Solution Parameters

MSC Nastran > Running an Analysis > 3.5 Solution Parameters

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

3.5 Solution Parameters

Linear Static

This subordinate form appears when the Dynamic Reduction button is selected on the Normal Modes, Complex Eigenvalue, Frequency Response, or Transient Response Solution Parameters forms. Use this form to create the DYNRED Bulk Data entry. Note that access to this form is only available when the Nastran version is less than 2005. Dynamic reduction parameters are not necessary for later versions of Nastran.


Database Run	Indicates whether a Structured Solution Sequence (SOL 101 or 114) is to be used or a Rigid Format (SOL 1 or 47). If selected, a Structured Solution Sequence is selected.
Cyclic Symmetry	Indicates that this model is a sector of a cyclically repeating part (SOL 114 or 47).
Automatic Constraints	Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Inertia Relief	Indicates that the inertia relief flags are to be set by including the PARAM, INREL,-1 command. This flag can only be chosen if Database Run is selected and Cyclic Symmetry is disabled. If inertia relief is selected, a node-ID for weight generation must be selected. A PARAM, GRDPNT and a SUPORT command will be written to the input file using the same node-ID selected for weight generation. The SUPORT entry will specify all 6 degrees of freedom.
Alternate Reduction	Indicates that an alternate method of performing the static condensation is desired. The PARAM, ALTRED,YES command is included if selected and if Database Run is also selected
SOL 600 Run	Indicates a SOL 600 run.
Contact Parameters	Same as the contact parameters available for the Implicit Nonlinear solution type. Only used with linear contact capability.
Shell Normal Tolerance Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Initial Temperature	Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature	Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry.
Rigid Element Type:	The Rigid element type optionmenu presents three different types of rigid elements, corresponding to the three possible values for the Nastran RIGID= case control. They are: • LINEAR: Selects linear rigid elements, which are the rigid elements that have been available in MD Nastran since its inception. • LAGR: Selects the new Lagrange rigid elements with the Lagrange multplier method. • LGELIM: Selects the new Lagrange rigid elements with the Lagrange elimination method. See the Nastran quick reference quide for more details.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

The table outlines the Database Run and Cyclic Symmetry selections, and the SOL types that will be used.


Database Run	Cyclic Symmetry	SOL
On	Off	101
On	On	114
Off	Off	1
Off	On	47

Nonlinear Static

This subordinate form appears when the Solution Parameters button is selected on the Solution Type form, when Nonlinear Static is selected. If the MD Nastran version specified is Version 66 or lower, then Solution Sequence (SOL) 66 will be employed. However, if the MD Nastran version specified is version 67 or higher, then Solution Sequence 106 will be employed except as described below. For more information about specification of the MD Nastran version number, see the Translation Parameters, 255 form.

The following table outlines the selections for Large Displacements and Follower Forces, and the altered LGDISP parameter setting for each.


Large Displacements	Follower Forces	LGDISP
Off	On	-1
On	On	1
On	Off	2

This is a list of the data input, available for defining the Nonlinear Static Solution Parameters, that were not shown on the previous page.


Parameter Name	Description
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Normal Modes

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Normal Modes is selected. Use this form to generate a SOL 103, 115, 3, or 48 input file, depending on the Database Run and Cyclic Symmetry parameters below.

The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each. Indicates whether a Structured Solution Sequence (SOLs 103 or 115) is to be used, or a Rigid Format (SOL 3 or 48). If Database Run is selected, a Structured Solution Sequence will be selected.


Database Run	Cyclic Symmetry	SOL
On	Off	103
On	On	115
Off	Off	3
Off	On	48

This is a list of data input, available for defining the Normal Modes Solution Parameters, that were not shown on the previous page.


Parameter Name	Description
Cyclic Symmetry	Indicates that this model is a sector of a cyclically repeating part (SOL 115 or 48).
Automatic Constraints	Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
SOL 600 Run	Select this to perform a SOL 600 analysis.
Residual Vector Computation	The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
Shell Normal Tolerance Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run (used to prevent runaway jobs). This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature	Specify the initial temperature.
Rigid Element Type	There are three ways to define a rigid element. They are 1) Linear, 2) Lagrangian, or 3) Lgelim.
Max p-Adaptive Cycles	Specify the maximum number of p-Adaptive cycles.
• Dynamic Reduction	Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Real Eigenvalue Extraction

This subordinate form appears when the Eigenvalue Extraction button is selected on the Normal Modes, Frequency Response, or Transient Response Solution Parameters forms. It also appears when the Real Eigenvalue Extraction button is selected on the Complex Eigenvalue Solution Parameter form. Use this form to create either EIGR or EIGRL Bulk Data entries.

This is a list of data input available for defining the Real Eigenvalue Extraction that was not shown on the previous page.


Parameter Name	Description
Number of Desired Roots	Indicates the limit to how many eigenvalues to be computed. This is the ND field on the EIGR or EIGRL Bulk Data entries.
Diagnostic Output Level	Defines the level of desired output. This can take any integer value between 0 and 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method	Indicates what type of eigenvalue normalization is to be done. This parameter can take one of three settings: Mass, Maximum, or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. Defines the setting of the NORM field on the EIGR Bulk Data entry.
Normalization Point	Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGR Bulk Data entry.
Normalization Component	Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGR Bulk Data entry.

Dynamic Reduction Parameters

Buckling

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Buckling is selected. Use this form to generate a SOL 105, 77, or 5 input file, depending on the setting of the Database Run and Cyclic Symmetry parameters.

The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each.


Database Run	Cyclic Symmetry	SOL
On	Off	105
On	On	77
Off	Off	5

This is a list of data input available for defining the Buckling Solution Parameters that were not shown on the previous page.


Parameter Name	Description
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
• Eigenvalue Extraction	Brings up the Buckling Eigenvalue Extraction form for defining the eigenvalue extraction controls.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Buckling Eigenvalue Extraction

This subordinate form appears when the Eigenvalue Extraction button is selected on the Buckling Solution Parameters form. Use this form to create either EIGB or EIGRL Bulk Data entries, depending on the selected extraction method.

This is a list of data input, available for defining the Buckling Eigenvalue Extraction, that was not shown on the previous page.


Parameter Name	Description
Number of Desired Positive Roots	Indicates the limit to how many positive eigenvalues to be computed. This value can only be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDP field on the EIGB entry.
Number of Desired Negative Roots	Indicates the limit to how many negative eigenvalues to be computed. This value cannot be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDN field on the EIGB entry.
Diagnostic Output Level	Defines the level of desired output. This can take any integer value in the range of 0 through 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method	Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the NORM field on the EIGB entry.
Normalization Point	Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGB entry.
Normalization Component	Defines the degree-of-freedom component at the Normalization Point to be used. This, too, can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGB entry.

Complex Eigenvalue

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Complex Eigenvalue is selected. When you specify the Database Run and Formulation parameters (from the Solution Type form), Patran generates a SOL 107, 110, 28, or 29 input file.

The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If you select Database Run, a Structured Solution Sequence (SOLs 107 or 110) will be selected. If you deselect Database Run a Rigid Format Solution Sequence (SOLs 28 or 29) will be selected.


Database Run	Formulation	SOL
On	Direct	107
On	Modal	110
Off	Direct	28
Off	Modal	29

This is a list of data input available for defining the Complex Eigenvalue Solution Parameters that was not shown on the previous page.


Parameter Name	Description
Automatic Constraints	Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Residual Vector Computation	The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
Shell Normal Tolerance Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature	Specify the initial temperature.
Default Load Temperature	Specify load temperature.
Rigid Element Type	There is one rigid element type, Linear.
Struct. Damping Coeff.	Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value).
• Complex Eigenvalue	Brings up the Complex Eigenvalue Extraction form for defining the complex eigenvalue extraction controls.
• Real Eigenvalue	Brings up the Real Eigenvalue Extraction form for defining the real eigenvalue extraction controls.
• Dynamic Reduction	Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Complex Eigenvalue Extraction

This subordinate form appears when the Complex Eigenvalue button is selected on the Complex Eigenvalue Solution Parameters form. Use this form to create an EIGC Bulk Data entry.

This is a list of data input available for defining the Complex Eigenvalue Extraction that was not shown on the previous page.


Parameter Name	Description
Omega of B Points	Defines the imaginary component of the end of lines in the complex plane. These values cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the OMEGABJ fields.
Width of Regions	Defines the width of the region in the complex plane. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the LJ fields.
Estimated Number of Roots	Indicates an estimate of the number of eigenvalues to be located within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NEJ fields.
Number of Desired Roots	Indicates the limit to how many eigenvalues to be computed within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NDJ fields.
Normalization Method	Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This is the NORM field on the EIGC entry.
Normalization Point	Defines the point to be used in the normalization. This is the G field on the EIGC Bulk Data entry.
Normalization Component	Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Extraction Method is set to Inverse Power or Determinate. This is the C field on the EIGC Bulk Data entry.

Frequency Response

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Frequency Response is selected. Patran generates a SOL 108, 111, 118, 26, or 30 input file when you specify the Database Run, Cyclic Symmetry, and Formulation parameters (from the Solution Type form).

The following table outlines the selections for Database Run, Formulation, and Cyclic Symmetry parameters, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 108, 111, 118) will be selected. If Database Run is deselected, a Rigid Format (SOLs 26 or 30) will be selected.


Database Run	Formulation	Cyclic Symmetry	SOL
On	Direct	Off	108
On	Direct	On	118
On	Modal	--	111
Off	Direct	--	26
Off	Modal	--	30

This is a list of data input, available for defining the Frequency Response Solution Parameters that were not shown on the previous page.


Parameter Name	Description
Cyclic Symmetry	Indicates that this model is a sector of a cyclically repeating part, and the appropriate flags will be set. This can only be set if Database Run is selected and Formulation is set to Direct (SOL 118).
Automatic Constraints	Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Residual Vector Computation	The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
Shell Normal Tolerance Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature	Specify the initial temperature.
Default Load Temperature	Specify load temperature.
Rigid Element Type	There is one rigid element type, Linear.
Struct. Damping Coeff.	Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value).
• Eigenvalue Extraction	Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal.
• Dynamic Reduction	Calls up another form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Transient Response

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Transient Response is selected. Patran generates a SOL 109, 112, 27, or 31 input file, when you specify Database Run and Formulation parameters (from the Solution Type form).

The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 109, 112) will be selected. If Database Run is deselected, a Rigid Format (SOLs 27 or 31) will be selected.


Database Run	Formulation	SOL
On	Direct	109
On	Modal	112
Off	Direct	27
Off	Modal	31

This is a list of data input available for defining the Transient Solution Parameters that was not shown on the previous page.


Parameter Name	Description
Automatic Constraints	Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Residual Vector Computation	The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
SOL 600 Run	Select this to perform a SOL 600 analysis.
SOL 700 Run	Select this to perform a SOL 700 analysis. To do this is necessary to use the Direct method.
Shell Normal Tolerance Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation	Defines how the mass matrix will be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature	Specify the initial temperature.
Default Load Temperature	Specify load temperature.
Rigid Element Type	There is one rigid element type, Linear.
Struct. Damping Coeff.	Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor W4, Damping Factor1	Defines W3 and W4 parameters. These parameters alter the damping characteristics of the model.
• Eigenvalue Extraction	Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal.
• Dynamic Reduction	Calls up the Dynamic Reduction Parameters form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Nonlinear Transient

This subordinate form appears when Solution Parameters is selected on the Solution Type form when Nonlinear Transient is selected. Use this form to generate either a SOL 99 or a SOL 129 input file, depending on the version of MD Nastran indicated on the translation parameter form except as indicated below. Version 66 and below yields SOL 99 and Version 67 and above yields SOL 129.

This is a list of data input available for defining the Nonlinear Transient Solution Parameters that was not shown on the previous page.


Parameter Name	Description
Plate Rz Stiffness Factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Struct. Damping Coeff.	Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor W4, Damping Factor	Define W3 and W4 parameters. These parameters alter the damping characteristics of the model.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Implicit Nonlinear

This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Implicit Nonlinear is selected. Use this form to generate a SOL 400 or 600 input file.


Solver / Options...	See Solver Options Subform (SOL 600), 297.
Contact Parameters...	See Contact Parameters Subform, 299.
Direct Text Input...	This subform is used to directly enter entries in the File Management, Executive Control, Case Control, and Bulk Data sections of the MD Nastran input file. See Direct Text Input, 266.
Restart Parameters...	See Restart Parameters Subform, 307.
Advanced Job Control...	See Advanced Job Control Subform (SOL 600), 309.
Domain Decomposition...	See Domain Decomposition, 310.
Assumed Strain	For SOL 600, if ON, (default is ON), places the MARCASUM parameter into the input file. This forces all elements that can deal with assumed strain to use this formulation. This improves the bending behavior of Marc elements 3, 7, and 11. For SOL 400, the NLMOPTS entry is written with the ASSUM option. Again, this is a global setting and forces all elements that can use this formulation to adopt it.
Constant Dilatation	If ON, (default is OFF), places the MARCDILT parameter into the input file. This will force all elements that can deal with constant dilatation (for nearly incompressible analysis) to use this formulation. This affects Marc element types 7, 10, 11, 19, and 20 only and recommended for elastic-plastic and creep analysis. (SOL 600 only)
Plane Stress	Replaces plane strain elements with plane stress elements. (SOL 600 only)
Reduced Integration	Specifies that a lower number of element integration points be used to integrate exactly. (SOL 600 only)
Creep	For SOL 400, writes the NLMOPTS entry with the CREEP option defaults for creep analysis.
Shell Shear Correction	For SOL 400 (only), forces all shell elements using nonlinear formulations to use the shear correction. This writes the NLMOPTS entry with the TSHEAR option.
SOL 400 Run	Use this to select a SOL 400 simulation, instead of a SOL 600 simulation.
Default Initial or Load Temperature	For SOL 400 allows for specification of a general initial temperature and a general loading temperature. TEMPD entries are written for both with Case Control TEMPERATURE(INITIAL) and TEMPERATURE(LOAD) entries calling out the corresponding TEMPD entries in the bulk data.
Results Output Format...	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Solver Options Subform (SOL 600)

Specifies the solver to be used in numerically inverting the system matrix of linear equilibrium equations.


Inconsistent MPCs	There are three choices for dealing with problem MPCs, 1) Reorder (reorder the DOFs that are used to define the problem MPCs), 2) Continue (continue the analysis with no changes to the MPCs DOFs), or 3) Stop (stop the analysis).
Solver Type	Can be set to Direct Profile, Iterative Sparse, Direct Sparse, Hardware Sparse, Multifrontal Sparse (default) or External Sparse. For MD Nastran 2010 or higher, Pardizo Direct Sparse and MUMPS Parallel Direct solvers are also supported.
Non-Symmetric	Specifies non-symmetric solution for Solver Types: Direct Profile, Multifrontal Sparse,or Pardizo Direct Sparse.
Non-Positive Definite	Turn this menu to ON to specify non-positive definite option. Valid for all solver types. Non Positive Definite is ON by default fo SOL 600. It is recommended to leave this menu set to Nastran Default. You may deselect this option by setting to OFF.
Memory	Defines the amount of work space in words. This can be left blank and the translator will automatically determine this based on model size.
Multifrontal Sparse Parameters
• Out-of-Core Threshold	For Hardware and Multifrontal Sparse solvers only. Default is 100. Represents the number of real*4 words in millions of words. Only for SGI computers running the IRIX operating system.
Bandwidth Optimization	Turns on the optimize option for the Direct Profile or Multifrontal Sparse solvers and uses the Sloan algorithm. Other solvers have their own optimizer and use it by default.
Number of Processes	Multiple treads can be specified for Pardiso(11) and Multifrontal (8) sparse solvers. The subsequent MD Nastran job is submitted with the MRTHREAD parameter set accordingly. Multiple processors can be specified for MUMPS(12) solver. The subsequent MD Nastran job is submitted with the MUMPSOLV parameter set accordingly. For DDM, by default the number of processes is set to the number of domains automatically. It can be manually changed if necessary.

Contact Parameters Subform

Defines options for detecting and handling contact.


Deformable-Deformable Method	In Double-Sided method, for each contact body pair, nodes of both bodies will be checked for contact. In Single-Sided method, for each contact body pair, only nodes of the lower-numbered body will be checked for contact. Results are dependent upon the order in which contact bodies are defined.
Optimize Constraint Equations	Use this to decrease the bandwidth of the model.
Contact Detection...	See Contact Detection Subform, 301.
Separation...	See Separation Subform, 303.
Friction Parameters...	See Friction Parameters Subform, 304.
Enable Initial Contact	Click on checkbox to activate the capability for control of initial contact. The initial contact is for creating an MD Nastran entry BCTABLE with ID = 0 to be used for increment 0. For SOL 600, this causes rigid contact bodies to be moved so they just touch adjacent flexible contact bodies. For SOL 101 and 400, a BCTABLE is used with ID = 0, which causes rigid contact bodies to be moved, as for SOL 600, and/or adjusting the coordinates of all active nodes on the surface of all deformable BCBODYs to remove any prestressed condition.
Initial Contact...	See Initial Contact Subform, 306.
Penetration Check	This controls contact penetration checking, sometimes referred to as the increment splitting option. Available options are: At End of Increment, Per Iteration (default), Suppressed (Fixed), Suppressed (Adaptive). At End of Increment means penetration is checked at the end of a load increment. Per Iteration means that penetration is checked at the end of every iteration within an increment. If penetration is detected, increments are split. Suppress is to suppress this feature for Fixed and Adaptive load stepping types.
Reduce Printout of Surface Definition	This controls reduction of printout of surface definition.

Contact Detection Subform

On the Contact Control Parameters subform, select Contact Detection... This form controls general contact parameters for contact detection.


Distance Tolerance	Distance below which a node is considered touching a body (error). Leave the box blank to have MSC.Marc calculate the tolerance as the smaller of 1/20 element edge length or 1/4 shell thickness.
Bias on Distance Tolerance	Contact tolerance BIAS factor. The value should be within the range of zero to one. Models with shell elements seem to be sensitive to this parameter. You may need to experiment with this value if you have shell element models that will not converge. The SOL 600 default is 0.9.
Suppress Bounding Box Check	Turn ON this button if you want to suppress bounding box checking. This might eliminate penetration, but slows down the solution.
Include Outside (Solid Element)	When detecting contact of elements (beam/bar, shell, solid elements) use this to include contact of the outside of the elements. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid).
Include Outside (Rigid Surface)	When detecting contact of rigid surfaces use this to include contact of the edges of the surfaces. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid).
Check Layers	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	Use this to detect contact of edges. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid).
Activate Quadratic Contact	Use this to detect the contact of the edges of quadratic elements (midside nodes).
Activate 3D Beam-Beam Contact	Turn this button ON to activate 3D beam-beam contact. Activate 3D Beam-Beam Contact enters a one(1) in the 13th field of the 2nd data block. This creates the MD Nastran Bulk Data entry BCPARA, and uses the entry BEAMP.

Separation Subform

On the Contact Control Parameters subform, select Separation... This form controls general contact parameters for contact separation.


Maximum Separations	Maximum number of separations allowed in each increment. Maximum Separations is entered in the 6th field of the 2nd data block. Default is 9999.
Retain Value on NCYCLE	Turn ON this button if you do not want to reset NCYCLE to zero when separation occurs. This speeds up the solution, but might result in instabilities. You can not set this and Suppress Bounding Box simultaneously. Retain Value of NCYCLE enters a three(3) in field 8 of the 2nd data block.
Increment	Specifies whether chattering is allowed or not. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
Chattering	Specifies the separation criterion (forces or stresses) and the critical value at which the separation will take place. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
Separation Criterion	Specifies in which increment (current or next) the separation is allowed to occur. Separation Criterion enters a one(1) in the 12th field of the 2nd data block if separation is based on stresses.
Force Value Stress Value	Force/Stress Value is placed in the 5th field of the 3rd data block.

Friction Parameters Subform

On the Contact Control Parameters subform, select Friction Parameters...


Friction Type	Available options for friction Type are: None (default), Shear (for metal forming), Coulomb (for normal contact), Shear for Rolling, Coulomb for Rolling, Stick-Slip, Bilinear Shear, and Bilinear Coulomb. The MD Nastran entry BCPARA is written to the .bdf file, with FTYPE used. Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction. Stick-Slip is a Coulomb type friction.
Method	For Coulomb type of friction models (options 2, 4, and 5 above), there are 2 methods for computing friction: Nodal Stress, Nodal Force (default). Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction.
Relative Sliding Velocity	Critical value for sliding velocity below which surfaces will be simulated as sticking. Relative Sliding Velocity is placed in the 1st field of the 3rd data block for all friction models except Stick-Slip.
Transition Region	Slip-to-Stick transition region. Transition Region is placed in the 1st field of the 3rd data block for Stick-Slip model.
Multiplier to Friction Coefficient	Friction coefficient multiplier. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Friction Force Tolerance	Friction Force Tolerance. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Heat Generation Conversion Factor	A factor related to how much heat is generated by the friction process.

Initial Contact Subform

On the Contact Control Parameters subform, select Initial Contact...

Restart Parameters Subform

Includes a Restart option in the MD Nastran input file. Restarts are only supported for SOL 600 in the current release.


Restart Type	You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File	If when restarting a job, you wish the results form the previous run to be copied into the new POST file, then turn this ON. This will place the RESTART or RESTART LAST options before the POST option in the input file. Otherwise they are placed after the POST option which flags MSC.Marc not to copy the results to the new POST file. If you turn this ON, you must have a restarname.t16 and/or restartname.t19 file in your local directory or the MSC.Marc analysis will fail.
Last Converged Increment	Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto	OFF by default. This places a REAUTO option in the input file. Any additional data needed for the REAUTO option are extracted from the first Load Step information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user.
Restart from Increment	Defines the increment to be read from the file specified in the Select Restart File form. This is entered in the 3rd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing	Defines the number of increments between writing data to the restart file. This is entered in the 2nd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Write or Read and Write. When Last Converted Increment is ON, this is the 4th field of the 2nd data block of the RESTART LAST option.
Select Restart File...	This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write. This file is specified on the command line for invoking the MSC.Marc solver using the -r option.

Advanced Job Control Subform (SOL 600)

Sets alternate versions of the solver and alternate formats for the results file, for SOL 600 jobs.


Marc Version	Specifies the version of MSC.Marc to run the analysis.
Marc Results File Format	Specifies the file format for the output from the analysis.
Marc Results File Type	Defines the binary output and/or text format of output from the analysis. Binary is recommended since .t16 files are linarily compatible across platforms and take up less space.
Marc scratch files w/ Nastran’s
Use Environment Variables	Use to enable the use of environment variables.
Suppress Non-SOLMARC Errors	Suppress errors that are not SOL 600 errors.
Submit Marc Job	Submit SOL 600 jobs to Marc.
Use Marc License	Use this to search for, then use Marc licenses.
Copy Marc Files	Make copies of Marc files; for example copy .t16 file.
Filter Marc Text
Delete Marc Files	Delete Marc files after the corresponding Patran files are created.
Gradually Release Constraints
Analysis Control Defaults	Creates the Nastran Bulk Data entry PARAM, MARCDEF. Its three values are Nastran Development (recommended by Nastran development; Marc SHELL_SECT parameter is set to 11), Marc-Mentat (current Marc standard), Marc Development (recommended by both Marc and Nastran development).
Marc Submit Command	Locates the submit command to run the MSC.Marc analysis (optional). For Specify Full Command its list box will be un-ghosted.

Domain Decomposition

Domain Decomposition is used to partition the model into seperate parts (domains) for parallel processing. The Method used to do this is named Domain Decomposition Method (DDM). This form designates that domain decomposition be done manually, semi-automatically, or automatically, for either SOL 400 or SOL 600 jobs.


Decomposition Method	Set this to Automatic if you wish MD Nastran to automatically create the domains during analysis run time. Set to Semi-Automatic if you wish to have MSC.Patran automatically break the model into domains which can be visualized before submittal. Set to Manual to have full control over the domains. This requires the creation of the groups before they can be selected here in this form and associated to a domain.
Number of Domains	This determines how many domains are to be created. When you change this number and press the Enter or Return key, the spread sheet updates with this number of rows. The default is 1. This corresponds to the number of CPUs desired to run the job. For the Automatic method, this is the only input that is required and the spreadsheet is not visible.
Model or Current Group	This is for choosing a part of the model to decompose for parallel processing: Model -- decompose all of the model, Current Group -- decompose just the current group. This choice must be consistent with what part of the model is specified for analysis (Analysis: Analyze / Entire Model or Selected Group). This is only active if Decomposition Method is set to Automatic or Semi-Automatic.
Metis Method	There are three Methods that can be used to partition the Model or Current Group into Domains. They are, 1) Nodal Position, 2) Element Topology, or 3) Best (a procedure that accounts for the best of the nodal, element, or vector type algorithms). This method can only be used if Decomposition Method is set to Automatic.
Domain Island Removal	Using this option causes some parts of disjoint domains (domain islands) to be combined with adjacent domains. This can only be used if Decomposition Method is set to Automatic.
Coarse Graph	Using this option sometimes produces domain islands (disjoint domains). This option (the default) is recommended to reduce the time to decompose the initial global domain. Use this only if there is a definite need for a better decomposition. This can only be used if Decomposition Method is set to Automatic.
Single POST File	If more than one CPU processor is used to solve the problem, the seperate/multiple results files can be compiled into a single file for postprocessing using Single POST File.
Create	Click Create to create Domain Information spreadsheet rows. After doing this the number of rows will equal the value of Number of Domains in the form. If Decomposition Method is set to Manual, the previously created group names will be selectable in Select a Group window at the bottom.
Visualize	This is used to display groups. Select a group name for the heading Domain Information under Group. Click Visualize to display just that group. This can be done for some or all of the groups.
Reset Graphics	Click Reset Graphics to reset the viewport graphics.
Validate	This is for validating (checking) that the domains are not disjoint. For two adjacent domains, the nodes at the interface of the domains must be in both domains.
Domain Information	The window with the definition of each Domain. For a given Domain there is a corresponding unique Group name.

DDAM

DDAM is an acronym for Dynamic Design Analysis Method, or DDAM is a methodology for analyzing ship-mounted equipment that the US Navy uses in the event of a near-miss underwater. Most FEA products follow the DDAM methodology, as does any hand calculation. MSC has made several improvements to its products that make DDAM easier to use.

To accommodate the special spectrum and summing conventions MSC made several modifications to MD Nastran. A DMAP alter in MD Nastran puts out data important for a DDAM analysis. A stand-alone Fortran program reads the MD Nastran data, calculates the spectral data, formats DDAM run information, and sends data back to MD Nastran for further postprocessing.

MSC’s DDAM has the following capabilities.

• Calculates all three shock directions simultaneously.

• Automatically calculates the appropriate spectra from input of the coefficients.

• Performs the NRL sum.

• Contains modal selection following 3010 Rev 1 convention.

• Provides manual mode selection if needed.

• Provides mode-by-mode output if desired.

• Uses all available MD Nastran elements.

• Provides NRL summed output in MD Nastran OP2 format for use with most postprocessors.

• Offers an alternate coefficient input method is available that avoids using the Fortran program, but the classified coefficients must be entered directly in the data file.

• Has unlimited model size.

• Uses MSC’s Lanczos Eigenvalue solver for fast solutions.

DDAM has the following limitations.

• All base input points must be rigidly connected to a single grid flagged on a SUPORT entry.

• There is no easy method to handle closely spaced modes as defined by 3010.

• MD Nastran printed output (.f06 file) is not labeled well, and must be used carefully in order to avoid mistakes. This is especially true of the mode-by-mode output.

• A DDAM data file will not read into Patran/MSC.FEA completely.

• .XDB output not available for NRL summed quantities

• MD Nastran requires additional input switch to be toggled in Patran in order to plot NRL summed von Mises and combined beam stresses.

• MD Nastran does not calculate beam and bar shear stresses. They are not included in the von Mises and combined stresses reported by MD Nastran DDAM.

DDAM in Patran

DDAM in MD Nastran is a process that involves three main parts, and a number of smaller parts. The entire procedure is accessed from a simple interface in Patran that integrates the process.

• Part 1, Modal Analysis - A modal analysis is run in MD Nastran. This supplies the frequencies, mode shapes and modal participation for the model.

• Part 2, Spectrum Generation – Using the output from Part 1, you can use a Fortran program to calculate the shock spectrum. This is based on the DDS-072 or NRL 1396 documents, or you can manually enter your own spectrum.

• Part 3, Spectrum Application and Data Recovery – The calculated spectrum from Part 2 is applied to the mode shapes calculated in Part 1, and the results are calculated on a mode-by-mode basis. The results from this are then summed using an NRL sum to produce results, one set for each shock direction.

The Patran interface presents you with a selection of options to calculate the spectrum and sum the results. The options are stored, and when the MD Nastran modal analysis completes, the Fortran program automatically starts, using the stored options to drive it. MD Nastran automatically resumes after the completion of the Fortran program and finishes the analysis.

During is process, a number of files will be created that are inputs and outputs from this process, all named jobname.xxx using the jobname chosen in Patran. The most important files are:

jobname.ddd – the DDAM potions file that drives the Fortran program

jobname.f11 – the modal information needed to calculate the spectrum

jobname.f13 – the calculated spectra information for input back into MD Nastran

jobname.ver – modal verification file

jobname.opw – Nastran OP2 file with the mode shapes

jobname.opx – Nastran op2 file with the NRL summed results for x-shock

jobname.opy – Nastran op2 file with the NRL summed results for y-shock

jobname.opz – Nastran op2 file with the NRL summed results for z-shock

Once the run is complete, you can look over both the results and the modal verification file. If the results are not as expected or desired, there are a number of more advanced capabilities of this DDAM procedure for more control over the process. These include some that are on the Patran forms (changes in 80% criterion, minimum G value) and ones that can be accessed using the Patran Direct Text capability (mode-by-mode output, specific mode selection).

DDAM Model Preparation

In order to run DDAM, all of the fixed base points (excitation inputs) in the model must be rigidly connected to a single point. The MD Nastran RBE2 element is used for this, connecting the independent node (the SUPORT point) to all of the other fixed base/excitation points (dependent grids) in all 6 degrees of freedom. This point is flagged for the SUPORT entry in the DDAM setup. It is not necessary that this point is separated (spatially) from the other input points, you can select one of the base points to be the SUPORT point, as long as all the excitation points are then connected to it. It is not advisable to have any other translational constraints in the model, as they will remove modal mass from the model and the 80% criterion will not necessarily be correct, and the model will have base points that will not be excited. You may have rotational constraints to hold shafting and to remove plate and bar singularities, as the rotational components are not used in the DDAM excitation.

No loads or other boundary conditions are needed for the analysis. As per 3010, you need to add operating loads to the shock loads at the conclusion of the analysis. Set up the model like any other modal analysis, with the exception of the SUPORT point. Mass and material density are required to obtain correct mode shapes. The modal analysis parameters are set up on the Subcase Options form, where you can select the number of desired modes, the lower frequency bound, and an upper frequency bound. The analysis uses a Lanczos extraction routine with mass normalization, and uses the default Lanczos debugging information level. You will not have control over these parameters in DDAM.

DDAM Solution Parameters

This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when DDAM is selected. Use this form to generate a SOL 187 input file.


Automatic Constraints	Indicates that an AUTOSPC entry is requested. MD Nastran will automatically constrain model singularities.
Shell Normal Tol. Angle	Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
• Lumped	Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
• Coupled
Data Deck Echo
• None	Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
• Sorted
• Unsorted
Plate Rz Stiffness factor	Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node id for Wt. Gener	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Initial Temperature	Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature	Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry.
SUPPORT Node	Selects the point you have chosen for your base input. Note that this is a required choice with no default, and that you can only pick one node. If multiple nodes are entered in the data box, only the first one is used.
Results Output Format	On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 340.

Explicit Nonlinear

This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Explicit Nonlinear is selected under Preferences: Analysis... . Use this form to generate a SOL 700 input file.


Parameter Name	Description
Large Displacements	Use this to cause the large displacement formulation to be used.
Follower Forces	Use this to cause the forces to move (translate and rotate) with the model.
Prestress Option	Use this to cause the pre-stresses to be calculated.
Maximum Printed Lines	Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time	Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion	Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.	Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
SOL 700 Default Settings	Either Dytran or Ls-Dyna default settings can be used.
• Sol700 Parameters...	Displays the Sol700 Parameters and Extra Data form that is used for specifing parameter values for such things as execution control, dynamic relaxation (entry DAMPGBL), general parameters, contact, and Eulerian parameters. See Sol700 Parameters Subform, 319
• Resultts Output Format...	Use this to specify the types of files that are to be written for the SOL 700 analysis. For example, XDB (jobname.xdb) and Print (jobname.f06).See Results Output Format, 340

Sol700 Parameters Subform

This subordinate form appears when Sol700 Parameters button is selected on the Solution Parameters form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Execution Control Parameters...	DYSTATIC, DYBLDTIM, DYINISTEP, DYTSTEPERODE, DYMINSTEP, DYMAXSTEP, DYSTEPFCTL, DYTERMNENDMAS, DYTSTEPDT2MS
Dynamic Relaxation...	This is for specifying the entries for the DAMPGBL Bulk Data entry. This is for defining parameter values for static analysis using dynamic relaxation for SOL 700 only.
General Parameters...	DYLDKND, DYCOWPRD, DYCOWPRP, DYBULKL, DYHRGIHQ, DYRGQH, DYENERGYHGEN, DYSHELLFORM, DYSHTHICK, DYSHNIP
Contact Parameters...	DYCONSLSFAC, DYCONRWPNAL, DYCONPENOPT, DYCONTHKCHG, DYCONENMASS, DYCONECDT, DYCONIGNORE, DYCONSKIPTWG
Binary Output Database File Parameters...	DYBEAMIP, DYMAXINT, DYNEIPS, DYNINTSL, DYNEIPH, DYSTRFLG, DYSIGFLG, DYEPSFLG, DYRLTFLG, DYENGFLG, DYCMPFLG, DYIEVERP, DYDCOMP, DYSHGE, DYSTSSZ, DYN3THDT
Time History Output Request...	This is for specifying the type of output file (Binary, ASCII, Both), and the Output Time Interval.
Hourglass Setting...	See Hourglass Setting Subform, 321
Merge Rigid Mat...	See Merge Rigid Material Subform, 323
Dynamic Relaxation for Restart...	See Dynamic Relaxation for Restart Subform, 325
Damping Per Property...	See Damping Per Property Subform, 327
Rigid Body Switch and Merge...	See Rigid Body Switch and Merge Subform, 329
Eulerian Parameters...	See Eulerian Parameters Subform, 335
SPH Control Parameters...	See SPH Control Parameters Subform, 338

Hourglass Setting Subform

This subordinate form appears when Hourglass Setting button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Existing Hourglass Setting	List of previously created hourglass settings.
Hourglass Name	Specify the name.
Property Type	Specify either a Shell (2D) or Solid (3D) element type.
Control Type	Choose one of several types of controlling the hourglass effects. The choices are: 1) Standard LSDyna Viscous (Property Type = Shell or Solid), 2) Flanagan-Belytschko Viscous (Property Type = Shell or Solid), 3) Flan-Bely. Visc. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 4) Flanagan-Belytschko Stiffness (Property Type = Shell or Solid), 5) Flan-Bely. Stiff. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 6) Flanagan-Bindeman Stiffness (Property Type = Solid), 7) Fully Integrated Shell (Property Type = Shell). These entries are defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Hourglass Coefficient	This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Warping Hourglass Coeff.	This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Bending Hourglass Coeff.	This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Linear Bulk Visc. Coeff.	This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Quadr. Bulk Visc. Coeff.	This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Select Property Set	Select a previously created element property. For example, Properties > Create > 2D > Shell > Options: Explicit PSHELL1 > Input Properties... > Shell Formulations > HUGHES.
Add	Click Add after input all necessary data into the Hourglass Setting form to create an Existing Hourglass Setting.
Modify	Click Modify after input all changed data into the Hourglass Setting form to update an Existing Hourglass Setting. You must first select the particular Existing Hourglass Setting.

Merge Rigid Material Subform

This subordinate form appears when Merge Rigid Mat button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Existing Merged Materials	List of previously merged MATRIG materials. MATRIG is an MD Nastran Bulk Data entry for defining rigid body properties.
Merged Material Name	Specify the name of merged material to be created.
Select Material to be Merged into	Specify the name of an MATRIG material to merge other MATRIG materials into.
Select Materials to be Merged	Specify the names of MATRIG materials that are to be merged into the merged material whos name is specified under Merged Material Name.
Add	Click Add after input all necessary data into the Rigid Materials form to create an Existing Merged Materials.
Modify	Click Modify after input all changed data into the Rigid Materials form to update an Existing Merged Materials. You must first select the particular Existing Merged Materials.

Dynamic Relaxation for Restart Subform

This subordinate form appears when Dynamic Relaxation for Restart button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Relaxation	Use this to not use (None Active) or use (Activated Relaxation) relaxation in performing the simulation.
[Termination Time]	The time to stop the simulation. This is optional ([ ]).
Convergence Tolerance	Specify convergence tolerance.
Number of Iterations	Specify the maximum number of iterations.
Papadrakakis Auto Control	Click the checkbox to specify that convergence control is to be automatic using the Papadrakakis method.
Papadrakakis Convergence Tolerance	To use this it is necessary to not select Papadrakakis Auto Control.
Relaxation Factor	Specify the value of the Relaxation Factor.
Time step scale Factor	Specify the value of the Time step scale Factor.

Damping Per Property Subform

This subordinate form appears when Damping Per Property button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Damping Type	Select either Property (use property) or Stiffness (use Rayleigh damping).
System Damping Constant Table	Select a time dependent field under Time Dependent Field. This field will be multiplied by the Scalar Factor for Load Curve entry. The (X,Y,Z) Trans. Damping Forces and (X,Y,Z) Rot. Damping Moments entries (all of these form a 6 component load vector) are multiplied by the scaled time dependent field.
Time Dependent Field	Select a Field, with it being entered into the System Damping Constant Table list box. For example, select the field named damping_vs_time under Time Dependent Field. For System Damping Constant Table f:damping_vs_time appears.
Scale Factor for Load Curve	Specify the scale factor that will multiply the Time Dependent Field specified under System Damping Constant Table.
X Trans. Damping Forces	Scale factor for X translation damping forces, in the global coordinate system directions.
Y Trans. Damping Forces	Scale factor for Y translation damping forces, in the global coordinate system directions.
Z Trans. Damping Forces	Scale factor for Z translation damping forces, in the global coordinate system directions.
X Rot. Damping Moments	Scale factor for X rotation damping moments, in the global coordinate system directions.
Y Rot. Damping Moments	Scale factor for Y rotation damping moments, in the global coordinate system directions.
Z Rot. Damping Moments	Scale factor for Z rotation damping moments, in the global coordinate system directions.
Rayleigh Damping Coeff.	Specify the scalar coefficient (β) that the global stiffness matrix is multiplied by to obtain the Rayleigh damping matrix.

Rigid Body Switch and Merge Subform

This subordinate form appears when Rigid Body Switch and Merge button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Option	Only option is At Start (D2R0000).
Existing Merged Properties	List of deformable body and rigid body properties that have already been merged.
Merged Body Name	Specify the name of the Existing Merged Properties entry to be created.
Deformable Property	Select an entry under Deformable Property
Master Rigid Property	Select an entry under Master Rigid Property
Add	Click Add to create an entry under Existing Merged Properties.
Modify	Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Define Set of Parts to be Switched	See Define Set of Parts to be Switched Subform, 332
Define Inertial Properties of Rigid Body	See Define Inertial Properties of Rigid Body Subform, 334

Define Set of Parts to be Switched Subform

This subordinate form appears when Define Set of Parts to be Switched button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient.

The supported parameters are shown in the following table:


Form	Parameters
Option	Only option is At Stage (D2RAUTO).
Existing Merged Properties	List of deformable body and rigid body properties that have already been merged.
Merged Body Name	Specify the name of the Existing Merged Properties entry to be created.
Deformable Property	Select an entry under Deformable Property.
Master Rigid Property	Select an entry under Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
Add	Click Add to create an entry under Existing Merged Properties.
Modify	Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Starting Switch Time	Specify the time to switch the deformable and rigid properties.
Ending Switch Time	Specify the time to terminate the switching of the deformable and rigid properties.
Delay Period	Specify the time delay (τ) for switching.
Rigid Wall/Contact Surf Number	Specify the surface numbers for rigid walls/surfaces that are to contact.
Related Switch Set
Max. Permited Time Step Size	Specify the maximum time step.
Number of Deformable Parts to Rigid	Specify the number of deformable parts that will be switched to rigid parts.
Number of Rigid Parts to Deformable	Specify the number of rigid parts that will be switched to deformable parts.
Activation Code Switch	Select one of the five flags, 1) EQ.0, 2) EQ.1, 3) EQ.2, 4) EQ.3, or 5) EQ.4.
Pair of Related Switches	Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.-1.
Nodal Rigid Body Activation Flag	Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Nodal Constraint Activation Flag	Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Rigid Wall Activation Flag	Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.

Define Inertial Properties of Rigid Body Subform

This subordinate form appears when Define Inertial Properties of Rigid Body button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Option	Only option is New Rigid Props. (D2RINNER).
Master Rigid Property	Select a Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
X Coord of Center of Mass	X coordinate of center of mass.
Y Coord of Center of Mass	Y coordinate of center of mass.
Z Coord of Center of Mass	Z coordinate of center of mass.
Translational Mass	Scalar mass value for translation, not rotation.
XX Comp. of Inertia Tensor (IXX)	XX (1,1) component of inertia tensor matrix.
XY Comp. of Inertia Tensor (IXY)	XY (1,2) component of inertia tensor matrix.
XZComp. of Inertia Tensor (IXZ)	XZ (1,3) component of inertia tensor matrix.
YY Comp. of Inertia Tensor (IYY)	YY (2,2) component of inertia tensor matrix.
YZ Comp. of Inertia Tensor (IYZ)	YZ (2,3) component of inertia tensor matrix.
ZZ Comp. of Inertia Tensor (IZZ)	ZZ (3,3) component of inertia tensor matrix.

Eulerian Parameters Subform

This subordinate form appears when Eulerian Parameters button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Euler Boundary Treatment	There are three choices, 1) Default, 2) Extrapolate (extrapolate structural mesh pressure to Euler elements at solid/fluid boundary), or 3) Element (solid/fluid boundary Euler element pressure equals the structural element pressure at the solid/fluid boundary).
Multi-Mat. Trans. Scheme	There are three choices, 1) Default (Impulse), 2) Average (face (surface) velocity is averaged simply), or 3) Impulse (face (surface) velocity is impulse weighted).
Material Failure Option	There are three choices, 1) Default (No Fail), 2) Fail (activates transport of fail fraction and thereby keeps track of material that has failed), or 3) No Fail (failed Euler material can support shear stress again as soon as new material enters the Euler element).
Multi-Material Array Size	The multi-material Eulerian elements use an overflow array to store their material data. This array can hold “Multi-Material Array Size” times the number of Eulerian elements. If more the 10% of the Eulerian elements have more than one material, the value of “Multi-Material Array Size” must be increased.
Initial Condition Accuracy	A parameter value used to specify the accuracy of the initial conditions in Eulerian elements, when using the geometric shape definition. The parameter value is specified in the input file using PARAM, MICRO, value.
Mimimum Velocity	A parameter value used to specify the minimum velocity. If a calculated velocity is less than this, it is set to zero (0). It is mainly used to eliminate harmless small values. The parameter value is specified in the input file using PARAM, VELCUT, value.
Maximum Velocity	Specify the maximum velocity for Eulerian and Lagrangian meshes. Although it is not usually necessary to limit the velocity in Eulerian meshes, there are occasions in regions of near-vacuous flow where using this can be an advantage. The same thing applies to Lagrangian meshes, where there is contact. The parameter value is specified in the input file using PARAM, VELMAX, value, YES/NO. Default is 1.0e10, YES. See the next row for information on what YES/NO means.
Small Mass Removal	Because very high velocities occur mostly in Eulerian elements with very small mass, the mass in these elements may need to be removed for the analysis to be stable. The above parameter (PARAM, VELMAX) is used to specify whether or not to eliminate small masses. YES = eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. NO = do not eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. Default = YES.
Universal Gas Constant	Specify the value of the universal gas constant. The parameter value is specified in the input file using PARAM, UGASC, value.
Single Material Elements	Specify the minimum density of single material Eulerian elements. For arbitrary Lagrange-Euler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Single Mats. with Strength	Specify the minimum density of single material Eulerian elements with strength. For arbitrary Lagrange-Euler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Multi-Material Elements	Specify the minimum density of multi-material Eulerian elements.
Roe Solver Scheme	Specify whether or not to use the Roe solver. The Roe solver accounts for momentum exchange between Lagrange (structure) and Eulerian material.
Spatial Accuracy	There are two schemes that can be used. They are, 1) 1st Order (left and right state variables are taken as the values the state variables have at the left- and the right-element center), or 2) 2nd Order (left- and right-state variable values at a face by including the left-left and the right-right element).
Time Integration Scheme	There are two schemes that can be used. They are, 1) 1st Order, or 2) 2nd Order (three-stage time integration scheme).

SPH Control Parameters Subform

This subordinate form appears when SPH Control Parameters (SPH refers to smooth “particle hydrodynamics”) button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:

• SOL700,101 - Linear Static

• SOL700,106 - NonLinear Static

• SOL700,109 - Direct Transient Response

• SOL700,129 - NonLinear Transient

The supported parameters are shown in the following table:


Form	Parameters
Number of Cycles	Specify the number of cycles between particle sorting.
Death Time	Specify the time when SPH calculations are to be stopped.
Initial Number of Neighbors	Specify the initial number of neighbors per particle. This parameter is for specifying how much memory is to be allocated for arrays during initialization. If the value is positive, the memory will be dynamically allocated. If the value is negative, the memory allocation will be static (constant). During the calculation only the closest SPH elements will be considered as neighbors. Using this option can avoid memory allocation problems.
Particle Approx. Theory	There are six theories to choose from, 1) Renormalization (approximation), 2) Symmetric (formulation), 3) Sym. Renormalization (symmetric renormalization approximation), 4) Tensor (tensor formulation), 5) Fluid Particle (fluid particle approximation), 6) Fluid Particle Renorm (fluid particle with renormalization approximation).
Start Time	Specify the time to begin particle approximation.
Maximum Velocity	Maximum velocity for the SPH particles. Particles whos velocity > this value are deactivated.
Computation of Approx.	Select one of the following for two different SPH parts, 1) Particle Approximation (approximation is calculated), or 2) No Particle Approximation (approximation is not calculated; two different SPH materials cannot interact with each other, and penetration is allowed).
Intergration Type	Select 1) 0 (), or 2) 1 (), for time integrating to obtain the smoothing length.
Smoothing Length Comput.	Select 1) Bucket (sort based on algorithm; very fast), or 2) Global (computation for all the model particles ). This is done during initialization.
Box Type	Select either 1) Fixed (the box remains fixed in space), or 2) Moving (the user specifies two corners of the box and a the time dependent Field to describe the motion of the two corners). As long as a given SPH particle is in a box, the SPH calculation for the particle is performed for the box. If the particle leaves the box it was inside, it is deactivated.
Select Box	Select the name of a box under Select Box. A box must have been previously created under Loads/BCs: Create / Box Definition / Nodal.
Tail Vector	Specify a vector, <X1 Y1 Z1>, that defines the minimum coordinates of the box (coordinates of the corner of the box at the minimum location).
Head Vector	Specify a vector, <X2 Y2 Z2>, that defines the maximum coordinates of the box (coordinates of the corner of the box at the maximum location).
Motion Vs Time Data	Specify the time dependent Field that defines the motion of the two corners of the box.
Vel./Disp. Flag	Specify whether the time dependent Field is a Velocity or Displacement field.
Coord. System	Specify the coordinate system that the Tail and Head Vectors are defined in.

Results Output Format

With the results output format form you can choose which output formats you want to use with each solution sequence. The appropriate defaults are set for each solution type. These defaults can be changed or set in the settings.pcl file.


Data Output	Defines the type of data output.
• OP2	Specifies output of data to a MD Nastran OUTPUT2 file (*.op2). This will place a PARAM, POST, -1 in the input file.
• XDB	Specifies output of data to a MSC.Access database (*.xdb). This will place a PARAM, POST, 0 in the input file.
• Print	Specifies output of data to a MD Nastran print file (*.f06).
• Punch	Specifies output of data to a MD Nastran punch file (*.pch).
• MASTER Only	When ON, only a .master file is written.
• MASTER/DBALL	When ON, both a .master file and a .dball file are written.
• XDB Buffer Size	For the XDB results file, defines the buffer size used for accessing results.
OUTPUT2 Requests	Specifies type of OUTPUT2 commands. • P3 Built In - signals the use of MD Nastran internal OUTPUT2 commands geared toward Patran. These commands are also appropriate for PATRAN 2. The “P3 Built In” option is appropriate only for Database Runs, see Solution Parameters, 268. If Database Run has been deselected, this option will be set internally to “Alter File”. • Alter File - specifies the use of an external alter file found on the Patran file path and following the “msc_v#_sol#.alt” naming convention. See Files, 550 for more details.
	• CADA-X Alter - specifies the use of an LMS CADA‑X specific alter file that is identical to the “Alter File” but with an additional “.lms” extension, for example, “msc_v67_sol103.alt.lms”. • P2 Built In - specifies use of MD Nastran internal OUTPUT2 commands geared toward PATRAN 2.
OUTPUT2 Format	Specifies format of the MD Nastran OUTPUT2 (*.op2) files. Use “Text” format when the resulting OUTPUT2 file must be transported between heterogeneous computer platforms.

A new variable has been added to the settings.pcl file for results output format defaults per SOL sequence:

NASTRAN_nnn_DATA_OUTPUT OP2+PUNCH

Where nnn is the solution sequence 101, 400 etc... and OP2+XDB+PRINT+PUNCH+MASTER +DBALL are the options. This variable is only read from the settings.pcl file when opening a new database, creating a new job or changing the solution sequence of an existing job. Otherwise the results output settings are retrieved from the database for an existing job. Note that these variables must be added to the settings.pcl file by the user and if they do not exist, a standard default is used. Also note that OP2 and XDB are mutually exclusive and both cannot be specified at the same time. The same is true for MASTER Only and MASTER/DBALL. The settings.pcl file may have one of these variables for each SOL sequence defined in Patran (>100).

ADAMS Preparation

This form is used when you want to prepare a database for an Adams job.


ADAMS Output	• MNF Only • Full Run + MNF
Units	• Mass - Your options are: Kilogram, Pound-Mass, Slug, Gram, Ounce-Mass, Kilo-Pound-Mass, Megagram • Force - Newton, Pounds-Force, Ounce-Force, Dyne, Kilo-Newton, Kilo-Pound-Force • Length - Millimeter, Centimeter, Meter, Kilometer, Inch, Foot, Mile • Time - Millisecond, Second, Minute, Hour
Craig-Bampton Modes Bounds	• Lower Bound • Upper Bound
Num. Shapes to Adams
ADAMS Debug Print
Strip Face
Create .out(OP2 file) for MSC Fatigue
Mass Options	• Partial • Constant File • Full • None
Output Requests
Transfer Groups to ADAMS