MSC Nastran > Running an Analysis > 3.9 Output Requests
XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">   
3.9 Output Requests
This allows the definition of what data is desired from the analysis code in the form of results. For most solution sequences, the form consists of two formats: Basic and Advanced. The Basic form retains the simplicity of being able to specify the output requests over the entire model and uses the default settings of MD Nastran Case Control commands. There is a special set defined in Patran called ALL FEM. This set represents all nodes and elements associated with Object defined on the Analysis Form, 251. This default set is used for all output requests in the Basic Output Requests, 409 form.
The Advanced version of this form allows the user to vary these default options. Since output requests have to be appropriate to the type of analysis, the form changes depending on the solution sequence. The Advanced Output Requests, 410 also adds the capability of being able to associate a given output request to a subset of the model using Patran groups. This capability can be used effectively in significantly reducing the results that are created for a model, optimizing the sizes and translation times of output files. The creation of Patran groups are documented in Group>Create (p. 271) in the Patran Reference Manual.
The results types that will be brought into Patran due to any of these requests, are documented in Supported OUTPUT2 Result and Model Quantities, 480. In that chapter, tables are presented that correlate the MD Nastran results block, and the Patran primary and secondary results labels with the various output requests.
Note:  
Many of the output requests that can be defined on the Output Request forms currently apply only to the printed values in the MD Nastran output file; these result quantities cannot be imported and postprocessed in Patran. For guidance on specific quantities, review Supported OUTPUT2 Result and Model Quantities, 480.
MD Nastran Implicit Nonlinear (SOL 600) produces stress and strain results that differ from those results available with other solution sequences. A detailed discussion of the stress and strain measures for SOL 600 is given in Stress and Strain Measures for Nonlinear Analysis (Ch. 2) in the MSC.Nastran Implicit Nonlinear (SOL 600) User’s Guide.
Basic Output Requests
This form is used to select output requests with their default options. The set is always All FEM, which means results for all nodes or elements in the model. A default set of output requests is always preselected.
Advanced Output Requests
This form provides great flexibility in creating output requests. Output requests may be associated with different groups (SET options in MD Nastran) as well as different superelements1. The output requests available depend on the chosen Solution Types, 261, Solution Parameters, 268, and Translation Parameters, 255. The Advanced Output Requests form is sensitive to the Result Type selected. The Form Type, Delete, OK, Defaults, and Cancel buttons operate exactly like on the Basic Output Requests, 409 form.
A description of the output requests and their associated options are listed in Table 3‑1 and Table 3‑2. 
 
Table 3‑1
Output Request
Case Control Command or Bulk Data Entry
Description
Acoustic Intensity
INTENSITY
Requests acoustic intensity for external acoustics analysis (frequency response).
Acoustic Power
ACPOWER
Requests acoustic power radiated from surface for external acoustics analysis (frequency response).
Acoustic Field Point Mesh
ACFPMRESULT
Requests acoustic field point mesh results for external acoustics analysis (frequency response). You are given a list of all acoustic field point meshes defined and groups with nodes. Each one selected is translated into its own BEGIN AFPM section in the bulk data.
Acoustic Velocities
VELOCITY
Requests nodal velocities. This is for acoustic velocities at the node points of Field Point Mesh.
Displacements
DISPLACEMENT
Requests nodal displacements.
Eigenvectors
VECTOR
Requests nodal eigenvectors.
Element Stresses
STRESS
Requests elemental stresses.
Constraint Forces
SPCFORCES
Requests forces of single- point constraints.
MultiPoint Constraint Forces
MPCFORCES
Requests forces of multipoint constraints (for versions 68 or higher).
Element Forces
FORCE
Requests elemental forces.
Applied Loads
OLOAD
Requests equivalent nodal applied loads.
Nonlinear Applied Loads
NLLOAD
Requests equivalent nonlinear applied loads. Sorting and format options are not allowed with this request.
Element Strain Energies
ESE
Requests elemental strain energies and energy densities. No options are allowed with this output request.
Element Strains
STRAIN
Requests elemental strains.
Grid Point Stresses
GPSTRESS
Requests stresses at grid points.
Velocities
VELOCITY
Requests nodal velocities.
Accelerations
ACCELERATION
Requests nodal accelerations.
Grid Point Force Balance
GPFORCE
Requests grid point force balance at nodes. Sorting and format options are not allowed with this request.
Grid Point Stress Discontinuities
GPSDCON
Requests mesh stress discontinuities based on grid point stresses.
Element Stress Discontinuity
ELSDCON
Requests mesh stress discontinuities based on element stresses.
Nonlinear Stress
NLSTRESS
Requests the form and type of nonlinear element stress output.
Contact Results
BOUTPUT
Requests contact regions for output.
 
Table 3‑2
Options
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Sorting
By Node/
Element
SORT1
Elements
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/
Time
SORT2
Elements
No
Output is presented as tabular listing of frequency or time for each node or element.
Format
Rectangular
REAL
Elements
No
Requests real and imaginary format for complex output.
Polar
PHASE
Elements
No
Requests magnitude and phase format for complex output.
Tensor
Von Mises
VONMISES
Elements
No
Requests von Mises stresses or strains.
Maximum Shear
MAXS
Elements
No
Requests Maximum shear or Octahedral stresses or strains.
Element Points
Cubic
CUBIC
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach with cubic bending correction.
Corner
CORNER
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center.
Center
CENTER
Elements
No
Requests QUAD4 stresses or strains at the center only.
Strain Gage
SGAGE
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach.
Bilinear
BILIN
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using bilinear extrapolation.
Composite Plate Options
Element Stresses
NOCOMPS= -1, LSTRN = 0 in Bulk Data
Elements: Surfaces
No
Composite element ply stresses and failure indices are suppressed. Element stresses for the equivalent homogeneous element are output.
Ply Stresses
NOCOMPS=1,LSTRN = 0 in Bulk Data
Elements: Surfaces
No
Composite element ply stresses and failure indices are output. Model should contain PCOMP entry defining composites.
Composite Plate Options
Ply Strains
NOCOMPS=1,LSTRN = 1 in Bulk Data
Elements: Surfaces
No
Composite element ply strains and failure indices are output. Model should contain PCOMP entry defining composites.
Ply Element Stresses
NOCOMPS=0,LSTRN=0 in Bulk Data
Elements: Surfaces
No
Composite element ply stresses and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Element and Ply Strains
NOCOMPS=0,LSTRN=1 in Bulk Data
Elements: Surfaces
No
Composite element ply strains and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Plate Strain Options
Plane Curv.
STRCUR
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains and curvatures are output at the reference plane for plate elements.
 
Fiber
FIBER
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains at locations Z1 and Z2 (specified under element properties) are output at the reference plane for plate elements.
Sorting
By Node /Element
SORT1
Nodes
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/ Time
SORT2
Nodes
No
Output is presented as tabular listing of frequency or time for each node or element.
Format
Rectangular
REAL
Nodes
No
Requests real and imaginary format for complex output.
Polar
PHASE
Nodes
No
Requests magnitude and phase format for complex output.
Output Coordinate
Coord
COORD CID
Elements:
Surfaces, Volumes
Yes
Selects the output coordinate frame for grid point stress output. Coord 0 is the basic coordinate frame.
Volume Output
Both
Blank
Elements:Volumes
Yes
Requests direct stress, principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
Principal
PRINCIPAL
Elements:Volumes
Yes
Requests principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
Direct
DIRECT
Elements:Volumes
Yes
Requests direct stress, mean pressure stress and von Mises equivalent stresses to be output.
Fiber
All
FIBER, ALL
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at all fibre locations, that is at Z1, Z2 and the reference plane. Z1 and Z2 distances are specified as element properties (default Z1=-thickness/2, Z2= +thickness/2).
Fiber
Mid
FIBER, MID
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at the reference plane.
Z1
FIBER, Z1
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z1 from the reference plane (default Z1=-thickness/2).
Z2
FIBER, Z2
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z2 from the reference plane (default Z2=+thickness/2).
Normal
X1
NORMAL X1
Elements: Surfaces,
Yes
Specifies the x-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X2
NORMAL X2
Elements: Surfaces
Yes
Specifies the y-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X3
NORMAL X3
Elements: Surfaces
Yes
Specifies the z-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
Method
Topological
TOPOLOGI-CAL
Elements: Surfaces
Yes
Specifies the topological method for calculating average grid point stresses. This is the default.
Geometric
GEOMETRIC
Elements: Surfaces
Yes
Specifies the geometric interpolation method for calculating average grid point stresses. This method should be used when there are large differences in slope between adjacent elements.
X-axis of Basic Coord
X1
AXIS, X1
Elements: Surfaces
Yes
Specifies that the x-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X-axis of Basic Coord
X2
AXIS, X2
Elements: Surfaces
Yes
Specifies that the y-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X3
AXIS, X3
Elements: Surfaces
Yes
Specifies that the z-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
Branch
Break
BREAK
Elements: Surfaces
Yes
Treats multiple element intersections as stress discontinuities in the geometric interpolation method.
No Break
NOBREAK
Elements: Surfaces
Yes
Does not treat multiple element intersections as stress discontinuities in the geometric interpolation method.
Tolerance
0.0
TOL=0.0
Elements: Surfaces
Yes
Defines the tolerance to be used for interelement slope differences. Slopes beyond this tolerance will signify discontinuous stresses.
Percent of Step Output
100
NOi Field of TSTEP and TSTEPNL entry
All
Once per subcase
An integer ‘n’ that specifies the percentage of intermediate outputs to be presented for transient and nonlinear transient analyses.
Adaptive Cycle Output Interval
0
BY = n on OUTPUT Bulk Data entry
p-elements
Once per subcase
An integer ‘n’ that requests intermediate outputs for each nth adaptive cycle. For n=0, only the last adaptive cycle results are output. This is available for SOLs 101 and 103 for versions 68 and higher.
Intermediate Output Options
Yes
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed load increment. Applicable for nonlinear static solution type only.
No
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for the last load of the subcase. Applicable for nonlinear static solution type only.
All
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed and user-specified load increment. Applicable for nonlinear static solution type only.
Suppress Print for Result Type
N/A
Specifies PLOT option instead of PRINT on the Case Control Output request entry.
All
Yes
Print to the .f06 file is suppressed for the result type when this is selected.
Output Device Options
Print
Specifies PRINT on a Case Control request entry, e.g. DISPL.
All
Yes
The printer will be the output medium for the .f06 file.
Punch
Specifies PUNCH on a Case Control request entry, e.g. DISPL.
All
Yes
The punch file will be the output medium.
Both
Specifies both PRINT and PUNCH.
All
Yes
The printer and punch file will be the output medium.
Edit Output Requests Form
Use this form to edit the outputs request associated with selected subcases. To access this form, select the Output Requests button on the Subcases form with the Action set to Global Data.
Notes:
• The Edit Output Requests form opens with focus in the first result type of the first subcase.
• The top half of the Edit Output Requests form is similar to the Advanced Output Request form.
• The spreadsheet column labels are the result types for the current solution type.
• Putting focus in a cell causes the top half of the form to reflect the current setting, just like the current advanced output request form. This means that the databox RESULT TYPE: gets updated with the result type of the currently selected cell. The OUTPUT REQUESTS: databox is also updated to show the actual content of the cell.
• If a cell is initially empty, selecting it will cause the top half of the form to display the appropriate default setting for the selected result type (i.e., column).
• Selecting a column header will allow you to change all subcase output requests of a particular type. The top half of the Edit Output Requests form will set to the default request of the particular result type.
• When you select a set of contiguous column cells, the top half of the form will configure to the upper most selected cell.
• You cannot select multiple columns.
Default Output Request Information
In order to make use of this new feature you will need to create a PCL file that contains the function user_change_default_out_req which will overwrite the existing default file in Patran. This new PCL file will need to be compiled and then the resulting library (.plb) will need to be loaded into Patran. This can be done using the p3midilog.pcl or the p3epilog.pcl file.
The user_change_default_out_req function makes use of the mscn_user_add_out_req and the mscn_user_del_out_req functions to add and delete default Output Request types. These two functions are defined as follows:  
mscn_user_add_out_req
(or_num, or_value)
Description:
 
 
This function adds either a specified version or a default version of an Output Request type to the list of default Output Requests.
 
 
Input:
 
 
INTEGER
or_num
The OR number of the output request type to add (See Table 3‑3).
STRING
or_value
The value of the selected output request type. Blank implies the default value.
  
mscn_user_del_out_req
(or_num)
Description:
 
 
This function deletes the specified Output Request type from the list of default Output Requests.
 
 
Input:
 
 
INTEGER
or_num
The OR number of the Output Request type to delete (See Table 3‑3).
Code Sample
FUNTION user_change_default_out_req(sol_seq)
INTEGER sol_seq
IF (sol_seq == 101 || sol_seq == 106) THEN
/* This will add this version of the Output Request type to the list of default */
/* Output Requests for solution 101 and 106. */
mscn_user_add_out_req (4,”MPCFORCES(SORT2,REAL)=ALL FEM”)
/* This will add the default version of these Output Request types from the list */
/* of default Output Requests for solution 101 and 106. */
mscn_user_add_out_req (10,“ ”)
mscn_user_add_out_req (6,“ ”)
/* This will delete these Output Request types from the list of default */
/* Output Requests for solution 101 and 106. */
mscn_user_del_out_req (1)
mscn_user_del_out_req (2)
mscn_user_del_out_req (3)
END IF
END FUNCTION
The following is a table that shows the current predefined default Output Requests (those marked with an X) and the allowed options (those marked with an O) for the various solution sequences.
Table 3‑3
Result ID Number (Solution Sequence)
OR Number
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
101
x
x
x
o
o
o
 
o
o
o
 
 
o
o
o
o
o
o
 
 
 
 
 
x
103
o
o
x
o
o
 
 
o
o
o
 
o
o
 
 
x
 
 
 
 
 
 
 
 
105
x
o
x
o
o
o
 
o
o
 
 
 
o
o
o
x
 
 
 
 
 
 
 
 
106
x
x
x
 
o
o
 
 
o
o
 
 
 
 
 
o
 
 
 
 
 
 
x
 
107
o
o
x
o
o
 
 
 
o
 
 
 
 
 
 
x
 
 
 
 
 
 
 
 
108
x
o
x
o
o
o
 
 
o
 
o
o
 
 
 
o
 
 
 
 
 
 
 
 
109
x
o
x
o
o
o
o
 
o
o
o
o
 
 
 
o
 
 
 
 
 
 
 
 
110
o
o
x
o
o
 
 
 
o
 
 
 
 
 
 
x
 
 
 
 
 
 
 
 
111
x
o
x
o
o
o
 
 
o
 
o
o
 
 
 
o
 
 
 
 
 
 
 
 
112
x
o
x
o
o
o
o
 
o
o
o
o
 
 
 
o
 
 
 
 
 
 
 
 
114
x
x
x
o
o
o
 
o
o
o
 
 
o
 
 
x
o
o
 
 
 
 
 
 
115
o
o
x
o
o
 
 
o
o
o
 
 
o
 
 
o
 
 
 
 
 
 
 
 
129
x
o
x
 
o
o
 
 
o
o
o
o
 
 
 
o
 
 
 
 
 
 
 
 
153
o
o
 
 
o
 
 
 
o
 
 
 
 
o
 
o
x
x
o
o
 
 
 
 
159
o
o
 
 
o
 
o
 
o
 
 
 
 
 
 
o
x
x
o
o
o
o
 
 
400
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
x
x
600
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
x
700
x
o
x
 
o
o
 
 
o
o
o
o
 
 
 
o
 
 
 
 
 
 
 
x
 
1 = Displacement, 2 = stress, 3 = spcforces, 4 = mpcforces, 5 = forces, 6 = oload, 7 = nlload, 8 = ese, 9 = strain, 10 = gpstress, 11 = velocity, 12 = acceleration, 13 = gpforce, 14 = gpsdcon, 15 = elsdcon, 16 = vector, 17 = thermal, 18 = flux, 19 = ht_oload, 20 = ht_spcforces, 21 =enthalpy, 22 = hdot
 
OR #
Default Value
1
DISPLACEMENT(SORT1,REAL)=All FEM
2
STRESS(SORT1,REAL,VONMISES,BILIN)=All FEM;PARAM,NOCOMPS,-1
3
SPCFORCES(SORT1,REAL)=All FEM
4
MPCFORCES(SORT1,REAL)=All FEM
5
FORCE(SORT1,REAL,BILIN)=All FEM
6
OLOAD(SORT1,REAL)=All FEM
7
NLLOAD=All FEM
8
ESE=All FEM
9
STRAIN(SORT1,REAL,VONMISES,STRCUR,BILIN)=All FEM
10
GPSTRESS=All FEM; VOLUME # SET,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL,BRANCH BREAK
11
VELOCITY(SORT1,REAL)=All FEM
12
ACCELERATION(SORT1,REAL)=All FEM
13
GPFORCE=All FEM
14
GPSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
15
ELSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
16
VECTOR(SORT1,REAL)=All FEM
17
THERMAL=(SORT1,PRINT)=All FEM
18
FLUX(SORT1,PRINT)=All FEM
19
OLOAD(SORT1,PRINT)=All FEM
20
SPCFORCES(SORT1,PRINT)=All FEM
21
ENTHALPY(SORT1,PRINT)=All FEM
22
HDOT(SORT1,PRINT)=All FEM
23
NLSTRESS
24
BCCONTACT
 
Note:  
In SOL 109, 112 & 159 will have SORT2 as the default in some versions of Patran.
Subcases Direct Text Input
This form is used to directly enter entries into the Case Control section for the defined subcase.
SOL 600 Output Requests
This subform defines the output data for a SOL 600 analysis subcase
 
Echo Marc Input File
Produces an echo of the input file.
Results in Marc Print File
Writes results to a print file.
Results (POST) File Options
 
• Increments between Writing Results
Defines the number of increments between writing results to the MD Nastran results file after the first increment of the analysis. The default is one (1) for every increment.
Note: You can select a fixed number of increments of output on the subcase parameters-load increments parameters form.
• Select Nodal Results...
Brings up a subform for selecting nodal results
• Select Element Results...
Brings up a subform for selecting elemental results.
Output requests for all subcases.
Select Nodal Results
This subform controls which nodal result quantities are returned from the analysis.
 
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers, that will be specified on the MARCOUT entry
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis.
Nodal Result
Postcode
Default(?)
DISPLACEMENT
1
YES
ROTATION
2
no
EXTERNAL FORCE
3
no
EXTERNAL MOMENT
4
no
REACTION FORCE
5
YES
REACTION MOMENT
6
no
PORE PRESSURE
23
no
VELOCITY
28
no
ROTATIONAL VELOCITY
29
no
ACCELERATION
30
no
ROTATIONAL ACCELERATION
31
no
MODAL MASS
32
no
ROTATION MODAL MASS
33
no
CONTACT NORMAL STRESS
34
no
CONTACT NORMAL FORCE
35
no
FRICTION STRESS
36
no
FRICTION FORCE
37
no
CONTACT STATUS
38
no
CONTACT TOUCHED BODY
39
no
HERRMANN VARIABLE
40
no
POST CODE, No. -11
-11 thru -16
no
POST CODE, No. -22
-21 thru -23
no
POST CODE, No. -31
-31
no
POST CODE, No. -41
-41
no
POST CODE, No. -51
-51
no
Note: The POST CODE (<0) are for user-defined quantities via user subroutine UPSTNO.
Element Output Requests
This subform controls which element result quantities are returned from the MSC.Marc analysis.
 
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers.
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
Element X-section Results
Defines the number of layer points to use through the cross section of homogeneous shells, plates and beams. This number must be odd if not a composite.
Note: If no changes are made to the default output requests, no MARCOUT entry will be written and MD Nastran will determine the appropriate output.
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis.
Elemental Result
Postcode
Solutions
Default(?)
STRAIN, TOTAL COMPONENTS
301
nonlinear only
YES
STRAIN, TOTAL COMPONENTS
(defined system)
461
nonlinear only
no
STRAIN, ELASTIC COMPONENTS
401
any
no
STRAIN, ELASTIC COMPONENTS
(global system)
421
any
no
STRAIN, ELASTIC EQUIVALENT
127
any
no
STRAIN, PLASTIC COMPONENTS
321
nonlinear only
no
STRAIN, PLASTIC COMPONENTS
(global system)
431
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT
27
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT
(from rate)
7
nonlinear only
no
STRAIN, CRACKING COMPONENTS
381
nonlinear only
no
STRAIN, CREEP COMPONENTS
331
creep only
no
STRAIN, CREEP COMPONENTS
(global system)
441
creep only
YES
STRAIN, CREEP EQUIVALENT
37
creep only
no
STRAIN, CREEP EQUIVALENT
(from rate)
8
creep only
no
STRAIN, THERMAL
371
any
no
STRAIN, THICKNESS
49
any
no
STRAIN, VELOCITY
451
nonlinear only
no
STRESS, COMPONENTS
311
any
no
STRESS, COMPONENTS
(defined system)
391
an
no
STRESS, COMPONENTS
(global system)
411
any
YES
STRESS, EQUIVALENT YIELD
59
nonlinear only
no
STRESS, EQUIVALENT MISES
17
any
no
STRESS, MEAN NORMAL
18
any
no
STRESS, INTERLAMINAR SHEAR No. 1
108
any
no
STRESS, INTERLAMINAR SHEAR No. 2
109
any
no
STRESS, INTERLAMINAR
COMPONENTS
501,511
any
no
STRESS, CAUCHY COMPONENTS
341
nonlinear only
no
STRESS, CAUCHY EQUIVALENT
47
nonlinear only
no
STRESS, HARMONIC COMPONENTS
351 (real)
361(imag)
harmonic only
no
STRESS, REBAR UNDEFORMED
471
any
no
STRESS, REBAR DEFORMED
481
any
no
FORCES, ELEMENT
264-269
any
no
BIMOMENT
270
any
no
STRAIN RATE, PLASTIC
28
nonlinear only
no
STRAIN RATE, EQUIVALENT
VISCOPLASTIC
175
any
no
STATE VARIABLE, SECOND
29
any
no
STATE VARIABLE, THIRD
39
any
no
TEMPERATURE, ELEMENT TOTAL
9
any
no
TEMPERATURE, ELEMENT
INCREMENTAL
10
any
no
STRAIN ENERGY DENSITY, TOTAL
48
nonlinear only
no
STRAIN ENERGY DENSITY, ELASTIC
58
any
no
STRAIN ENERGY DENSITY, PLASTIC
68
nonlinear only
no
THICKNESS, ELEMENT
20
any
no
VOLUME, ELEMENT
78
any
no
VOLUME, VOID FRACTION
177
any
no
GRAIN SIZE
79
any
no
FAILURE, INDEX No. 1-7
91-103
any
no
DENSITY, RELATIVE
179
any
no
POST CODE, No. 19
19
any
no
POST CODE, No. 38
38
any
no
POST CODE, No. -11
-11 thru -16
any
no
POST CODE, No. -21
-21 thru -23
any
no
POST CODE, No. -31
-31
any
no
POST CODE, No. -41
-41
any
no
POST CODE, No. -51
-51
any
no
DDAM Output Requests
The output requests form has been altered for the DDAM solution. Because the program performs an NRL sum and has no explicit constraints, only a few result quantities are available:
Nodal Results:
Displacement
Velocity
Accelerations
Element Results:
Stress
Force
The results reported in the .f06 file are printed sequentially, first x-shock results, then y, then z, but all are labeled as TIME = 0.000000E+00. To differentiate these in the file, there is a small header printer prior to the results for each shock direction that looks something like this:
 ^^^     
 ^^^ *************************************** 
 ^^^     
 ^^^ SUMMED MODAL RESPONSES IN X-DIRECTION   
 ^^^     
 ^^^ *************************************** 
 ^^^
If you need to find the start of the X-shock results, search for X-DIRECTION to find this header and proceed from there.
It is necessary to specify that Patran calculate the combined stresses on a mode-by-mode basis, and NRL sum the combined results. See Defining Translation Parameters for DDAM (SOL 187) (Ch. 4).
Mode by Mode Output
You can use the Direct Text Input section of Patran Analysis forms to obtain more data. Using the parameters XBYMODE, YBYMODE and ZBYMODE you can get mode by mode data for the selected direction. To get this data, enter the following lines into the Bulk Data direct text area:
PARAM,XBYMODE,YES
PARAM,YBYMODE,YES
PARAM,ZBYMODE,YES
You can select one or more of these parameters. Keep in mind that this generates a lot of data for an analysis with a lot of modes, and that you must have an output request for the corresponding data – e.g., if you want mode-by-mode displacements, you must have a DISPLACEMENT request as chosen above.
Each of these parameters outputs the data to the .f06 file if you have the (PRINT) option on, or an .op2 file if the (PLOT) option is on. Both are on by default when you specify something like:
DISPLACEMENT = ALL
Alternately,
DISPLACEMENT(PLOT) = ALL
DISPLACEMENT(PRINT) = ALL
plots or prints the results. If unassigned, the mode-by-mode results outputs to generic Fortran files (like fort.42), so it is necessary to add an ASSIGN statement to the file if you wish to have these files named appropriately. To do this, use the FMS section in the Direct Text Input form, and add lines like:
ASSIGN OUTPUT2=’jobname_mbmx.op2’, UNIT=41, DELETE
ASSIGN OUTPUT2=’jobname_mbmy.op2’, UNIT=42, DELETE
ASSIGN OUTPUT2=’jobname_mbmz.op2’, UNIT=43, DELETE
In the .f06 file, the mode-by-mode results are labeled with their own header prior to the section:
 ^^^     
 ^^^ **************************************************  
 ^^^     
 ^^^ INDIVIDUAL SCALED MODAL RESPONSES IN Y-DIRECTION    
 ^^^     
 ^^^ **************************************************  
 ^^^
Since the mode-by-mode velocities and accelerations are calculated by multiplying the displacements by the frequency (omega and omega2), MD Nastran labels them as Eigenvectors. If you ask for displacement, velocity, and acceleration for three modes, you will find nine Eigenvectors in the .f06 file with repeating frequencies – the first three (1-3) are displacements, the next three (4-6) velocities, and the last three (7-9) the accelerations. The .op2 files are similar, reporting the three as Eigenvectors with repeating frequencies. The magnitude of the values should be a clue as to what you are looking at for all but the lowest frequencies. The Fortran Driver File (jobname.ddd)
 
Some of the options you choose on the Subcase Parameters form are written to an external file that is read by the Fortran file when it calculates the spectrum. While you do not have the ability to edit this file when using MSC.FEA, the file is a hardcopy ASCII record of what options were used when running the DDAM analysis. The file is small and has just a few lines that comprise the answers to questions that the ddam.exe program asks if it is run interactively. File Format (varies depending on chosen options on the first record)
Record 1
(user spectrum file) (user coef file) (DDS-072 format)
user spectrum file = T (use a user defined spectrum)
= F (use coefficients)
user coef file = T (use an external coefficient file)
= F (use the coefficients compiled into the Fortran)
DDS-072 format = T (use DDS-072 style equations)
= F (use NRL 1396 style equations)
 
Record 1a (if either file option on record 1 was true)
filename
filename = name of either the spectrum file or coefficient file
Record 2 (if using coefficients)
nsurf nstruc nplast
ship type = 1 (surface ship equations)
= 2 (submarine equations)
mount location = 1 (file mounted equipment)
= 2 (hull mounted equipment)
elastic/plastic = 1 (use elastic factors)
= 2 (use elastic/plastic factors)
 
Record 3
pref
pref = 0.0 (use default cutoff in program)
= nnn.nn
 
Record 4
Ming
Ming = 0.0 (no minimum G)
= n.n (use this minimum G value)
 
Record 5
(F/A axis) (Vert axis)
F/A axis = X (F/A is along the X axis)
= Y (F/A is along the Y axis)
= Z (F/A is along the Z axis)
Vert axis = X (Vertical is along the X axis)
= Y (Vertical is along the Y axis)
= Z (Vertical is along the Z axis)
 
Record 6
.f11 filename
.f11 filename = name of the .f11 file
 
Record 7
.f13 filename
.f13 filename = name of the .f13 file
 
Record 8
.ver filename
.ver filename = name of the modal verification file
 
Depending on the chosen options, the file will look like one of the following:
No special user options – coefficients from default source:
 
F F T
nsurf nstruc nplast
pref
ming
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
User coefficient option:
 
F T T
coef.dat filename
nsurf nstruc nplast
pref
ming
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
 
User spectrum Option:
 
T F T
spec.dat filename
pref
ming
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
 
Note: Note that capitalization is required. The file is read free-format, so spacing is not important. A sample file for a conventional analysis might look like:
 
F F T
1 1 1
100.
1.
X Z
d1.f11
d2.f11
d1.ver
 
1 At the present time, superelement specifications are allowed only in the structured linear static solution type (Solution Sequence 101).