defines the relative enforced translational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced translation is to be specified, the particular component should be left blank. |
Relative Rotations (R1,R2,R3) | Defined the relative enforced rotational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced rotation is to be specified, the particular component should be left blank. |
Object | Type | Analysis Type |
Force | Nodal | Structural |
Input Data | Description |
Force (F1,F2,F3) | Defines the applied forces in the translation degrees of freedom. This defines the N vector and the F magnitude on the FORCE entry. |
Moment (M1,M2,M3) | Defines the applied moments in the rotational degrees of freedom. This defines the N vector and the M magnitude on the MOMENT entry. |
Force Phase Angles (Fth1,Fth2,Fth3) | Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding force components. These are in degrees. |
Moment Phase Angles (Mth1,Mth2,Mth3) | Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding moment components. These are in degrees. |
Object | Type | Analysis Type | Dimension |
Pressure | Element Uniform | Structural | 2D |
Input Data | Description |
Top Surf Pressure | Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. These values are all equal for a given element, producing a uniform pressure field across that face. |
Bot Surf Pressure | Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values.These values are all equal for a given element, producing a uniform pressure field across that face. |
Edge Pressure | For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (i.e. independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated at the middle of the application region. |
Object | Type | Analysis Type | Dimension |
Pressure | Element Uniform | Structural | 3D |
Input Data | Description |
Pressure | Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated once at the center of the applied region. |
Object | Type | Analysis Type | Dimension |
Pressure | Element Variable | Structural | 2D |
Input Data | Description |
Top Surf Pressure | Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values. |
Bot Surf Pressure | Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values. |
Edge Pressure | For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (e.g., independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated independently at each node. |
Object | Type | Analysis Type | Dimension |
Pressure | Element Variable | Structural | 3D |
Input Data | Description |
Pressure | Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for each of the P1 through P4 values. |
Object | Type | Analysis Type |
Temperature | Nodal | Structural |
Input Data | Description |
Temperature | Defines the T fields on the TEMP entry. |
Object | Type | Analysis Type | Dimension |
Temperature | Element Uniform | Structural | 1D |
Input Data | Description |
Temperature | Defines a uniform temperature field using a TEMPRB entry. The temperature value is used for both the TA and TB fields. The T1a, T1b, T2a, and T2b fields are all defined as 0.0. |
Object | Type | Analysis Type | Dimension |
Temperature | Element Uniform | Structural | 2D |
Input Data | Description |
Temperature | Defines a uniform temperature field using a TEMPP1 entry. The temperature value is used for the T field. The gradient through the thickness is defined to be 0.0. |
Object | Type | Analysis Type | Dimension |
Temperature | Element Variable | Structural | 1D |
Input Data | Description |
Centroid Temp | Defines a variable temperature file using a TEMPRB entry. A field reference will be evaluated at either end of the element to define the TA and TB fields. |
Axis-1 Gradient | Defines the temperature gradient in the 1 direction. A field reference will be evaluated at either end of the element to define the T1a and T1b fields. |
Axis-2 Gradient | Defines the temperature gradient in the 2 direction. A field reference will be evaluated at either end of the element to define the T2a and T2b fields. |
Object | Type | Analysis Type | Dimension |
Temperature | Element Variable | Structural | 2D |
Input Data | Description |
Top Surf Temp | Defines the temperature on the top surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry. |
Bot Surf Temp | Defines the temperature on the bottom surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry. |
Object | Type | Analysis Type | Dimension |
Temperature | Element Uniform Element Variable | Structural | 1D, 2D, 3D |
Input Data | Description |
Temperature | Defines the temperature or temperature distribution in the element. |
Object | Type | Analysis Type |
Inertial Load | Element Uniform | Structural |
Input Data | Description |
Trans Accel (A1,A2,A3) | Defines the N vector and the G magnitude value on the GRAV entry. |
Rot Velocity (w1,w2,w3) | Defines the R vector and the A magnitude value on the RFORCE entry. |
Rot Accel (a1,a2,a3) | Defines the R vector and the RACC magnitude value on the RFORCE entry. |
Object | Type | Analysis Type |
Initial Displacement | Nodal | Structural |
Input Data | Description |
Translations (T1,T2,T3) | Defines the U0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry. |
Rotations (R1,R2,R3) | Defines the U0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry. |
Object | Type | Analysis Type |
Initial Velocity | Nodal | Structural |
Input Data | Description |
Trans Veloc (v1,v2,v3) | Defines the V0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry. |
Rot Veloc (w1,w2,w3) | Defines the V0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry. |
Object | Type | Analysis Type | Dimension |
Distributed Load | Element Uniform Element Variable | Structural | 1D |
Input Data | Description |
Edge Distributed Load (f1,f2,f3) | Defines the FXE, FYE, and FZE fields on three PLOAD1 entries. |
Edge Distributed Moment (m1,m2,m3) | Defines the MXE, MYE, and MZE fields on three PLOAD1 entries. |
Object | Type | Analysis Type | Dimension |
Distributed Load | Element Uniform Element Variable | Structural | 2D |
Input Data | Description |
Edge Distributed Load (f1,f2,f3) | For axisymmetric solid elements (CTRIAX6), the PA, PB, and THETA fields on the PLOADX1 entry are defined. For other 2D elements, the input vector is interpreted as load per unit length and converted into equivalent nodal loads (FORCE entries). |
Edge Distributed Moment (m1,m2,m3) | For 2D shell elements, the input vector is interpreted as moment per unit length and converted into equivalent nodal moments (MOMENT entries). |
Object | Type | Analysis Type |
Contact | Element Uniform | Structural |
Input | Description |
Penetration Type | If the Penetration Type is One Sided, nodes in the Slave Region are not allowed to penetrate the segments of the Master Region. If Symmetric, in addition, nodes in the Master Region are not allowed to penetrate segments of the Slave Region. |
Static Friction Coefficient (MU1) | Coefficient of static friction between the two surfaces. |
Stiffness in Stick (FSTIF) | FSTIF is a penalty parameter in the contact formulation. The default value is usually adequate. |
Penalty Stiffness Scaling Factor (SFAC) | SFAC is a penalty parameter in the contact formulation. The default value is usually adequate. |
Slideline Width (W1) | Slideline Width is constant along the slideline and is used to determine the area for contact stress calculation. This is the Wi field on the BFRIC entry. |
Vector Pointing from Master to Slave Surface | A vector must be defined which lies in the contact plane and points from the Master region to the Slave region. This vector is used to define the coordinate system on the BCONP entry and the BLSEG entries for each region. |
Description | |
Friction Coefficient (MU) | Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients, the average value is used. |
Define (type of contact) | Select 1) Analytic Contact, 2) Contact Area, 3) Exclusion Region, or 4) Glue Deactivation. The Contact Area and Exclusion Region are defined using MD Nastran entry BCHANGE in the .bdf file, with NODE for Contact Area, and EXCLUDE for Exclusion Region. The Glue Deactivation is defined using MD Nastran entry UNGLUE. |
Boundary Type | Select either 1) Analytic, or 2) Discrete. By default, a deformable contact body boundary is defined by the free faces of its elements; this is used by the Discrete option. However, instead of using the free faces of the elements (Discrete), it is possible to use spline surfaces (2D) to represent the outer faces (element faces) of the contact bodies; this is used by the Analytic option. The Analytic option can improve the accuracy of deformable-deformable contact analysis. |
C0 Continuity | Using this, enforces C0-continuity at edges where the normal vector to the outer contour of the structure indicates a discontinuity. This is enabled for 3D analysis only. |
Auto Detect Discontinuities | Select this to cause the automatic detection of any discontinuity. |
Feature Angle | If the angle between the normals of two touching (adjacent) segments of contact bodies is greater than the Feature Angle, there is a discontinuity there, and the discontinuity (at edge) is preserved. |
MFD Increment | The MFD file contains the spline surfaces that were created to represent some or all of the outer faces of the contact model. Using this causes the spline surfaces to be written to an MFD file every nth increment. This file is an Patran database, and can be opened with Patran, and the spline surfaces can be compared with the contact model. |
Select Discontinuities... | |
Edge Contact... | |
Select Contact Area... | |
Select Exclusion Region... | |
Select Deactivation Region... |
Description | |
Select (entity type) | Choose to either select Geometry or FEM to define any discontinuities. |
Detect Discontinuities | Click on this button to determine if there are any discontinuities for the entities that define the Application Region. |
Define Discontinuities | Select entities to define the discontinuities. |
Description | |
Include Outside (Solid Element) | When detecting contact of solid elements (for example, CHEXA elements) use this to include contact of the outside of the elements. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact). |
Check Layers (Shell Element) | For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block. |
Ignore Thickness | Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block. |
Include Edges (Edges) | Use this to specify how body surfaces may contact. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact). |
Description | |
Select (entity type) | Choose to either select Geometry or FEM to define the contact area. |
Define Contact Area | Select entities to define the contact area. |
Description | |
Select (entity type) | Choose to either select Geometry or FEM to define the exclusion region. |
Define Exclusion Region | Select entities to define the exclusion region. |
Description | |
Select (entity type) | Choose to either select Geometry or FEM to define the glue deactivation region. |
Define Deactivated Entities | Select entities to define the entities that are to be un-glued. |
Input | Description |
Flip Contact Side | Upon defining each rigid body, MSC.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 use the modify option to turn this toggle . The direction of the inward normal will be reversed. |
Symmetry Plane | This specifies that the surface or body is a symmetry plane. It is by default. |
Null Initial Motion | This toggle is enabled only for Velocity and Position type of Motion Control. If it is ON, the initial velocity, position, and angular velocity/rotation are set to zero in the CONTACT option regardless of their settings here (for increment zero). |
Motion Control | Motion of rigid bodies can be controlled in a number of different ways: velocity, position (displacement), or forces/moments. |
Velocity (vector) | For velocity controlled rigid bodies, define the X and Y velocity components for 2D problems or X, Y, and Z for 3D problems. |
Angular Velocity (rad/time) | 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). |
Friction Coefficient (MU) | Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients the average value is used. |
Rotation Reference Point | 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. |
Axis of Rotation | 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. |
First Control Node | This is for Force or SPCD controlled rigid motion. It is the node to which the force or SPCD 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. If only 1 control node is specified the rigid body will not be allowed to rotate. |
Second Control Node | This is for Moment controlled rigid motion. It is the node to which the moment is applied. A separate LBC must be defined for the moment, but the application node must also be specified here. It also acts as the rotation reference point. If both force and moment are specified, they must use different control nodes even if they are coincident. |
Object | Type | Analysis Type |
Planar Rigid Wall | Nodal | Explicit Nonlinear |
Input Data | Description |
Static Friction Coefficient | Static coefficient of friction. |
Kinetic Friction Coefficient | Kinetic coefficient of friction. |
Exponential Decay Coefficient | Exponential decay coefficient EXP. |
Object | Type | Analysis Type |
Init. Rotation Field | Nodal | Explicit Nonlinear |
Input Data | Description |
Trans Veloc(v1,v2,v3) | Defines the initial translational velocity values. These are in model length units per unit time. |
Rot Veloc (w1,w2,w3) | Defines the initial rotational velocity values. These are in degrees per unit time. |
Rotation Center | Defines a point at the center of rotation. |