Analysis Control Data

Outline of Analysis Control Data

In FrontISTR, an analysis control data file is input to acquire the computing control data, solver control data and post process (visualization) control data as shown in the following figure, in order to implement the analytical calculations.

The features of the analysis control data file are as follows.

This is an ASCII format file based on a free format.
This file consists of a header which starts with "!" and the data following this.
The order of description of the header is basically free.
A "," is used as a punctuation mark of the data.
The inside of the file is briefly divided into three zones.
"!END" is input at the end of the file for completion.

Example of Analysis Control Data

#############################################################
##### (1) Computing control data portion ####################
#############################################################
### Control File for HEAT solver
!SOLUTION,TYPE=HEAT
!FIXTEMP
 XMIN, 0.0
 XMAX, 500.0

#############################################################
##### (2) Solver control data portion #######################
#############################################################
### Solver Control
!SOLVER,METHOD=1,PRECOND=1,ITERLOG=NO,TIMELOG=NO
100, 1
1.0e-8,1.0,0.0

#############################################################
##### (3) Post control (visualization) data portion #########
#############################################################
### Post Control
!WRITE,RESULT
!WRITE,VISUAL
!VISUAL, method=PSR
!surface_num = 1
!surface 1
!surface_style = 1
!display_method 1
!color_comp_name = TEMPERATURE
!color_subcomp = 1
!output_type = BMP
!x_resolution = 500
!y_resolution = 500
!num_of_lights = 1
!position_of_lights =
-20.0, 5.8, 80.0
!viewpoint = -20.0 10.0 8.0
!up_direction = 0.0 0.0 1.0
!ambient_coef= 0.3
!diffuse_coef= 0.7
!specular_coef= 0.5
!color_mapping_style= 1
!!interval_mapping= -0.01, 0.02
!color_mapping_bar_on = 1
!scale_marking_on = 1
!num_of_scale = 5
!font_size = 1.5
!font_color = 1.0 1.0 1.0
!END

Input Rules

The analysis control data consists of a header line, data line and a comment line.

One header is always included in the header line.

Header: The header specifies the meaning of the data and the data block in the analysis control data. When the head of the term starts with a "!", it is considered to be a header.
Header Line: The header and the parameter accompanying this are described in this line.; The header line must start with a header. When a parameter is required, a "," must be used to continue after that. When the parameter takes on a value, use an "=" after the parameter and describe the value after that.; The header line can not be described in more than two lines.
Data Line: The data line starts after the header line, and the necessary data is described.; The data lines may be in multiple lines; however, this is determined according to the rules of the data description defined by each header.; There are cases where data lines are not required.
Punctuation: A comma "," is used as a punctuation of the data.
Handling of Blanks: Blanks are disregarded.
Name: Regarding the characters which can be used for the name, there is the underscore "_", hyphen "-", and alphanumeric characters "a - z, A - Z, 0 - 9"; however, the first letter of the name must start with "_", or an alphabetic character "a - z, A - Z". There is no distinction between uppercase and lowercase letters, and all letters are internally handled as uppercase letters.; The maximum length of the name is 63 characters.
File Name: Regarding the characters which can be used for the file name, there are the underscore "_", hyphen "-", period ".", slash "/", and the alphanumeric characters "a - z, A - Z, 0 - 9".; As long as there is no specific description, a path can be included in the file name. Both the relative path and the absolute path can be specified.; The maximum length of the file name is 1,023 characters.
Floating Point Data: Exponents are optional. An "E" or "e" character must be added before the exponent. The selection of "E" or "e" is optional.
!!, #, Comment Line: Lines starting with "!!" or "#" are considered to be comment lines, and are disregarded. A comment line can be inserted in any position in the file, and there are no restrictions on the number of lines.
!END: End of mesh data; When this header is displayed, the reading of the mesh data is completed.

Analysis Control Data

Header List of Computing Control Data

In FrontISTR, the following items can be mentioned as the boundary conditions which can be used for the computing control data.

Distributed load conditions (body force, pressure loading, gravity, centrifugal force)
Concentrated load conditions
Heat load
Single point restriction conditions (SPC conditions)
Spring boundary conditions
Contact
Concentrated heat flux
Distributed heat flux
Convective heat transfer boundary
Radiant heat transfer boundary
Specified temperature boundary

The same as the mesh data, the !HEADER format is used as the definition method of the above boundary conditions.

The header list of the common control data is shown in the following Table 7.3.1, and the header list for each analysis type is shown in Table 7.3.2.

Table 7.3.1: Control Data Common to All Analysis

Header	Meaning	Remarks	Description No.
`!VERSION`	Solver version number		1-1
`!SOLUTION`	Specification of analysis type	Mandatory	1-2
`!WRITE,VISUAL`	Specification of visualization output		1-3
`!WRITE,RESULT`	Specification of results output		1-4
`!WRITE,LOG`	Specification of results output		1-5
`!OUTPUT_VIS`	Control of visualization output items		1-6
`!OUTPUT_RES`	Control of results output items		1-7
`!RESTART`	Control of restarting		1-8
`!ECHO`	Echo output		1-9
`!ORIENTATION`	Definition of local coordinate system		1-10
`!SECTION`	Definition of local coordinate system the sction correspondent to		1-11
`!INITIAL_CONDITION`	Definition of initial condition		1-12
`!END`	Ending specification of control data		1-13

Table 7.3.2: Control Data for Static Analysis

Header	Meaning	Description No.
`!STATIC`	Static analysis control	2-1
`!MATERIAL`	Material name	2-2
`!ELASTIC`	Elastic material physical properties	2-2-1
`!PLASTIC`	Plastic material physical properties	2-2-2
`!HYPERELASTIC`	Hyperelastic material physical properties	2-2-3
`!VISCOELASTIC`	Viscoelastic material physical properties	2-2-4
`!CREEP`	Creep material physical properties	2-2-5
`!DENSITY`	Mass density	2-2-6
`!EXPANSION_COEFF`	Coefficient of linear expansion	2-2-7
`!TRS`	Tempearture dependent behaviour of viscoelastic material	2-2-8
`!FLUID`	Flow Condition	2-2-9
`!USER_MATERIAL`	User defined material	2-2-10
`!BOUNDARY`	Displacement boundary conditions	2-3
`!SPRING`	Spring boundary conditions	2-3-1
`!CLOAD`	Concentrated load	2-4
`!DLOAD`	Distributed load	2-5
`!ULOAD`	User defined external load	2-6
`!CONTACT_ALGO`	Contact analytic algorithm	2-7
`!CONTACT`	Contact	2-8
`!TEMPERATURE`	Nodal temperature in thermal stress analysis	2-9
`!REFTEMP`	Reference temperature in thermal stress analysis	2-10
`!STEP`	Analysis step control	2-11
`!AUTOINC_PARAM`	Auto increment control	2-12
`!TIME_POINTS`	Output time point control	2-13
`!CONTACT_PARAM`	Contact scan control	2-14

Table 7.3.3: Control Data for Eigenvalue Analysis

Header	Meaning	Remarks	Description No.
`!EIGEN`	Eigenvalue analysis control	Mandatory in eigenvalue analysis	3-1

Table 7.3.4: Control Data for Heat Conduction Analysis

Header	Meaning	Remarks	Description No.
`!HEAT`	Heat conduction analysis control	Mandatory in heat conduction analysis	4-1
`!FIXTEMP`	Nodal temperature		4-2
`!CFLUX`	Concentrated heat flux given to node		4-3
`!DFLUX`	Distributed heat flux / internal heat generation given to element surface		4-4
`!SFLUX`	Distributed heat flux by surface group		4-5
`!FILM`	Heat transfer coefficient given to boundary plain		4-6
`!SFILM`	Heat transfer coefficient by surface group		4-7
`!RADIATE`	Radiation factor given to boundary plane		4-8
`!SRADIATE`	Radiation factor by surface group		4-9
`!WELD_LINE`	Weld line		4-10

Table 7.3.5: Control Data for Dynamic Analysis

Header	Meaning	Remarks	Description No.
`!DYNAMIC`	Dynamic analysis control	Mandatory in dynamic analysis	5-1
`!VELOCITY`	Velocity boundary conditions		5-2
`!ACCELERATION`	Acceleration boundary conditions		5-3
`!COUPLE`	Coupled surface definition Required in coupled analysis		5-4
`!EIGENREAD`	Specification of eigenvalues and eigenvectors	Mandatory in frequency response analysis	5-5
`!FLOAD`	Definition of concentrated load for frequency response analysis		5-6

In each header, there are data items which comply with the parameter and each header.

Each of the above headers is described in the following with examples of data creation for each analysis type. The description number in the above Table is the number indicated on the right end of the example of the data creation.

(1) Control data common to all analyses

Example of Analysis Control Data

### Control File for FISTR
!VERSION                                        1-1
  5
!SOLUTION, TYPE=STATIC                          1-2
!WRITE, VISUAL                                  1-3
!WRITE, RESULT                                  1-4
!ECHO                                           1-9
!BOUNDARY                                       2-3
  FIX, 1, 3, 0.0
!CLOAD                                          2-4
  CL1, 3, -1.0
!END                                            1-12

Description of Header

1-1 `!VERSION`

Refer to the solver version.

1-2 `!SOLUTION, TYPE=STATIC`

TYPE=analysis type

1-3 `!WRITE, VISUAL`

Output of data by visualizer via memory

Outputs the file just by entering

1-4 `!WRITE, RESULT`

Output of analysis results file

Outputs the file just by entering

1-6 `!ECHO`

Output of node data, element data and material data to log file

Outputs to the file just by entering

1-8 `!END`

Indicates the end of control data

(2) Static analysis control data

Example of Static Analysis Control data

### Control File for FISTR
!SOLUTION, TYPE=STATIC                          1-2
!WRITE, VISUAL                                  1-3
!WRITE, RESULT                                  1-4
!ECHO                                           1-9
!MATERIAL, NAME=M1                              2-2
!ELASTIC, TYPE=ISOTROPIC                        2-2-1
  210000.0, 0.3
!BOUNDARY                                       2-3
  FIX, 1, 3, 0.0
!SPRING 2-3-1
  200, 1, 0.03
!CLOAD 2-4
  CL1, 3, -1.0
!DLOAD 2-5
  1, P1, 1.0
!TEMPERATURE                                    2-9
  1, 10.0
!REFTEMP                                        2-10
!STEP, CONVERG=1.E-5, MAXITER=30                2-11
!END                                            1-12

Description of Header

Red figures are the values indicated in the example.
Alphabetic characters in the 2nd line of the table express the parameter name.

2-1 `!STATIC`

Setting of static analysis method

2-2 `!MATERIAL`

Definition of material physical properties

NAME = name of material physical properties

2-2-1 `!ELASTIC, TYPE=ISOTROPIC`

Definition of elastic substance

TYPE = elastic type

Young's Modulus	Poisson's Ratio
YOUNG_MODULUS	POISSON_RATIO
210000.0	0.3

2-3 `!BOUNDARY`

Definition of displacement boundary conditions

Node ID or Node Group Name	Start No. of Restricted Degree of Freedom	End No. of Restricted Degree of Freedom	Restricted Value
NODE_ID	DOF_idS	DOF_idE	Value
FIX,	1,	3,	0.0

2-3-1 `!SPRING`

Definition of spring boundary conditions

Node ID or Node Group Name	Restricted Degree of Freedom	Spring Constant
NODE_ID	DOF_id	Value
200,	1,	0.03

2-4 `!CLOAD`

Definition of concentrated load

Node ID or Node Group Name	Degree of Freedom No.	Load Value
NODE_ID	DOF_id	Value
CL1,	3,	-1.0

2-5 `!DLOAD`

Definition of distributed load

Element ID or Element Group Name	Load Type No.	Load Parameter
ELEMENT_ID	LOAD_type	param
1,	P1,	1.0

2-9 `!TEMPERATURE`

Specification of nodal temperature used for thermal stress analysis

Node ID or Node Group Name	Temperature
NODE_ID	Temp_Value
1,	10

2-10 `!REFTEMP`

Definition of reference temperature in thermal stress analysis

2-11 `!STEP`

Control of nonlinear static analysis (Omissible in the case of linear analysis)

Convergence Value Judgment Threshold	No. of Sub Steps (When AMP exists, AMP has priority)	Max No. of Iterative Calculations	Time Function Name (Specified in `!AMPLITUDE`)
CONVERG	SUBSTEPS	MAXITER	AMP
1.0E-05	10	30

(3) Eigenvalue analysis control data

Example of Eigenvalue Analysis Control Data

### Control File for FISTR
!SOLUTION, TYPE=EIGEN                           1-2
!WRITE, VISUAL                                  1-3
!WRITE, RESULT                                  1-4
!ECHO                                           1-9
!EIGEN                                          3-1
  3, 1.0E-8, 60
!BOUNDARY                                       2-3
 FIX, 1, 2, 0.0
!END

Description of Header

Red figures are the values indicated in the example.

3-1 `!EIGEN`

Parameter settings of eigenvalue analysis

No. of Eigenvalue	Allowance	Max No. of Iterations
NSET	LCZTOL	LCZMAX
3,	1.0E-8,	60

2-3 `!BOUNDARY` (Same items an in Static Analysis)

Definition of displacement boundary conditions

Node ID or Node Group Name	Start No. of Restricted Degree of Freedom	End No. of Restricted Degree of Freedom	Restricted Value
NODE_ID	DOF_idS	DOF_idE	Value
FIX,	1,	3,	0.0

(4) Heat conduction analysis control data

Example of Heat Conduction Analysis Control Data

### Control File for FISTR
!SOLUTION, TYPE=HEAT                            1-2
!WRITE, VISUAL                                  1-3
!WRITE, RESULT                                  1-4
!ECHO                                           1-9
!HEAT                                           4-1
!FIXTEMP                                        4-2
  XMIN, 0.0
  XMAX, 500.0
!CFLUX                                          4-3
  ALL, 1.0E-3
!DFLUX                                          4-4
  ALL, S1, 1.0
!SFLUX                                          4-5
  SURF, 1.0
!FILM                                           4-6
  FSURF, F1, 1.0, 800
!SFILM                                          4-7
  SFSURF, 1.0, 800.0
!RADIATE                                        4-8
  RSURF, R1, 1.0E-9, 800.0
!SRADIATE                                       4-9
  RSURF, R1, 1.0E-9, 800.0
!END                                            1-12

Description of Header

Red figures are the values indicated in the example.

4-1 `!HEAT`

Definition of control data for calculation

!HEAT
  (No data)                         ----- Steady calculation
!HEAT
  0.0                               ----- Steady calculation
!HEAT
  10.0, 3600.0                      ----- Fixed time increment unsteady calculation
!HEAT
  10.0, 3600.0, 1.0                 ----- Automatic time increment unsteady calculation
!HEAT
  10.0, 3600.0, 1.0, 20.0           ----- Automatic time increment unsteady calculation

4-2 `!FIXTEMP`

Node group name, or node ID and fixed temperature

4-3 `!CFLUX`

Definition of concentrated heat flux given to node

Node Group Name or Node ID	Heat Flux Value
NODE_GRP_NAME	Value
ALL,	1.0E-3

4-4 `!DFLUX`

Definition of distributed heat flux and internal heat generation given to surface of element

Element Group Name or Element ID	Load Type No.	Heat Flux Value
ALL,	S1,	1.0

Load Parameter

Load Type No.	Applied Surface	Parameter
BF	Element Overall	Calorific value
S1	Surface No. 1	Heat flux value
S2	Surface No. 2	Heat flux value
S3	Surface No. 3	Heat flux value
S4	Surface No. 4	Heat flux value
S5	Surface No. 5	Heat flux value
S6	Surface No. 6	Heat flux value
S0	Shell surface	Heat flux value

4-5 `!SFLUX`

Definition of distributed heat flux by surface group

Surface Group Name	Heat Flux Value
SURFACE_GRP_NAME	Value
SURF,	1.0

4-6 `!FILM`

Definition of heat transfer coefficient given to boundary plane

Element Group Name or Element ID	Load Type No.	Heat Transfer Coefficient	Ambient Temperature
ELEMENT_GRP_NAME	LOAD_type	Value	Sink
FSURF,	F1,	1.0,	800.0

Load Parameter

Load Type No.	Applied Surface	Parameter
F1	Surface No. 1	Heat transfer coefficient and ambient temperature
F2	Surface No. 2	Heat transfer coefficient and ambient temperature
F3	Surface No. 3	Heat transfer coefficient and ambient temperature
F4	Surface No. 4	Heat transfer coefficient and ambient temperature
F5	Surface No. 5	Heat transfer coefficient and ambient temperature
F6	Surface No. 6	Heat transfer coefficient and ambient temperature
F0	Shell surface	Heat transfer coefficient and ambient temperature

4-7 `!SFILM`

Definition of heat transfer coefficient by surface group

Surface Group Name	Heat Transfer Rate	Ambient Temperature
SURFACE_GRP_NAME	Value	Sink
SFSURF,	1.0,	800.0

4-8 `!RADIATE`

Definition of radiation factor given to boundary plane

Element Group Name or Element ID	Load Type No.	Radiation Factor	Ambient Temperature
ELEMENT_GRP_NAME	LOAD_type	Value	Sink
RSURF,	R1,	1.0E-9,	800.0

Load Parameter

Load Type No.	Applied Surface	Parameter
R1	Surface No. 1	Radiation factor and ambient temperature
R2	Surface No. 2	Radiation factor and ambient temperature
R3	Surface No. 3	Radiation factor and ambient temperature
R4	Surface No. 4	Radiation factor and ambient temperature
R5	Surface No. 5	Radiation factor and ambient temperature
R6	Surface No. 6	Radiation factor and ambient temperature
R0	Shell surface	Radiation factor and ambient temperature

4-9 `!SRADIATE`

Definition of radiation factor by surface group

Surface Group Name	Radiation Factor	Ambient Temperature
SURFACE_GRP_NAME	Value	Sink
SRSURF,	1.0E-9,	800.0

(5) Dynamic analysis control data

Example of Dynamic Analysis Control Data

### Control File for FISTR
!SOLUTION, TYPE=DYNAMIC                         1-2
!DYNAMIC, TYPE=NONLINEAR                        5-1
  1 , 1
  0.0, 1.0, 500, 1.0000e-5
  0.5, 0.25
  1, 1, 0.0, 0.0
  100, 5, 1
  0, 0, 0, 0, 0, 0
!BOUNDARY, AMP=AMP1                             2-3
  FIX, 1, 3, 0.0
!CLOAD, AMP=AMP1                                2-4
  CL1, 3, -1.0
!COUPLE, TYPE=1                                 5-4
  SCOUPLE
!STEP, CONVERG=1.E-6, ITMAX=20                  2-11
!END                                            1-12

Description Header

Red figures are the values indicated in the example.
Alphabetic characters in the 2nd line of the table express the parameter name.

5-1 `!DYNAMIC`

Controlling the linear dynamic analysis

Solution of Equation of Motion	Analysis Types
idx_eqa	idx_resp
11	1

Analysis Start Time	Analysis End Time	Overall No. of STEPS	Time Increment
t_start	t_end	n_step	t_delta
0.0	1.0	500	1.0000e-5

Parameter $\gamma$ of Newmark- $\beta$ Method	Parameter $\beta$ of Newmark- $\beta$ Method
gamma	beta
0.5	0.25

Type of Mass Matrix	Type of Damping	Parameter $R_m$ of Rayleigh Damping	Parameter of $R_k$ of Rayleigh Damping
idx_mass	idx_dmp	ray_m	ray_k
1	1	0.0	0.0

Resules Output Interval	Monitoring Node ID or Node Group Name	Results Output Interval of Displacement Monitoring
nout	node_monit_1	nout_monit
100	55	nout_monit

Output Control Displacement	Output Control Velocity	Output Control Acceleration	Output Control Reaction Force	Output Control Strain	Output Control Stress
iout_list(1)	iout_list(2)	iout_list(3)	iout_list(4)	iout_list(5)	iout_list(6)
0	0	0	0	0	0

2-3 `!BOUNDARY` (Same items as in Static Analysis)

Definition of displacement boundary conditions

Node ID or Node Group Name	Start No. of Restricted Degree of Freedom	End No. of Restricted Degree of Freedom	Restricted Value
NODE_ID	DOF_idS	DOF_idE	Value
FIX,	1,	3,	0.0

2-4 `!CLOAD` (Same items as in Static Analysis)

Definition of concentrated load

Node ID or Node Group Name	Degree of Freedom No.	Load Value
CL1,	3,	-1.0

5-4 `!COUPLE, TYPE=1`

Definition of coupled surface

Coupling Surface Group Name
SCOUPLE

2-11 `!STEP, CONVERG=1.E-10, ITMAX=20`

Control of nonlinear static analysis

(Omissible in the case of linear analysis, and unnecessary for explicit method)

Convergence Value Judgment Threshold (Default: 1.0E-06)	No. of Sub Steps (When AMP exists, AMP has priority)	Max No. of Iterative Calculations
CONVERG	SUBSTEPS	ITMAX
1.0E-10		20

(6) Dynamic analysis (Frequency Response Analysis) Control Data

Example of Dynamic analysis (Frequency Response Analysis)

!SOLUTION, TYPE=DYNAMIC                         1-2
!DYNAMIC                                        5-1
  11 , 2
  14000, 16000, 20, 15000.0
  0.0, 6.6e-5
  1, 1, 0.0, 7.2E-7
  10, 2, 1
  1, 1, 1, 1, 1, 1
!EIGENREAD                                      5-5
  eigen0.log
  1, 5
!FLOAD, LOAD CASE=2                             5-6
  _PickedSet5, 2, 1.0
!FLOAD, LOAD CASE=2
  _PickedSet6, 2, 1.0

Description of Header

Red figures are the values indicated in the example.
Alphabetic characters in the 2nd line of the table express the parameter name.

5-1 `!DYNAMIC`

Controlling the frequency response analysis

Solution of Equation of Motion	Analysis Types
idx_eqa	idx_resp
11	2

Minimum Frequency	Maximum Frequency	Number of divisions for the frequency range	Frequency to obtain displacement
f_start	f_end	n_freq	f_disp
14000	16000	20	15000.0

Analysis Start Time	Analysis End Time
0.0	6.6e-5

Type of Mass Matrix	Type of Damping	Parameter $R_m$ of Rayleigh Damping	Parameter $R_k$ of Rayleigh Damping
idx_mass	idx_dmp	ray_m	ray_k
1	1	0.0	7.2E-7

Results Output Interval in Time Domain	Visualization Type (1-Mode shapes, 2-Time history result at f_disp)	Monitoring Node ID in Frequency Domain
nout	vistype	nodeout
10	2	1

Output Control Displacement	Output Control Velocity	Output Control Acceleration	Output Control ignored	Output Control ignored	Output Control ignored
iout_list(1)	iout_list(2)	iout_list(3)	iout_list(4)	iout_list(5)	iout_list(6)
1	1	1	1	1	1

5-5 `!EIGENREAD`

Controlling the input file for frequency response analysis

The name of eigenvalue analysis log
eigenlog_filename
eigen0.log

lowest mode to be used in frequency response analysis	highest mode to be used frequency response analysis
start_mode	end_mode
1	5

5-6 `!FLOAD`

Defining external forces applied in frequency response analysis

Node ID, Node Group Name or Surface Group Name	Degree of Freedom No.	Load Value
_PickedSet5	2	1.0

Solver Control Data

Example of Solver Control Data

### SOLVER CONTROL
!SOLVER, METHOD=CG, PRECOND=1, ITERLOG=YES, TIMELOG=YES        6-1
  10000, 1                                                     6-2
  1.0e-8, 1.0, 0.0

Description of Header

Red figures are the values indicated in the example.

6-1 `!SOLVER`

METHOD    = method
           (CG, BiCGSTAB, GMRES, GPBiCG, etc.)
TIMELOG   = whether solver computation time is output
MPCMETHOD = method for multipoint constraints
            (1: Penalty method,
             2: MPC-CG method (Deprecated),
             3: Explicit master-slave elimination)
DUMPTYPE  = type of matrix dumping
DUMPEXIT  = whether program exits right after dumping matrix

The following parameters will be disregarded when a direct solver is selected in the method.

PRECOND   = preconditioner
ITERLOG   = whether solver convergence history is output
SCALING   = whether matrix is scaled so that each diagonal element becomes 1
USEJAD    = whether matrix ordering optimized for vector processors is performed
ESTCOND   = frequency for estimating condition number
            (Estimation performed at every specified number of iterations and
             at the last iteration.  No estimation when 0 is specified.)

6-2

No. of Iterations	Iteration Count of Preconditioning	No. of Krylov Subspaces	No. of Colors for Multi-Color ordering	No. of Recycling Set-Up Info for Preconditioning
NITER	iterPREMAX	NREST	NCOLOR_IN	RECYCLEPRE
10000	1

6-3

Truncation Error	Scale Factor for Diagonal Elements when computing Preconditioning Matrix	Not Used
1.0e-8,	1.0,	0.0

Post Process (Visualization) Control Data

An example of the post process (visualization) control data and the contents are shown in the following.

Example of Visualization Control Data

Each description number (P1-0, P1-1, etc.) is linked to the number of the detailed descriptions in the following.

P1-○ expresses the common data, and P2-○ expresses the parameter for the purpose of the rendering.
In addition, the rendering will become valid only when the output_type=BMP.
When the surface_style is !surface_style = 2 (isosurface) !surface_style = 3 (user specified curved surface), a separate setting is required. The data is indicated collectively after the common data.
(P3-○ is a description of the isosurface in !surface_style = 2. P4-○ is a description of the user specified curved surface in !surface_style = 3.)
The items indicated with two ! like "!!", will be recognized as a comment and will not affect the analysis.

### Post Control                                Description No.
!VISUAL, method=PSR                             P1-0
!surface_num = 1                                P1-1
!surface 1                                      P1-2
!surface_style = 1                              P1-3
!display_method = 1                             P1-4
!color_comp_name = STRESS                       P1-5
!colorsubcomp_name                              P1-6
!color_comp 7                                   P1-7
!!color_subcomp = 1                             P1-8
!iso_number                                     P1-9
!specified_color                                P1-10
!deform_display_on = 1                          P1-11
!deform_comp_name                               P1-12
!deform_comp                                    P1-13
!deform_scale = 9.9e-1                          P1-14
!initial_style = 1                              P1-15
!deform_style = 3                               P1-16
!initial_line_color                             P1-17
!deform_line_color                              P1-18
!output_type = BMP                              P1-19
!x_resolution = 500                             P2-1
!y_resolution = 500                             P2-2
!num_of_lights = 1                              P2-3
!position_of_lights = -20.0, 5.8, 80.0          P2-4
!viewpoint = -20.0 -10.0 5.0                    P2-5
!look_at_point                                  P2-6
!up_direction = 0.0 0.0 1.0                     P2-7
!ambient_coef= 0.3                              P2-8
!diffuse_coef= 0.7                              P2-9
!specular_coef= 0.5                             P2-10
!color_mapping_style= 1                         P2-11
!!interval_mapping_num                          P2-12
!interval_mapping= -0.01, 0.02                  P2-13
!rotate_style = 2                               P2-14
!rotate_num_of_frames                           P2-15
!color_mapping_bar_on = 1                       P2-16
!scale_marking_on = 1                           P2-17
!num_of_scale = 5                               P2-18
!font_size = 1.5                                P2-19
!font_color = 1.0 1.0 1.0                       P2-20
!background_color                               P2-21
!isoline_color                                  P2-22
!boundary_line_on                               P2-23
!color_system_type                              P2-24
!fixed_range_on = 1                             P2-25
!range_value = -1.E-2, 1.E-2                    P2-26

Common Data List<P1-1 - P1-19>

No.	Keywords	Types	Contents
P1-0	`!VISUAL`		Specification of the visualization method
P1-1	`surface_num`		No. of surfaces in one surface rendering
P1-2	`surface`		Setting of the contents of surface
P1-3	`surface_style`	integer	Specification of the surface type (Default: 1) 1: Boundary surface 2: Isosurface 3: Curved surface defined by user based on the equation
P1-4	`display_method`	integer	Display method (Default: 1) 1. Color code display 2. Boundary line display 3. Color code and boundary line display 4. Display of 1 specified color 5. Isopleth line display by classification of color
P1-5	`color_comp_name`	character(100)	Compatible with parameter name and colormap (Default: 1st parameter name)
P1-6	`color_subcomp_name`	character(4)	When the parameter is a vector, specifies the component to be displayed. (Default: x) norm: Norm of the vector x: x component y: y component z: z component
P1-7	`color_comp`	integer	Provides an ID number to the parameter name (Default: 0)
P1-8	`color_subcomp`	integer	When the degree of freedom of the parameter is 1 or more, specifies the degree of freedom number to be displayed. 0: Norm (Default: 1)
P1-9	`iso_number`	integer	Specifies the number of isopleth lines. (Default:5)
P1-10	`specified_color`	real	Specified the color when the `display_method = 4` 0.0 < specified_color < 1.0
P1-11	`!deform_display_on`	integer	Specifies the existence of deformation. 1: On, 0: Off (Default: 0)
P1-12	`!deform_comp_name`	character(100)	Specifies the attribution to be adopted when specifying deformation. (Default: Parameter called DISPLCEMENT)
P1-13	`!deform_ comp`	integer	ID number of the parameter when specifying deformation. (Default: 0)
P1-14	`!deform_scale`	real	Specifies the displacement scale when displaying deformation. Default:Auto `standard_scale` = 0.1 * sqrt(`x_range`² + `y_range`² + `z_range`²) / `max_deform` `user_defined`: `real_scale` = `standard_scale` * `deform_scale`
P1-15	`!initial_style`	integer	Specifies the type of deformation display.(Default: 1) 0: Not specified 1: Solid line mesh(Displayed in blue if not specified) 2: Gray filled pattern 3: Shading (Let the physical attributions respond to the color) 4: Dotted line mesh (Displayed in blue if not specified)
P1-16	`!deform_style`	integer	Specifies the shape display style after the initial deformation.(Default: 4) 0: Not specified 1: Solid line mesh (Displayed in blue if not specified) 2: Gray filled pattern 3: Shading (Let the physical attributions respond to the color) 4: Dotted line mesh (Displayed in blue if not specified)
P1-17	`!initial_line_color`	real (3)	Specifies the color when displaying the initial mesh. This includes both the solid lines and dotted lines. (Default: Blue(0.0, 0.0, 1.0))
P1-18	`!deform_line_color`	real (3)	Specifies the color when displaying the deformed mesh. This includes both the solid lines and dotted lines. (Yellow(1.0, 1.0, 0.0))
P1-19	`output_type`	character(3)	Specifies the type of output file. (Default: AVS) `AVS`: UCD Data for AVS(only on object surface) `BMP`: Image data (BMP format) `COMPLETE_AVS`: UCD data for AVS `COMPLETE_REORDER_AVS`: Rearranges the node and element ID `SEPARATE_COMPLETE_AVS`: For each decomposed domain `COMPLETE_MICROAVS`: Outputs the physical value scalar `FSTR_FEMAP_NEUTRAL`: Neutral file for FEMAP

Rendering Data List <P2-1 - P2-26>

(Valid only when the output_type=BMP)

	Keywords	Types	Contents
P2-1	`x_resolution`	integer	Specifies the width of final figure. (Default: 512)
P2-2	`y_resolution`	integer	Specifies the height of final figure. (Default: 512)
P2-3	`num_of_lights`	integer	Specifies the number of lights. (Default: 1)
P2-4	`position_of_lights`	real(:)	Specifies the position of the lights by coordinates.(Default: Directly above front) Specification method `!position_of_lights= x, y, z, x, y, z,...` Ex) `!position_of_lights=100.0, 200.0, 0.0`
P2-5	`viewpoint`	real(3)	Specifies the viewpoint position by coordinates. (Default: x = (x_min + x_max)/2.0) y = y_min + 1.5 ( y_max - y_min) z = z_min + 1.5 ( z_max - z_min) )
P2-6	`look_at_point`	real(3)	Specifies the look at point position. (Default: Center of data)
P2-7	`up_direction`	real(3)	Defines the view frame at Viewpoint, `look_at_point` and `up_direction` (Default: 0.0, 0.0, 1.0)
P2-8	`ambient_coef`	real	Specifies the peripheral brightness. (Default: 0.3)
P2-9	`diffuse_coef`	real	Specifies the intensity of the diffused reflection light by coefficient. (Default: 0.7)
P2-10	`specular_coef`	real	Specifies the intensity of specular reflection by coefficient. (Default: 0.6)
P2-11	`color_mapping_style`	integer	Specifies the color mapping style. (Default: 1) 1: Complete linear mapping (Maps overall color in RGB linear) 2: Clip linear mapping (Maps from `mincolor` to `maxcolor` in the RGB color space) 3: Nonlinear color mapping (Patitions all domains into multiple sections, and performs linear mapping for each section) 4: Optimum auto adjustment (Performs a statistical process of the data distribution to determine the color mapping)
P2-12	`interval_mapping_num`	integer	Specifies the number of sections when the `color_mapping_style = 3`
P2-13	`interval_mapping`	real(:)	Specifies the section position and color number when the `color_mapping_style = 2` or `3`. if the `color_mapping_style=2`; `!interval_mapping=[minimum color], [maximum color]` If the `color_mapping_style=3`; `!interval_mapping=[section,compatible color value],... repeats number specified` Note: Must be describe in one line.
P2-14	`rotate_style`	integer	Specifies the rotating axis of animation. 1: Rotates at x-axis. 2: Rotates at y-axis. 3: Rotates at z axis. 4: Particularly, specifies the viewpoint to perform animation. (8 frames)
P2-15	`rotate_num_of_frames`	integer	Specifies the cycle of animation. (`rotate_style` = 1, 2, 3) (Default: 8)
P2-16	`color_mapping_bar_on`	integer	Specifies the existence of color mapping bar. 0: off; 1: on; Default: 0
P2-17	`scale_marking_on`	integer	Specifies whether to display the value on the color mapping bar. 0: off; 1: on; Default: 0
P2-18	`num_of_scale`	integer	Specifies the number of memories of the color bar. (Default: 3)
P2-19	`font_size`	real	Specifies the font size when displaying the value of the color mapping bar. Range: 1.0-4.0 (Default: 1.0)
P2-20	`font_color`	real(3)	Specifies the display color when displaying the value of the color mapping bar. (Default: 1.0, 1.0, 1.0 (White))
P2-21	`background_color`	real(3)	Specifies the background color. (Default: 0.0, 0.0, 0.0 (Black))
P2-22	`isoline_color`	real(3)	Specifies the color of the isopleth line. (Default: Same color as the value)
P2-23	`boundary_line_on`	integer	Specifies whether to display the zone of the data. 0: off; 1: on; Default: 0
P2-24	`color_system_type`	integer	Specifies the color mapping style. (Default: 1) 1: (Blue - Red)(in ascending order) 2: Rainbow mapping (Ascending order from red to purple) 3: (Black - White)(in ascending order)
P2-25	`fixed_range_on`	integer	Specifies whether to maintain the color mapping style for other time steps. 0: off; 1: on; (Default: 0)
P2-26	`range_value`	real(2)	Specifies the section.

Data List by Setting Values of `surface_style`

In the case of isosurface (`surface_style=2`)

	Keywords	Types	Contents
P3-1	`data_comp_name`	character(100)	Provides the name to the attribution of the isosurface.
P3-2	`data_subcomp_name`	character(4)	When the parameter is a vector, specifies the component to be displayed. (Default: x) norm: Norm of the vector x: x component y: y component z: z component
P3-3	`data_comp`	integer	Provides an ID number to the parameter name (Default: 0)
P3-4	`data_subcomp`	integer	When the degree of freedom of the parameter is 1 or more, specifies the degree of freedom number to be displayed. 0: Norm (Default: 1)
P3-5	`iso_value`	real	Specifies the value of the isosurface.

In the case of a curved surface (surface_sytle = 3) specified by the equation of the user

	Keywords	Types	Contents
P4-1	method	integer	Specifies the attribution of the curved surface. (Default: 5) 1: Spherical surface 2: Ellipse curved surface 3: Hyperboloid 4: Paraboloid 5: General quadric surface
P4-2	point	real(3)	Specifies the coordinates of the center when method = 1, 2, 3, or 4 (Default: 0.0, 0.0, 0.0)
P4-3	radius	real	Specifies the radius when method = 1 (Default: 1.0)
P4-4	length	real	Specifies the length of the diameter when method = 2, 3, or 4. Note: The length of one diameter in the case the ellipse curved surface is 1.0.
P4-5	coef	real	Specifies the coefficient of a quadric surface when method=5. coef[1]x² + coef[2]y² + coef[3]z² + coef[4]xy + coef[5]xz + coef[6]yz + coef[7]x + coef[8]y + coef[9]z + coef[10]=0 Ex: coef=0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 1.0, 0.0, -10.0 This means the plain surface of y=10.0

Details of Analysis Control Data Parameters

The details of each parameter explained in item 7.3 are described in the following.

The analysis control data is classified as follow.

Common control data
Control data for static analysis
Control data for eigenvalue analysis
Control data for heat conduction analysis
Control data for dynamic analysis
Solver control data
Post process (visualization) control data

Common Control Data

(1) `!VERSION` (1-1)

Specifies the solver version number. The current version number is 5.

Example of Use

!VERSION
 5

(2) `!SOLUTION` (1-2)

Specifies the type of analysis.

Parameter

TYPE=
     STATIC      : Linear static analysis
     NLSTATIC    : Nonlinear static analysis (same as TYPE=STATIC, NONLINEAR)
     HEAT        : Heat conduction analysis
     EIGEN       : Eigenvalue analysis
     DYNAMIC     : Dynamic analysis
     STATICEIGEN : Nonlinear static analysis &rarr; Eigenvalue analysis
     ELEMCHECK   : Element shape check
NONLINEAR        : Consider Nonlinearity（only available when TYPE=STATIC/DYNAMIC ）

Example of Use

Linear static analysis

!SOLUTION, TYPE=STATIC

Nonlinear static analysis

!SOLUTION, TYPE=STATIC, NONLINEAR

(3) `!WRITE, VISUAL` (1-3)

Specifies the output data by the visualizer via memory.

Parameter

FREQUENCY = step interval of output (Default: 1)

Example of Use

!WRITE, VISUAL, FREQUENCY=2

(4) `!WRITE, RESULT` (1-4)

Specifies the output of the analysis results file.

Parameter

FREQUENCY = step interval of output (Default:1)

Example of Use

!WRITE, RESULT, FREQUENCY=2

(5) `!WRITE, LOG` (1-5)

Specifies the step interval for output to the log file.

Parameter

FREQUENCY = step interval of output (Default:1)

Example of Use

!WRITE, LOG, FREQUENCY=2

(6) `!OUTPUT_VIS` (1-6)

Output item control of the visualization

!WRITE, VISUAL must be specified

Parameter

N/A

2nd Line or later

(2nd line or later) Parameter name, ON/OFF

The following parameter names can be specified.

Parameter Names	Physical Values
`DISP`	Displacement (Default output)
`ROT`	Rotation (Only for 781,761 shell)
`REACTION`	Reaction force of nodes
`NSTRAIN`	Strain of nodes
`NSTRESS`	Stress of nodes (Default output)
`NMISES`	Mises stress of nodes (Default output)
`TH_NSTRAIN`	Thermal strain of nodes (Not included)
`VEL`	Velocity
`ACC`	Acceleration
`TEMP`	Temperature
`PRINC_NSTRESS`	Nodal principal stress(Scalar value)
`PRINCV_NSTRESS`	Nodal principal stress(Vector value)
`PRINC_NSTRAIN`	Nodal principal strain(Scalar value)
`PRINCV_NSTRAIN`	Nodal principal strain(Vector value)
`SHELL_LAYER`	Output per layer of layerd shell element
`SHELL_SURFACE`	Output of surface information of shell element
`CONTACT_NFORCE`	Contact normal force(Vector value)
`CONTACT_FRICTION`	Contact friction force(Vector value)
`CONTACT_RELVEL`	Contact relative displacement (Vector value / slave point only)
`CONTACT_STATE`	Contact state(Scalar value / -1, 0, 1 and 2 means free, undefined, stick and slip respectively)
`CONTACT_NTRACTION`	Contact normal traction(Vector value)
`CONTACT_FTRACTION`	Contact friction traction(Vector value)

Example of Use

!OUTPUT_VIS
  NSTRAIN, ON
  NSTRESS, OFF

(7) `!OUTPUT_RES` (1-7)

Output item control of the result

!WRITE, RESULT must be specified

Parameter

N/A

2nd Line or later

(2nd line or later) Parameter name, ON/OFF

The following parameter names can be specified.

Parameter Names	Physical Values
`DISP`	Displacement (Default output)
`ROT`	Rotation (Only for 781,761 shell)
`REACTION`	Reaction force of nodes
`NSTRAIN`	Strain of nodes
`NSTRESS`	Stress of nodes (Default output)
`NMISES`	Mises stress of nodes (Default output)
`ESTRAIN`	Strain of elements
`ESTRESS`	Stress of elements (Default output)
`EMISES`	Mises stress of elements (Default output)
`ISTRAIN`	Strain of integration points
`ISTRESS`	Stress of integration points
`PL_ISTRAIN`	Plastic strain of integration points
`TH_NSTRAIN`	Thermal strain of nodes (Not included)
`TH_ESTRAIN`	Thermal strain of elements (Not included)
`TH_ISTRAIN`	Thermal strain of integration points (Not included)
`VEL`	Velocity
`ACC`	Acceleration
`TEMP`	Temperature
`PRINC_NSTRESS`	Nodal principal stress(Scalar value)
`PRINCV_NSTRESS`	Nodal principal stress(Vector value)
`PRINC_NSTRAIN`	Nodal principal strain(Scalar value)
`PRINCV_NSTRAIN`	Nodal principal strain(Vector value)
`PRINC_ESTRESS`	Elemental principal stress(Scalar value)
`PRINCV_ESTRESS`	Elemental principal stress(Vector value)
`PRINC_ESTRAIN`	Elemental principal strain(Scalar value)
`PRINCV_ESTRAIN`	Elemental principal strain(Vector value)
`SHELL_LAYER`	Output per layer of layerd shell element
`SHELL_SURFACE`	Output of surface information of shell element
`CONTACT_NFORCE`	Contact normal force(Vector value)
`CONTACT_FRICTION`	Contact friction force(Vector value)
`CONTACT_RELVEL`	Contact relative displacement (Vector value / slave point only)
`CONTACT_STATE`	Contact state(Scalar value / -1, 0, 1 and 2 means free, undefined, stick and slip respectively)
`CONTACT_NTRACTION`	Contact normal traction(Vector value)
`CONTACT_FTRACTION`	Contact friction traction(Vector value)

Example of Use

! OUTPUT_RES
ESTRESS, OFF
ISTRESS, ON

(8) `!RESTART` (1-8)

Controls the writing of the restart file. When not specified, the restart file can not be written.

Parameter

FREQUENCY = n        :step interval of output (Default: 0)
            n > 0    :Output for each n step
            n < 0    :First, reads the restart file, then outputs for each n step

Example of Use

!RESTART, FREQUENCY=-2

(9) `!ECHO` (1-9)

Outputs the node data, element data and material data to the log file.

Parameter

N/A

(10) `!ORIENTATION` (1-10)

Definition of local coordinate system

Parameter

NAME = Name of local coordinate system
DEFINITION = COORDINATES (Default)/NODES

2nd Line of later

In case of DEFINTION=COORDINATES

(2nd line or later) a1, a2, a3, b1, b2, b3, c1, c2, c3

In case of DEFINTIION=NODES

(2nd line or later) a, b, c

Parameter Name	Attributions	Contents
a1, a2, a3	R	coodinate of point a
b1, b2, b3	R	coodinate of point b
c1, c2, c3	R	coodinate of point c
a,b,c	I	Node ID of a,b,c, respectively

Analysis Control Data

(11) `!SECTION` (1-11)

Definition of local coordinate system the sction correspondent to.

Parameter

SECNUM = Index of section defined in M1-10 in chapter 6.3.
ORIENTATION = Name of local coordinate system defined in (1-10) above.
FORM361 = FBAR (Default in nonlinear analysis)/IC (Default in linear analysis)/BBAR/FI
FORM341 = FI (Default)/SELECTIVE_ESNS(smoothed element)

2nd Line or later

N/A

(12) `!INITIAL_CONDITION` (1-12)

Definition of initial condition

Parameter

TYPE = TEMPERATURE/VELOCITY/ACCELERATION

# In case of `TYPE = TEMPERATURE`

(2nd line) ng1, t1

(3rd line or later) ng2, t2

...

Parameter Name	Attributions	Contents
ng1,ng2, ...	C/I	name of node group/index of node
t1, t2, ...	R	temperature

# In case of `TYPE= VELOCITY/ACCELERATION`

(2nd line) ng1, dof1, v1

(3rd line or later) ng2, dof2, v2

...

Parameter Name	Attributions	Contents
ng1,ng2, ...	C/I	name of node group/index of node
dof1, dof2, ...	I	dof number(1-6)
v1, v2, ...	R	velocity/acceleration

(13) `!END` (1-13)

Displays the end of the control data.

Parameter

N/A

Control Data for Static Analysis

(1) `!STATIC` (2-1)

Performs the static analysis. (Default: omissible)

Parameter

N/A

(2) `!MATERIAL` (2-2)

Definition of material physical properties

The definition of the material physical properties is used in a set with the !MATERIAL and the !ELASTIC, !PLASTIC and etc. entered next. The !ELASTIC, !PLASTIC and etc. entered before !MATERIAL will be disregarded.

Note: When the !MATERIAL is defined in the analysis control data, the !MATERIAL definition in the mesh data will be disregarded. When the !MATERIAL is not defined in the analysis control data, the !MATERIAL definition in the mesh data is used.

Parameter

NAME = Material name

(3) `!ELASTIC` (2-2-1)

Definition of elastic material

Parameter

TYPE = ISOTROPIC (Default)/ ORTHOTROPIC / USER
DEPENDENCIES = 0 (Default)/1
INFINITESIMAL    When specified, infinitesimal deformation is assumed

2nd Line or later

In the case of TYPE = ISOTROPIC

(2nd Line) YOUNGS, POISSION, Temperature

Parameter Name	Attributions	Contents
YOUNGS	R	Young's Modulus
POISSON	R	Poisson's Ratio
Temperature	R	Temperature (required when DEPENDENCIES = 1)

In case of TYPE=ORTHOTROPIC

(2nd Line) E1, E2, E3, ν12, ν13, ν23, G12, G13, G23, Temperature

$\begin{equation} \begin{bmatrix} \varepsilon\_{11} \\\ \varepsilon\_{22} \\\ \varepsilon\_{33} \\\ 2\varepsilon\_{12} \\\ 2\varepsilon\_{23} \\\ 2\varepsilon\_{31} \end{bmatrix} = \begin{bmatrix} 1/E_1 & -\nu\_{12}/E_1 & -\nu\_{13}/E_1 & 0 & 0 & 0 \\\ & 1/E_2 & -\nu\_{23}/E_2 & 0 & 0 & 0 \\\ & & 1/E_3 & 0 & 0 & 0 \\\ & & & 1/G\_{12} & 0 & 0 \\\ & Symmetric & & & 1/G\_{23} & 0 \\\ & & & & & 1/G\_{31} \end{bmatrix} \begin{bmatrix} \sigma\_{11} \\\ \sigma\_{22} \\\ \sigma\_{33} \\\ \sigma\_{12} \\\ \sigma\_{23} \\\ \sigma\_{31} \end{bmatrix} \end{equation}$

In the case of TYPE=USER

(2nd line - 10th line)v1, v2, v3, v4, v5, v6, v7, v8, v9, v10

(4) `!PLASTIC` (2-2-2)

Definition of plastic material

!PLASTIC must be defined together with !ELASTIC.

Parameter

YIELD        = MISES (Default), Mohr-Coulomb, DRUCKER-PRAGER, USER
HARDEN       = BILINEAR (Default), MULTILINEAR, SWIFT, RAMBERG-OSGOOD,
               KINEMATIC, COMBINED
DEPENDENCIES = 0 (Default)/1
INFINITESIMAL    When specified, infinitesimal deformation is assumed

2nd line or later

# In case of `YIELD = MISES` (Default)

In case of HARDEN = BILINEAR (Default)

(2nd line) YIELD0, H

In case of HARDEN = MULTILINEAR

(2nd line) YIELD, PSTRAIN, Temperature
(3rd line) YIELD, PSTRAIN, Temperature

...continues

In case of HARDEN = SWIFT

(2nd line) $\epsilon$0, K, n

In case of HARDEN = RAMBERG-OSGOOD

(2nd line) $\epsilon$0, D, n

In case of HARDEN = KINEMATIC

(2nd line) YIELD0, C

In case of HARDEN = COMBINED

(2nd line) YIELD0, H, C

# In case of `YIELD =` Mohr-Coulomb or Drucker-Prager

In case of HARDEN = BILINEAR(Default)

(2nd line) c, $\phi$, H, $\psi$

In case of HARDEN = MULTILINEAR

(2nd line) $\phi$, $\psi$
(3nd line) c, PSTRAIN
(4th line) c, PSTRAIN
...continues

HARDEN =others will be disregarded, becomes the default (BILINEAR).

Parameter Name	Attributions	Contents
YIELD0	R	Initial yield stress
H	R	Hardening factor
PSTRAIN	R	Plastic strain
YIELD	R	Yield stress
$\varepsilon0, K, n$	R	$\overline{\sigma} = k\left( \varepsilon_{0} + \overline{\varepsilon} \right)^{n}$
$\varepsilon0, D, n$	R	$\varepsilon = \frac{\sigma}{E} + \varepsilon_{0}\left( \frac{\sigma}{D} \right)^{n}$
$\phi$	R	Angle of internal friction
$\psi$	R	Dilatancy angle (Default: same value as $\phi$)
c	R	Cohesion
C	R	Linear motion hardening factor
Tempearture	R	Temperature (required when `DEPENDENCIES = 1`)
v1, v2...v10	R	Material constant

In the case of YIELD= USER

(2nd Line or later) v1, v2, v3, v4, v5, v6, v7, v8, v9, v10

Example of Use

!PLASTIC, YIELD=MISES, HARDEN=MULTILINEAR, DEPENDENCIES=1
  276.0, 0.0, 20.
  296.0, 0.0018, 20.
  299.0, 0.0053, 20.
  303.0, 0.008, 20.
  338.0, 0.0173, 20.
  372.0, 0.0271, 20.
  400.0, 0.037, 20.
  419.0, 0.0471, 20.
  437.0, 0.0571, 20.
  450.0, 0.0669, 20.
  460.0, 0.0767, 20.
  469.0, 0.0867, 20.
  477.0, 0.0967, 20.
  276.0, 0.0, 100.
  276.0, 0.0018, 100.
  282.0, 0.0053, 100.
  295.0, 0.008, 100.
  330.0, 0.0173, 100.
  370.0, 0.0271, 100.
  392.0, 0.037, 100.
  410.0, 0.0471, 100.
  425.0, 0.0571, 100.
  445.0, 0.0669, 100.
  450.0, 0.0767, 100.
  460.0, 0.0867, 100.
  471.0, 0.0967, 100.
  128.0, 0.0, 400.
  208.0, 0.0018, 400.
  243.0, 0.0053, 400.
  259.0, 0.008, 400.
  309.0, 0.0173, 400.
  340.0, 0.0271, 400.
  366.0, 0.037, 400.
  382.0, 0.0471, 400.
  396.0, 0.0571, 400.
  409.0, 0.0669, 400.
  417.0, 0.0767, 400.
  423.0, 0.0867, 400.
  429.0, 0.0967, 400.

The work hardening coefficient will be calculated by inserting the data from the above inputdata, regarding the specified temperature or plastic strain. It is necessary to input the same PSTRAIN array for each temperature.

(5) `!HYPERELASTIC` (2-2-3)

Definition of hyperelastic material

Parameter

TYPE = NEOHOOKE (Default)
       MOONEY-RIVLIN
       ARRUDA-BOYCE
       MOONEY-RIVLIN-ANISO
       USER

2nd Line or later

# In the case of `TYPE = NEOHOOKE`

(2nd line) C₁₀, D

Parameter Name	Attributions	Contents
C₁₀	R	Material constant
D	R	Material constant

# In case of `TYPE = MOONEY-RIVLIN`

(2nd line) C₁₀, C₀₁, D

Parameter Name	Attributions	Contents
C₁₀	R	Material constant
C₀₁	R	Material constant
D	R	Material constant

# In case of `TYPE = ARRUDA-BOYCE`

(2nd line) mu, lambda_m, D

Parameter Name	Attributions	Contents
mu	R	Material constant
lambda_m	R	Material constant
D	R	Material constant

# `TYPE = MOONEY-RIVLIN-ANISO`の場合

(2nd line) C₁₀, C₀₁, D, C₄₂, C₄₃

変数名	属性	内容
C₁₀	R	Material constant
C₀₁	R	Material constant
D	R	Material constant
C₄₂	R	Material constant
C₄₃	R	Material constant

# In case of `TYPE = USER`

(2nd line-10th line) v1, v2, v3, v4, v5, v6, v7, v8, v9, v10

(6) `!VISCOELASTIC` (2-2-4)

Definition of viscoelastic material

!VISCOELASTIC must be defined together with !ELASTIC.

Parameter

DEPENDENCIES = the number of parameters depended upon (Not included)
INFINITESIMAL    When specified, infinitesimal deformation is assumed

2nd Line or later

(2nd line) g, t

Parameter Name	Attributions	Contents
g	R	Shear relaxation modulus
t	R	Relaxation time

(7) `!CREEP` (2-2-5)

Definition of creep material

!CREEP must be defined together with !ELASTIC.

Parameter

TYPE = NORTON (Default)
DEPENDENCIES = 0 (Default) / 1

2nd Line or later

(2nd line) A, n, m, Tempearature

Parameter Name	Attributions	Contents
A	R	Material modulus
n	R	Material modulus
m	R	Material modulus
Tempearture	R	Temperature(required when `DEPENDENCIES=1`)

(8) `!DENSITY` (2-2-6)

Definition of mass density

Parameter

DEPENDENCIES = the number of parameters depended upon (Not included)

2nd Line or later

(2nd line) density

Parameter Name	Attributions	Contents
density	R	Mass density

(9) `!EXPANSION_COEFF` (2-2-7)

Definition of coefficient of linear expansion

The coefficient to be input here is not the coefficient of linear expansion $\alpha$ at each temperature, but its averaged value between the reference temperature $T_{ref}$ and each temperature $T$ as follows:

$\begin{equation} \overline{\alpha}(T)=\frac{1}{T-T_{ref}} \int_{T_{ref}}^T \alpha(T) dT \end{equation}$

Parameter

TYPE = ISOTROPIC(Default) / ORTHOTROPIC
DEPENDENCIES = 0(Default) / 1

2nd Line or later

# In case of `TYPE=ISOTROPIC`

(2nd line) expansion, Temperature

# In case of `TYPE=ORTHOTROPIC`

(2nd line) $\alpha$11, $\alpha$22, $\alpha$33, Temperature

Parameter Name	Attributions	Contents
expansion	R	Coefficient of thermo expansion
$\alpha$11, $\alpha$22, $\alpha$33	R	Coefficient of thermo expansion
Tempearture	R	Temperature (required when DEPENDENCIES = 1)

(10) `!TRS` (2-2-8)

Thermorheological Simplicity description on temperature behavior of viscoelastic materials

This definition must be placed after !VISCOELASTIC. If not, this definition will be ignored.

Parameter

DEFINITION = WLF(Default) /ARRHENIUS

2nd line or later

(2nd line) $\theta_0$, C₁, C₂

Parameter Name	Attributions	Contents
$\theta_0$	R	Reference temperature
C₁, C₂	R	Material constants

(11) `!FLUID` (2-2-9)

Definition of flow condition

Parameter

TYPE = INCOMP_NEWTONIAN (Default)

2nd Line or later

(2nd line) mu

Parameter Name	Attributions	Contents
mu	R	Viscosity

(12) `!USER_MATERIAL` (2-2-10)

Input of user defined material

Parameter

NSTATUS = Specifies the number of state variables of material (Default: 1)

2nd line or later

(2nd line-10th line) v1, v2, v3, v4, v5, v6, v7, v8, v9, v10

(13) `!BOUNDARY` (2-3)

Definition of displacement boundary conditions

Parameter

GRPID      = Group ID
AMP        = Time function name (Specified in !AMPLITUDE, valid in dynamic analysis)
ROT_CENTER = Node number of rotational constraint or node group name. 
             When specified it, this `!BOUNDARY` is recognized as rotational constraint. 
TOTAL        When specified, the displacements are treated as total displacements from
             the initial configuration (Default is relative displacements from the
             configuration at the beginning of the step)

2nd line or later

(2nd line) NODE_ID, DOF_idS, DOF_idE, Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
DOF_idS	I	Start No. of restricted degree of freedom
DOF_idE	I	End No. of restricted degree of freedom
Value	R	Restricted value (Default: 0)

Example of Use

!BOUNDARY, GRPID=1
  1, 1, 3, 0.0
  ALL, 3, 3,

Note: Resricted value is 0.0

(14) `!SPRING` (2-3-1)

Definition of spring boundary conditions

Parameter

GRPID = Group ID

2nd line or later

(2nd line) NODE_ID, DOF_id, Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
DOF_id	I	Restricted degree of freedom
Value	R	Spring constant

Example of Use

!SPRING, GRPID=1
  1, 1, 0.5

(15) `!CLOAD` (2-4)

Definition of concentrated load

Parameter

GRPID      = Group ID
AMP        = Time function name (Specified in !AMPLITUDE, valid in dynamic analysis)
ROT_CENTER = Node number of rotational constraint or node group name.
             When specified it, this `!CLOAD` is recognized as load of torque.

2nd line or later

(2nd line) NODE_ID, DOF_id, Value

Parameters	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
DOF_id	I	Degree of freedom No.
Value	R	Load value

Example of Use

!CLOAD, GRPID=1
  1, 1, 1.0e3
  ALL, 3, 10.0
!CLOAD, ROT_CENTER=7, GRPID=1
  TORQUE_NODES, 1, 3
  TORQUE_NODES, 3, -4

(16) `!DLOAD` (2-5)

Definition of distributed load

Parameter

GRPID = Group ID
AMP = Time Function Name (Specified in !AMPLITUDE, valid in dynamic analysis)
FOLLOW = YES(Default) / NO
         (whether pressure load follow deformation, valid in finite displacement analysis)

2nd Line or later

(2nd line) ID_NAME, LOAD_type, param1, param2,...

Parameter Name	Attributions	Contents
ID_NAME	I/C	Surface group name, element group name, or element ID
LOAD_type	C	Load type No.
param*	R	Load parameter (refer to following)

# Load Parameters

Load Type No.	Types	No. of Parameters	Parameter Array & Meaning
S	Applies pressure to surface specified in the surface group	1	Pressure value
P0	Applies pressure to shell element	1	Pressure value
PX	Pressure to shell element along X direction	1	Pressure value
PY	Pressure to shell element along Y direction	1	Pressure value
PZ	Pressure to shell element along Z direction	1	Pressure value
P1	Applies pressure to 1st surface	1	Pressure value
P2	Applies pressure to 2nd surface	1	Pressure value
P3	Applies pressure to 3rd surface	1	Pressure value
P4	Applies pressure to 4th surface	1	Pressure value
P5	Applies pressure to 5th surface	1	Pressure value
P6	Applies pressure to 6th surface	1	Pressure value
BX	Body force in X direction	1	Body force value
BY	Body force in Y direction	1	Body force value
BZ	Body force in Z direction	1	Body force value
GRAV	Gravity	4	Gravitaional acceleration, gravity direction cosine
CENT	Centrifugal force	7	Angular velocity, position vector at a point on the rotation axis, vector in the rotating axis direction

# Example of Use

!DLOAD, GRPID=1
  1, P1, 1.0
  ALL, BX, 1.0
  ALL, GRAV, 9.8, 0.0, 0.0, -1.0
  ALL, CENT, 188.495, 0.0, 0.0, 0.0, 0.0, 0.0, 1.0

(17) `!ULOAD` (2-6)

Input of user definition load

Parameter

FILE = file name (Mandatory)

(18) `!CONTACT_ALGO` (2-7)

Specification of the contact analysis algorithm

Parameter

TYPE = SLAGRANGE (Lagrange multiplier method)
       ALAGRANGE (Extended Lagrange multiplier method)

(19) `!CONTACT` (2-8)

Definition of contact conditions

Parameter

GRPID       = Boundary conditions group ID
INTERACTION = SSLID (Infinitesimal slip contact, Default) / FSLID (Finite slip contact) / TIED (Tied)
NTOL        = Contact normal direction convergence threshold (Default: 1.e-5)
TTOL        = Contact tangential direction convergence threshold (Default: 1.e-3)
NPENALTY    = Contact normal direction Penalty (Default: stiffness matrix 1.e3)
TPENALTY    = Contact tangential direction Penalty (Default: 1.e3)
CONTACTPARAM = Contact scan parameter set name（specified by `!CONTACT_PARAM, NAME`）

2nd line or later

# Using `INTERACTION = SSLID, FSLID`

(2nd line) PAIR_NAME, fcoef, factor

Parameter Name	Attributions	Contacts
PAIR_NAME	C	Contact pair name (Defined in `!CONTACT_PAIR`)
fcoef	R	Friction coefficient (Default: 0.0)
factor	R	Friction penalty stiffness

# Using `INTERACTION = TIED`

(2nd line) PAIR_NAME

Parameter Name	Attributions	Contacts
PAIR_NAME	C	Contact pair name (Defined in `!CONTACT_PAIR`)

Example of Use

!CONTACT_ALGO, TYPE=SLAGRANGE
!CONTACT, GRPID=1, INTERACTION=FSLID
  CP1, 0.1, 1.0e+5

# Note

if CONTACTPARAM is specified, the destination !CONTACT_PARAM must be defined prior to the !CONTACT card. If this parameter is omitted, the default contact scan parameter set is used.

(20) `!TEMPERATURE` (2-9)

Specification of nodal temperature used for thermal stress analysis

Parameter

READRESULT = Number of result steps of heat conduction analysis.
             When specified, the temperature is sequentially input from
             the results file of the heat conduction analysis,
             and the 2nd line and later will be disregarded.
SSTEP      = First step number that performs the reading
             of the heat conduction analysis results (Default: 1)
INTERVAL   = Step interval that performs the reading
             of the heat conduction analysis results (Default: 1)
READTYPE   = STEP(Default) / TIME
             When TIME is specified, analysis time of the stress
             analysis is synchronized with the heat conduction
             analysis (value of INTERVAL is ignored, and the
             temperature is linearly interpolated from results of the
             heat conduction analysis right before and after the
             current analysis time)

When unsteady heat conduction analysis using auto time increment was performed, and the results were output at specified time points using !TIME_POINTS, READTYPE=TIME needs to be specified because the step interval of the results is not constant.

2nd line or later

(2nd line) NODE_ID, Temp_Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
Temp_Value	R	Temperature (Default: 0)

Example of Use

!TEMPERATURE
  1, 10.0
  2, 120.0
  3, 330.0
!TEMPERATURE
  ALL, 20.0
!TEMPERATURE, READRESULT=1, SSTEP=1

(21) `!REFTEMP` (2-10)

Definition of reference temperature in thermal stress analysis

Parameter

N/A

2nd line or later

(2nd line) Value

Parameter Name	Attributions	Contents
Value	R	Reference temperature (Default: 0)

(22) `!STEP` (2-11)

Analysis step settings

Required for nonlinear static and nonlinear dynamic analysis

If you omit this definition for any analysis other than the above, all boundary conditions are in effect and the calculation is done in one step

If the material properties are visco-elasticity and creep, specify TYPE=VISCO and set the calculation time condition to

Parameter

TYPE     = STATIC (default)/VISCO (quasi-static analysis)
SUBSTEPS = Number of substeps of the boundary conditions (Default: 1)
CONVERG  = Convergence threshold (Default: 1.0e-6)
MAXITER  = Maximum number of iterations in nonelinear analysis (Default: 50)
AMP      = Time function name (specified in !AMPLITUDE)
INC_TYPE = FIXED (fixed increment, default) / AUTO (automatic increment)
MAXRES   = Setting of maximum allowable residuals (default: 1.0e+10)
TIMEPOINTS = Name of the time list (specified by `!TIME_POINTS, NAME`)
AUTOINCPARAM = auto-incremental parameter set name (specified by `!AUTOINC_PARAM, NAME`)
MAXCONTITER = Maximum number of contact iterations in contact analysis (default: 10)

2nd line or later

In case of INC_TYPE=FIXED (If TYPE=STATIC, it can be omitted.)

(2nd line) DTIME, ETIME

Parameter Name	Attribution	Contents
DTIME	R	Time increment value (Default: 1/SUBSTEPS)
ETIME	R	End value of time increment in this step (Default: 1)

In case of INC_TYPE=AUTO (regardless of TYPE)

(2nd line) DTIME_INIT, ETIME, MINDT, MAXDT

Parameter Name	Attribution	Contents
DTIME_INIT	R	Initial time increment
ETIME	R	Step time width
MINDT	R	Lower limit of time increments
MAXDT	R	Maximum limit of time increments

3rd line or later

  BOUNDARY, id          GRPID defined in id=!BOUNDARY
  LOAD, id              GRPID defined in id=!CLOAD, !DLOAD, !SPRING, !TEMPERATURE
  CONTACT, id           GRPID defined in id=!CONTACT

example

# Examples of fixed time increment usage

!STEP, CONVERG=1.E-8
  0.1, 1.0
  BOUNDARY, 1
  LOAD, 1
  CONTACT, 1

Enable automatic incremental adjustment, set the initial time increment to 0.01, step time width to 2.5, lower time increment 1E-5, upper time increment 0.3, and maximum number of sub-steps to 200.

!STEP, INC_TYPE=AUTO, SUBSTEPS=200
   0.01, 2.5, 1E-5, 0.3

Enable automatic incremental adjustment and specify time list TP1 as the calculated and resulting output time

!STEP, INC_TYPE=AUTO, TIMEPOINTS=TP1
    0.1, 2.0, 1E-3, 0.2

# Note

In the case of automatic incremental adjustment, SUBSTEPS is treated as the maximum number of substeps
Time-list name TIMEPOINTS and automatic contact parameter set AUTOINCPARAM are valid only when INC_TYPE=AUTO.
if TIMEPOINTS is specified, the destination !TIME_POINT must be defined before the !STEP card.
if AUTOINCPARAM is specified, the destination !AUTOINC_PARAM must be defined prior to the !STEP card. If this parameter is omitted, the default auto-incremental parameter set is used.

(23) `!AUTOINC_PARAM` (2-12)

Specify auto-incremental parameters.

Parameter

Parameter Name	Attribution	Contents
NAME	C	Automatic incremental parameter name (required)

2nd line

Specify the reduction conditions and the rate of time incremental reduction.

(2nd line) RS, NS_MAX, NS_SUM, NS_COUT, N_S

Parameter Name	Attribution	Contents
RS	R	Time incremantal rate of decline (default:0.25)
NS_MAX	I	Threshold for maximum number of Netwon method iterations (default: 10)
NS_SUM	I	Threshold for the total number of Netwon method iterations (default: 50)
NS_CONT	I	Number of contact iterations threshold (default: 10)
N_S	I	Number of sub-steps until the reduction condition is met (default: 1)

3rd line

Specifies the condition for the increase and the rate of increase of the time increment at that time.

(3rd line) RL, NL_MAX, NL_SUM, NL_COUT, N_L

Parameter Name	Attribution	Contents
RL	R	Incremental rate of increase by time (default:1.25)
NL_MAX	I	Threshold for maximum number of Netwon method iterations (default: 1)
NL_SUM	I	Threshold for the total number of Netwon method iterations (default: 1)
NL_CONT	I	Number of contact iterations threshold (default: 1)
N_L	I	Number of sub-steps until the increase condition is met (default: 2)

4th line

(4th line) RC, N_C

Parameter Name	Attribution	Contents
RC	R	Decrease of time increment at cutback (default: 0.25)
N_C	I	Maximum permissible number of continuous cutbacks (default: 5)

example

With the same settings as the default settings

!AUTOINC_PARAM, NAME=AP1
  0.25, 10, 50, 10, 1
  1.25,  1,  1,  1, 2
  0.25,  5

(24) `!TIME_POINTS` (2-13)

Parameter

Parameter Name	Attribution	Contents
NAME	C	Time list name (required)
TIME	C	STEP (input based on the time from the step start time, default value) / TOTAL (input based on total time from the initial time)
GENERATE	-	Automatic generationi of time points by start time, end time and time interval

2nd line or later

When don't use GENERATE

(2nd line or later) TIME

Parameter Name	Attribution	Contents
TIME	R	time

When using GENERATE

(2nd line) STIME, ETIME, INTERVAL

Parameter Name	Attribution	Contents
STIME	R	start time
ETIME	R	end time
INTERVAL	R	interval between time points

example

Time 1.5, 2.7 and 3.9 are defined as total times without using GENERATE.

!TIME_POINTS, TIME=STEP, GENERATE, NAME=TP1
1.5, 3.9, 1.2

note

The time points must be entered in ascending order.

(25) `!CONTACT_PARAM` (2-14)

Specify contact scan parameter set.

Parameter

Parameter Name	Attribution	Contents
NAME	C	Contact scan parameter set name (required)

2nd line

Specify clearance values in in-surface directions.

(2nd line) CLEARANCE, CLR_SAME_ELEM, CLR_DIFFLPOS, CLR_CAL_NORM

Parameter Name	Attribution	Contents
CLEARANCE	R	ordinary clearance (Default: 1e-4)
CLR_SAME_ELEM	R	clearance for already-in-contct elems (loosen to avoid moving too easily) (Default: 5e-3)
CLR_DIFFLPOS	R	clearance to be recognized as different position (loosen to avoid oscillation) (Default: 1e-2)
CLR_CAL_NORM	R	clearance used when calculating surface normal (Default: 1e-40

3rd line

Specify clearance values in directions vertical to the surface.

(3rd line) DISTCLR_INIT, DISTCLR_FREE, DISTCLR_NOCHECK, TENSILE_FORCE, BOX_EXP_RATE

Parameter Name	Attribution	Contents
DISTCLR_INIT	R	dist clearance for initial scan (Default: 1e-6)
DISTCLR_FREE	R	dist clearance for free nodes (wait until little penetration to be judged as contact) (Default: -1e-6)
DISTCLR_NOCHECK	R	dist clearance for skipping distance check for nodes already in contact (big value to keep contact because contact-to-free is judged by tensile force) (Default: 1.0)
TENSILE_FORCE	R	tensile force to be judged as free node (Default: -1e-8)
BOX_EXP_RATE	R	expansion rate of the box used for contact scan (the smaller the faster, the bigger the safer) (Default: 1.05)

Example of Use

With the same settings as the default settings

!CONTACT_PARAM, NAME=CPARAM1
 1.0e-4,  5.0e-3,  1.0e-2,  1.0e-4
 1.0e-6, -1.0e-6,  1.0,    -1.0e-8,  1.05

`!EMBED` (2-15)

Definition of embedding

Parameters

GRPID = boundary condition group ID

2nd line or later

(2nd line or later) PAIR_NAME

Variable Name	Attribute	Contents
PAIR_NAME	C	embedded pair name (defined in `!EMBED PAIR`)

Example usage

!CONTACT_ALGO, TYPE=SLAGRANGE
!EMBED, GRPID=1
  IP1
!STEP
CONTACT,1

Notes

To enable embedding in a step, specify the GRPID with the keyword “CONTACT” in the data line of the !STEP.

Control Data for Eigenvalue Analysis

(1) `!EIGEN` (3-1)

Parameter settings of eigenvalue analysis

Parameter

N/A

2nd line or later

(2nd line) NGET, LCZTOL, LCZMAX

Parameter Name	Attributions	Contents
NSET	I	No. of eigenvalue
LCZTOL	R	Allowance (Default: 1.0e-8)
LCZMAX	I	Max No. of iterations (Default: 60)

Example of Use

!EIGEN
  3, 1.0e-10, 40

Control Data for Heat Conduction Analysis

(1) `!HEAT` (4-1)

Definition of control data regarding calculation

Parameter

TIMEPOINTS = Time list name (specify with !TIME_POINTS, NAME)

2nd line or later

(2nd line) DT, ETIME, DTMIN, DELTMX, ITMAX, ESP

Parameter Name	Attributions	Contents
DT	R	Initial time increment ≦ 0: Steady calculation > 0: Unsteady calculation
ETIME	R	Unsteady calculation time (mandatory for unsteady calculation)
DTMIN	R	Minimum time increment ≦ 0: Fixed time increment > 0: Auto time increment
DELTMX	R	Allowable change in temperature
ITMAX	I	Maximum number of iterations of nonlinear calculation (Default: 20)
EPS	R	Convergence judgment value (Default: 1.0e-6)

Example of Use

!HEAT
  (No data)               ----- Steady calculation
!HEAT
  0.0                     ----- Steady calculation
!HEAT
  10.0, 3600.0            ----- Fixed time increment unsteady calculation
!HEAT
  10.0, 3600.0, 1.0       ----- Auto time increment unsteady calculation
!HEAT
  10.0, 3600.0, 1.0, 20.0 ----- Auto time increment unsteady calculation

Remarks

Only when performing auto time increment unsteady calculation, TIMEPOINTS parameter can be used to specify time points at which results and/or visualization files are output.

(2) `!FIXTEMP` (4-2)

Definition of fixed temperature

Parameter

AMP = Flux history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) NODE_GRP_NAME, Value

Parameter Name	Attributions	Contents
NODE_GRP_NAME	C/I	Node group name or node ID
Value	R	Temperature (Default: 0)

Example of Use

!FIXTEMP
  ALL, 20.0
!FIXTEMP, AMP=FTEMP
  ALL, 1.0

(3) `!CFLUX` (4-3)

Definition of centralized heat flux given to the node

Parameter

AMP = Flux history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) NODE_GRP_NAME, Value

Parameter Name	Attributions	Contents
NODE_GRP_NAME	C/I	Node group name or node ID
Value	R	Heat flux value

Parameter

!CFLUX
  ALL, 1.0E-3
!CFLUX, AMP=FUX1
  ALL, 1.0

(4) `!DFLUX` (4-4)

Definition of distributed heat flux and internal heat generation given to surface of element

Parameter

AMP = Flux history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) ELEMENT_GRP_NAME, LOAD_type, Value

Paramater Name	Attributions	Contents
ELEMENT_GRP_NAME	C/I	Element group name or element ID
LOAD_type	C	Load type No.
Value	R	Heat flux value

Parameter

!DFLUX
  ALL, S1, 1.0
!DFLUX, AMP=FLUX2
  ALL, S0, 1.0

# Load Parameters

Load Type No.	Applied Surface	Parameter
BF	Element overall	Calorific value
S1	Surface No. 1	Heat flux value
S3	Surface No. 2	Heat flux value
S4	Surface No. 3	Heat flux value
S5	Surface No. 4	Heat flux value
S6	Surface No. 5	Heat flux value
S2	Surface No. 6	Heat flux value
S3	Shell surface	Heat flux value

(5) `!SFLUX` (4-5)

Definition of distributed heat flux by surface group

Parameter

AMP = Flux history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) SURFACE_GRP_NAME, Value

Parameter Name	Attributions	Contents
SURFACE_GRP_NAME	C	Surface group name
Value	R	Heat flux value

Example of Use

!SFLUX
  SURF, 1.0
!SFLUX, AMP=FLUX3
  SURF, 1.0

(6) `!FILM` (4-6)

Definition of heat transfer coefficient given to the boundary plane

Parameter

AMP1 = Heat transfer coefficient history table name (specified in !AMPLITUDE)
AMP2 = Ambient temperature history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) ELEMENT_GRP_NAME, LOAD_type, Value, Sink

Parameter Name	Attributions	Contents
ELEMENT_GRP_NAME	C/I	Element group name or element ID
LOAD_type	C	Load type No.
Value	R	Heat transfer coefficient
Sink	R	Ambient temperature

Example of Use

!FILM
  FSURF, F1, 1.0, 800.0
!FILM, AMP1=TFILM
  FSURF, F1, 1.0, 1.0

# Load Parameters

Load Type No.	Applied Surface	Parameter
F1	Surface No. 1	Heat transfer coefficient and ambient temperature
F2	Surface No. 2	Heat transfer coefficient and ambient temperature
F3	Surface No. 3	Heat transfer coefficient and ambient temperature
F4	Surface No. 4	Heat transfer coefficient and ambient temperature
F5	Surface No. 5	Heat transfer coefficient and ambient temperature
F6	Surface No. 6	Heat transfer coefficient and ambient temperature
F0	Shell Surface	Heat transfer coefficient and ambient temperature

(7) `!SFILM` (4-7)

Definition of heat transfer coefficient by surface group

Parameter

AMP1 = Heat transfer coefficient history table name (specified in !AMPLITUDE)
AMP2 = Ambient temperature history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) SURFACE_GRP_NAME, Value, Sink

Parameter Name	Attributions	Contents
SURFACE_GRP_NAME	C	Surface group name
Valu	R	Heat Transfer Rate
Sink	R	Ambient Temperature

Example of Use

!SFILM
  SFSURF, 1.0, 800.0
!SFILM, AMP1=TSFILM, AMP2=TFILM
  SFSURF, 1.0, 1.0

`!RADIATE` (4-8)

Definition of radiation factor given to boundary plane

Parameter

AMP1 = Radiation factor history table name (specified in !AMPLITUDE)
AMP2 = Ambient temperature history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) ELEMENT_GRP_NAME, LOAD_type, Value, Sink

Parameter Name	Attributions	Contents
ELEMENT_GRP_NAME	C/I	Element group name or element ID
LOAD_type	C	Load type No.
Value	R	Radiation factor
Sink	R	Ambient temperature

Example of Use

!RADIATE
  RSURF, R1, 1.0E-9, 800.0
!RADIATE, AMP2=TRAD
  RSURF, R1, 1.0E-9, 1.0

# Load Parameters

Load Type No.	Applied Surface	Parameter
R1	Surface No. 1	Radiation factor and ambient temperature
R2	Surface No. 2	Radiation factor and ambient temperature
R3	Surface No. 3	Radiation factor and ambient temperature
R4	Surface No. 4	Radiation factor and ambient temperature
R5	Surface No. 5	Radiation factor and ambient temperature
R6	Surface No. 6	Radiation factor and ambient temperature
R0	Shell Surface	Radiation factor and ambient temperature

(9) `!SRADIATE` (4-9)

Definition of radiation factor by surface group

Parameter

AMP1 = Radiation factor history table name (specified in !AMPLITUDE)
AMP2 = Ambient temperature history table name (specified in !AMPLITUDE)

2nd line or later

(2nd line) SURFACE_GRP_NAME, Value, Sink

Parameter Name	Attributions	Contents
SURFACE_GRP_NAME	C	Surface group name
Value	R	Radiation factor
Sink	R	Ambient temperature

Example of Use

!SRADIATE
  RSURF, 1.0E-9, 800.0
!SRADIATE, AMP2=TSRAD
  RSURF, 1.0E-9, 1.0

(10) `!WELD_LINE` (4-10)

Definition of weld line (Linear)

Parameter

N/A

2nd line

(2nd line) I, U, Coef, V

Parameter Name	Attributions	Contents
I	R	Current
U	R	Voltage
Coef	R	Heat input coefficient
V	R	Movement speed of the welding torch

3rd line

(3rd line) EGROUP, XYZ, C1, C2, H, tstart

Parameter Name	Attributions	Contents
EGROUP	C	Element group name for heat input
XYZ	I	Movement direction of welding torch (Degree of freedom No.)
C1	R	Starting point coordinates of welding torch
C2	R	Ending point coordinates of welding torch
H	R	Width of welding torch, inside which thermo energy inputted
tstart	R	Welding start time

Control Data for Dynamic Analysis

(1) `DYNAMIC`

Dynamic analysis control

Time t for each !AMPLITUDE specified in !BOUNDARY, !CLOAD and !DLOAD must be started from 0.0.

Parameter

TYPE = LINEAR    : Linear dynamic analysis
       NONLINEAR : Nonlinear dynamic analysis

2nd line or later

(2nd line) idx_eqa, idx_resp

Parameter Name	Attributions	Contents
idx_eqa	I	Solution of equation of motion (Direct time integration) (Default: 1) 1: Implicit method (Newmark-β method) 11: Explicit method (Center difference method)
idx_resp	I	Analysis type (Default: 1) 1: Time history response analysis 2: Frequency response analysis (Not included)

# `idx_resp=1` (Time history response analysis)

(3rd line) t_start , t_end , n_step, t_delta

Parameter Name	Attributions	Contents
t_start	R	Analysis start time (Default: 0.0), not used
t_end	R	Analysis end time (Default: 1.0), not used
n_step	I	Overall No. of steps (Default: 1)
t_delta	R	Time increment (Default: 1.0)

(4th line) ganma , beta

Parameter Name	Attributions	Contents
ganma	R	Parameter γ of Newmark-β method (Default: 0.5)
beta	R	Parameter β of Newmark-γ method (Default: 0.25)

(5th line) idx_mas ,idx_dmp , ray_m ,ray_k

Parameter Name	Attributions	Contents
idx_mas	I	Type of mass matrix (Default: 1) 1: Lumped mass matrix 2: Consistent mass matrix
idx_dmp	I	1: Rayleigh damping (Default: 1)
ray_m	R	Parameter R_m of Rayleigh damping (Default: 0.0)
ray_k	R	Parameter R_k of Rayleigh damping (Default: 0.0)

(6th line) nout, node_monit_1, nout_monit

Parameter Name	Attributions	Contents
nout	I	not used
node_monit_1	I	Monitoring node ID (Global) or node group name
nout_monit	I	Results output interval of displacement monitoring (Default: 1)

Note: Regarding the information of the monitoring node specified in this line, the displacement is output to the file <dyna_disp_NID.txt>, where NID is the global ID of the monitoring node, and each line includes the step number, time of the step, NID, u1, u2, and u3 in this order. The velocity and acceleration are also output to <dyna_velo_NID.txt> and <dyna_acce_NID.txt>, respectively, in the same format as the displacement. The nodal strain is output to <dyna_strain_NID.txt> and each line includes the step number, time of the step, NID, e11, e22, e33, e12, e23, and e13 in this order. The nodal stress is output to <dyna_stress_NID.txt> and each line includes the step number, time of the step, NID, s11, s22, s33, s12, s23, s13, and s_mises in this order. When monitoring nodes are specified by a node group, each of the files stated above is separately output for each node. When this output is specified, the kinetic energy, deformation energy and the overall energy of the overall analytic model will also be output to <dyna_energy.txt>.

(7th line) iout_list(1),iout_list(2),iout_list(3),iout_list(4),iout_list(5),iout_list(6)

Parameter Name	Attributions	Contents
iout_list(1)	I	Displacement output specification (Default: 0) 0: Not output, 1: Output
iout_list(2)	I	Velocity output specification (Default: 0) 0: Not output, 1: Output
iout_list(3)	I	Acceleration output specification (Default: 0) 0: Not output, 1: Output
iout_list(4)	I	Reaction force output specification (Default: 0) 0: Not output, 1: Output
iout_list(5)	I	Strain output specification (Default: 0) 1: Output 2: Output (Node base) 3: Output (Element base)
iout_list(6)	I	Stress output specification (Default: 0) 0: Not output (Element base and node base) 1: Output 2: Output (Node base) 3: Output (Element base)

Example of Use

!DYNAMIC, TYPE=NONLINEAR
  1 , 1
  0.0, 1.0, 500, 1.0000e-5
  0.5, 0.25
  1, 1, 0.0, 0.0
  100, 55, 1
  0, 0, 0, 0, 0, 0

# `idx_resp=2` (Frequency response analysis)

(3rd line) f_start, f_end, n_freq, f_disp

Parameter Name	Attributions	Contents
f_start	R	Minimum frequency
f_end	R	Maximum frequency
n_freq	I	Number of divisions for the frequency range
f_disp	R	Frequency to obtain displacement

(4th line) t_start, t_end

Parameter Name	Attributions	Contents
t_start	R	Analysis start time
t_end	R	Analysis end time

(5th line) idx_mas, idx_dmp, ray_m ,ray_k

Parameter Name	Attributions	Contents
idx_mas	I	Type of mass matrix (Default: 1) 1: Lumped mass matrix
idx_dmp	I	1: Rayleigh damping (Default: 1)
ray_m	R	Parameter R_m of Rayleigh damping (Default: 0.0)
ray_k	R	Parameter R_k of Rayleigh damping (Default: 0.0)

(6th line) nout, vistype, nodeout

Parameter Name	Attributions	Contents
nout	I	Results output interval in time domain
vistype	I	Visuzalization type 1:Mode shapes 2:Time history results at f_disp
nodeout	I	Monitoring NODE ID in frequency domain

(7th line) iout_list(1),iout_list(2),iout_list(3),iout_list(4),iout_list(5),iout_list(6)

Parameter Name	Attributions	Contents
iout_list(1)	I	Displacement output specification (Default: 0) 0: Not output, 1: Output
iout_list(2)	I	Velocity output specification (Default: 0) 0: Not output, 1: Output
iout_list(3)	I	Acceleration output specification (Default: 0) 0: Not output, 1: Output
iout_list(4)	I	not used
iout_list(5)	I	not used
iout_list(6)	I	not used

Example of Use

!DYNAMIC
  11 , 2
  14000, 16000, 20, 15000.0
  0.0, 6.6e-5
  1, 1, 0.0, 7.2E-7
  10, 2, 1
  1, 1, 1, 1, 1, 1

(2) `!VELOCITY` (5-2)

Definition of velocity boundary conditions

Parameter

TYPE = INITIAL (Initial velocity boundary conditions)
     = TRANSIT (Time history velocity boundary conditions
                specified in !AMPLITUDE;Default)
AMP  = Time function name (specified in !AMPLITUDE)
       Provides the relationship betweentime t and factor f(t) in !AMPLITUDE.
       The time multiplied by factor f(t) to the following value
       becomes the restrained value of that time
       (when not specified: time and factor relationship becomes f(t) = 1.0).

2nd line or later

(2nd line) NODE_ID, DOF_idS, DOF_idE, Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
DOF_idS	I	Start No. of restricted degree of freedom
DOF_idE	I	End No. of restricted degree of freedom
Value	R	Restricted value (Default: 0)

Example of Use

!VELOCITY, TYPE=TRANSIT, AMP=AMP1
  1, 1, 1, 0.0
  ALL, 3, 3
  * Restricted value is 0.0
!VELOCITY, TYPE=INITIAL
  1, 3, 3, 1.0
  2, 3, 3, 1.0
  3, 3, 3, 1.0

Note: The velocity boundary conditions are different than the displacement boundary conditions, and the multiple degrees of freedom can not be defined collectively. Therefore, the same number must be used for DOF_idS and DOF_idE. When the TYPE is INITIAL, AMP becomes invalid.

(3) `!ACCELERATION` (5-3)

Definition of acceleration boundary conditions

Parameter

TYPE = INITIAL (Initial acceleration boundary conditions)
     = TRANSIT ((Time history acceleration boundary conditions
                 specified in AMPLITUDE; Default)
AMP  = Time function name (specified in !AMPLITUDE)
       Provides the relationship between time t and factor f(t) in !AMPLITUDE.
       The time multiplied by factor f(t) to the following Value
       becomes the restrained value of that time (when not specified:
       time and factor relationship becomes f(t) = 1.0).

2nd line or later

(2nd line) NODE_ID, DOF_idS, DOF_idE, Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID or node group name
DOF_idS	I	Start No. of restricted degree of freedom
DOF_idE	I	End No. of restricted degree of freedom
Value	R	Restricted value (Default: 0)

Example of Use

!ACCELERATION, TYPE=TRANSIT, AMP=AMP1
  1, 1, 3, 0.0
  ALL, 3, 3
  i* Restricted value is 0.0
!ACCELERATION, TYPE=INITIAL
  1, 3, 3, 1.0
  2, 3, 3, 1.0
  3, 3, 3, 1.0

Note: The acceleration boundary conditions are different than the displacement boundary conditions, and the multiple degrees of freedom can not be defined collectively. Therefore, the same number must be used for DOF_idS and DOF_idE.

When the TYPE is INITIAL, AMP becomes invalid.

(4) `!COUPLE` (5-4)

Definition of coupled surface (Used only in coupled analysis)

Parameter

TYPE =  1: One-way coupled (FrontISTR starts from receiving data)
        2: One-way coupled (FrontISTR starts from sending data)
        3: Staggered two-way coupled (FrontISTR starts from receiving data)
        4: Staggered Two-way coupled (FrontISTR starts from sending data)
        5: Iterative partitioned two-way coupled (FrontISTR starts from receiving data)
        6: Iterative partitioned two-way coupled (FrontISTR starts from sending data)
ISTEP = Step No.
        From the beginning of analysis to the step specified here, a linearly increasing
        function from 0 to 1 is multiplied to the input fluid traction.
        After this step, the input fluid traction is directly applied.
WINDOW => 0: Multiply window function(*) to input fluid traction

(*) $\frac{1}{2}(1 - \cos\frac{2\pi i}{N})$ , $i$ : current step, $N$ : no. of steps of current analysis

2nd line or later

(2nd line) COUPLING_SURFACE_ID

Parameter Name	Attributions	Contents
SURFACE_ID	C	Surface group name

Example of Use

!COUPLE , TYPE=1
  SCOUPLE1
  SCOUPLE2

(5) `!EIGENREAD` (5-5)

Controlling the input file for frequency response analysis

Parameter

N/A

2nd line or later

Parameter Name	Attributions	Contents
eigenlog_filename	C	The name of eigenvalue analysis log

(3rd line) start_mode, end_mode

Parameter Name	Attributions	Contents
start_mode	I	lowest mode to be used in frequency response analysis
end_mode	I	highest mode to be used in frequency response analysis

Example of Use

!EIGENREAD
  eigen_0.log
  1, 5

(6) `!FLOAD` (5-6)

Defining external forces applied in frequency response analysis

Parameter

LOAD CASE = (1: Real part, 2: Imaginary part)

2nd line or later

(2nd line) NODE_ID, DOF_id, Value

Parameter Name	Attributions	Contents
NODE_ID	I/C	Node ID, node group name or surface group name
DOF_id	I	Degree of freedom No.
Value	R	Load value

Example of Use

!FLOAD, LOAD CASE=2
  _PickedSet5, 2, 1.0

Solver Control Data

(1) `!SOLVER` (6-1)

Control of solver

Mandatory control data

Parameter

METHOD =    Method (CG, BiCGSTAB, GMRES, GPBiCG, DIRECT, DIRECTmkl, MUMPS)
            DIRECT: Direct method other than contact analysis (serial processing only) (currently unavailable)
            DIRECTmkl: Direct method by Intel MKL
            MUMPS    : Direct method by MUMPS
            When any of direct methods is selected, the data lines will be disregarded.
            Thread-parallel computation by OpenMP is available in iterative methods
            for 3D problems.

PRECOND =   Preconditioner for iterative methods (1, 2, 3, 5, 10, 11, 12)
            1, 2       : (Block) SSOR (with multi-color ordering only for 3D problems)
            3          : (Block) Diagonal Scaling
            5          : AMG by multigrid preconditioner package ML
            10         : Block ILU(0)
            11         : Block ILU(1)
            12         : Block ILU(2)
            10, 11 and 12 are available only in 3D problems.
            In thread-parallel computation, SSOR, Diagonal Scaling or ML is recommended.

ITERLOG =   Whether solver convergence history is output (YES/NO) (Default: NO)

TIMELOG =   Whether solver computation time is output (YES/NO/VERBOSE) (Default: NO)

USEJAD =    Whether matrix ordering optimized for vector processors are performed
            (YES/NO) (Default: NO)
            Valid only in 3D problems with iterative solvers.

SCALING =   Whether matrix is scaled so that each diagonal element becomes 1 (YES/NO)
            (Default: NO)
            Valid only in 3D problems with iterative solvers.

DUMPTYPE =  Type of matrix dumping (NONE, MM, CSR, BSR) (Mainly for debugging)
            NONE : no dumping (Default)
            MM   : matrix is dumped in Matrix Market format
            CSR  : matrix is dumped in Compressed Sparse Row (CSR) format
            BSR  : matrix is dumped in Blocked CSR format

DUMPEXIT =  Whether the program terminates right after matrix dumping (YES/NO)
            (Default: NO)

MPCMETHOD = Method for multipoint constraints
            1: Penalty method (Default for direct methods)
            2: MPC-CG method (Deprecated)
            3: Explicit master-slave elimination (Default for iterative methods)

ESTCOND =   Frequency of condition number estimation (experimental)
            Estimation is performed at every specified number of iterations and at the last
            iteration.  No estimation when 0 is specified.

METHOD2 =   Secondary method (BiCGSTAB, GMRES, GPBiCG) (experimental)
            Valid only when CG is specified as METHOD.
            When specified, the method is swithced and solution continues when CG diverged.
            All the other parameters and data lines are shared with the CG method.

CONTACT_ELIM = Whether DOF elimination is performed in contact analysis (0, 1)
               0: Perform DOF elimination only when using iterative methods (Default)
               1: Always perform DOF elimination (even when using direct methods)

2nd line or later

(2nd line) NITER, iterPREmax, NREST, NCOLOR_IN, RECYCLEPRE

Parameter Name	Attributions	Contents
NITER	I	No. of iterations (Default: 100)
iterPREmax	I	No. of iteration of preconditioning based on Additive Schwarz (Default: 1) (recommended value : 1 (2 might be efficient in some parallel computation))
NREST	I	No. of Krylov subspaces (Default: 10) (Valid only when GMRES is selected as the solution)
NCOLOR_IN	I	No. of Colors for Multi-Color ordering (Default: 10) (Valid only when no. of OpenMP threads >= 2)
RECYCLEPRE	I	No. of recycling set-up info for preconditioning (Default: 3) (Valid only in nonlinear analyses)

(3rd line) RESID, SIGMA_DIAG, SIGMA

Parameter Name	Attributions	Contents
RESID	R	Truncation error (Default: 1.0e-8)
SIGMA_DIAG	R	Scale factor for diagonal elements when computing preconditioning matrix (Default: 1.0) (When divide-by-zero or divergence occurs with ILU preconditioning, convergence might be obtained by setting number greater than 1.0)
SIGMA	R	Not used (Default: 0.0)

# In case of `PRECOND=5` (Optional)

When any other value is specified for PRECOND, the 4th line will be disregarded.

(4th line) ML_CoarseSolver, ML_Smoother, ML_MGCycle, ML_MaxLevels, ML_CoarseningScheme, ML_NumSweep

Parameter Name	Attributions	Contents
ML_CoarseSolver	I	Coarse solver of ML (1: smoother, 2: KLU (serial direct solver), 3: MUMPS (parallel direct solver)) (Default: 1) (recommended value : 3 or 2 for stiff problems, 1 for other problems)
ML_Smoother	I	Smoother of ML (1: Chebyshev, 2: SymBlockGaussSeidel, 3: Jacobi) (Default: 1) (recommended value : 1)
ML_MGCycle	I	Multigrid cycle of ML (1: V-cycle, 2: W-cycle, 3: Full-V-cycle) (Default: 1) (recommended value : 2 for stiff problems, 1 for other problems)
ML_MaxLevels	I	Max No. of levels of ML (Default: 10) (recommended value : 2 (or 3 when memory is not sufficient) with direct coarse solver for very stiff problems, 10 for other problems)
ML_CoarseningScheme	I	Coarsening scheme of ML (1: UncoupledMIS, 2: METIS, 4: Zoltan, 5: DD) (Default: 1) (recommended value : 1 or 5)
ML_NumSweep	I	No. of smoother sweeps of ML (polinomial degree for Chebyshev) (Default: 2) (recommended value : 2 for Chebyshev, 1 for SymBlockGaussSeidel)

Example of Use

Use CG with SSOR preconditioning, and set No. of iteration to 10000 and truncation error to 1.0e-8

!SOLVER, METHOD=CG, PRECOND=1, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.0, 0.0

Use GMRES with SSOR preconditioning, and set No. of Krylov subspace to 40 and No. of colors for Multi-Color ordering to 100

!SOLVER, METHOD=GMRES, PRECOND=1, ITERLOG=YES, TIMELOG=YES
  10000, 1, 40, 100
  1.0e-8, 1.0, 0.0

Use CG with ILU(0) preconditioning, and set scale factor for diagonal elements when computing preconditioning matrix to 1.1

!SOLVER, METHOD=CG, PRECOND=10, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.1, 0.0

Use CG with AMG preconditioning by ML

!SOLVER, METHOD=CG, PRECOND=5, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.0, 0.0

Use CG with AMG preconditioning by ML, and set coarse solver to MUMPS (for stiff problems)

!SOLVER, METHOD=CG, PRECOND=5, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.0, 0.0
  3

Use CG with AMG preconditioning by ML, and set multigrid cycle to W-cycle (for stiff problems)

!SOLVER, METHOD=CG, PRECOND=5, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.0, 0.0
  1, 1, 2

Use CG with AMG preconditioning by ML, and set coarse solver to MUMPS and max No. of levels to 2 (for very stiff problems)

!SOLVER, METHOD=CG, PRECOND=5, ITERLOG=YES, TIMELOG=YES
  10000, 1
  1.0e-8, 1.0, 0.0
  3, 1, 1, 2

Post Process (Visualization) Control Data

(1) `!VISUAL` (P1-0)

Specifies the visualization method.

METHOD = PSR             : Surface rendering
  visual_start_step      : Specification of time step number which starts the visualization process
                           (Default: 1)
  visual_end_step        : Specification of time step number which ends the visualization process
                           (Default: All)
  visual_interval_step   : Specification of time step interval which performs the visualization process
                           (Default: 1)

(2) `!surface_num`, `!surface`, `!surface_style` (P1-1 - 3)

`!surface_num` (P1-1)

No. of surfaces in one surface rendering

Ex.: There are four surfaces in Figure 7.4.1, which includes two isosurfaces pressure = 1000.0 and pressure = -1000.0, and two cut end plane surfaces z = -1.0 and z = 1.0.

Example of surface_num Setting

Figure 7.4.1: Example of surface_num Setting

`!surface` (P1-2)

Sets the contents of the surface.

Ex: Then contents of the four surface in Figure 7.4.2 are as follows.

Example of Surface Setting

Figure 7.4.2: Example of Surface Setting

!surface_num = 2
!SURFACE
!surface_style = 2
!data_comp_name = press
!iso_value = 1000.0
!display_method = 4
!specified_color = 0.45
!output_type = BMP
!SURFACE
!surface_style = 2
!data_comp_name = press
!iso_value = -1000.0
!display_method = 4
!specified_color = 0.67

`!surface_style` (P1-3)

Specifies the style of the surface.

Boundary plane
Isosurface
Arbitary quadric surface
coef[1]x2 + coef[2]y2 + coef[3]z2 + coef[4]xy + coef[5]xz
+ coef[6]yz + coef[7]x + coef[8]y + coef[9]z + coef[10]=0

Example of surface_style Setting

Figure 7.4.3: Example of surface_style Setting

(3) `!display_method` (P1-4)

Display method (Default: 1)

Color code display
Boundary line display
Color code and boundary line display
Display of 1 specified color
Isopleth line display by classification of color

Example of display_method Setting

Figure 7.4.4:Example of display_method Setting

(2) `!color_comp_name`, `!color_comp`, `!color_subcomp` (P1-5, P1-7, P1-8)

Specifies the selections for the color map from the physical values. Provides the names to the necessary physical values and the degree of freedom numbers. Accordingly, the names will be entered for the structure node_label(:) and nn_dof(:) of the results data.

Then you can define which one you hope to map into color by

`!color_comp_name` (Character string, default: 1st parameter)

Example

!color_comp_name = pressure
  In static analysis;        = DISPLASEMENT : Specification 
                                              of the results displacement data
                             = STRAIN       : Specification of strain data
                             = STRESS       : Specification of stress data
  In heat transfer analysis; = TEMPERATURE  : Specification
                                              of the results temperature data

`!color_comp` (Integer, default: 0)

Physical value ID number (Integers above 0)

Example

!color_comp = 2

This is the specification of the ID number and component name of the results data type; however, this is not included.

`!color_subcomp` (Integer, default: 0)

When the physical value is 1 degree of freedom or more like the vector quantity, it’s the number of the degree of freedom.

Example:

!color_subcomp = 0

    When !color_comp_name=DISPLACEMENT is specified
        1: X Component,  2: Y Component, 3: Z Component

    When !color_comp_name=STRAIN is specified
        1: $\epsilon$x,  2: $\epsilon$y,  3: $\epsilon$z
        4: $\epsilon$xy, 5: $\epsilon$yz, 6: $\epsilon$zx

    When !color_comp_name=STRESS is specified
        1: $\sigma$x,  2: $\sigma$y,  u: $\sigma$z
        4: $\tau$xy, 5: $\tau$yz, 6: $\tau$zx

    When !color/comp\_name=TEMPERATURE is specified
        1: Temperature

In the structural analysis, for example;

Physical Value	Displacement	Strain	Stress
No. of degrees of freedom	3	6	7

Example of color_comp, color_subcomp and color_comp_name Setting

Figure 7.4.5: Example of color_comp, color_subcomp and color_comp_name Setting

(5) `!isoline_number`, `!isoline_color` (P1-9, P2-22)

When display_method=2,3 or 5

Example of isoline_number and isoline_color Setting

Figure 7.4.6: Example of isoline_number and isoline_color Setting

(6) `!initial_style`, `!deform_style` (P1-15, P1-16)

Specifies the display style of the initial shape and the deformed shape.

Not specified
Solid line mesh (Displayed in blue if not specified)
Gray filled pattern
Shading (Let the physical attributions respond to the color)
Dotted line mesh (Displayed in blue if not specified)

(7) `!deform_scale` (P1-14)

Specifies the displacement scale when displaying deformation.

Default: Auto

standard_scale = 0.1 * sqrt(x_range² + y_range² + z_range²) / max_deform

Example of Display Styles Setting

Figure 7.4.7: Example of display_styles Setting

Example of deform_scale Setting

Figure 7.4.8: Example of deform_scale Setting

(8) `!output_type` (P1-19)

Specifies the type of output file. (Default: AVS)

AVS                   : UCD data for AVS (only on object surface)
BMP                   : Image data (BMP format)
VTK                   : VTK data for ParaView
COMPLETE_AVS          : UCD data for AVS
COMPLETE_REORDER_AVS  : Rearranges the node and element ID in the UCD data for AVS
SEPARATE_COMPLETE_AVS : UCD data for AVS for each decomposed domain
COMPLETE_MICROAVS     : Outputs the physical values in the scalar in the UCD data for AVS
BIN_COMPLETE_AVS      : Outputs COMPLETE_AVS in binary format
FSTR_FEMAP_NEUTRAL    : Neutral file for FEMAP

Example of output_type

Figure 7.4.9: Example of output_type

(9) `!x_resolution`, `!y_resolution` (P2-1, P2-2)

Specifies the resolution when output_type=BMP

Example of x_resolution and y_resolution Setting

Figure 7.4.10: Example of x_resolution and y_resolution Setting

(10) `!viewpoint`, `!look_at_point`, `!up_direction` (P2-5, P2-6, P2-7)

viewpoint

Specifies the viewpoint position by coordinates.

Default: x = (xmin + xmax)/2.0, y = ymin + 1.5 (ymax – ymin), z = zmin + 1.5 (zmax – zmin)

look_at_point

Specifies the look at point position.

Default: Center of data

up_direction

Specifies the view frame in viewpoint, look_at_point and up_direction.

default: 0.0 0.0 1.0

View coodinate frame

Origin: look_at_point
Z-axis: viewpoint - look_at_point
X-axis: up_direction × z axis

View Frame Determination Method

Figure 7.4.11: View Frame Determination Method

Example of !viewpoint, look_at_point and up_direction Setting

Figure 7.4.12: Example of !viewpoint, look_at_point and up_direction Setting

(11) `!ambient_coef` `!diffuse_coef` `!specular_coef` (P2-8 P2-9 P2-10)

Coefficient setting of lighting model

When the ambient_coef is increased, information on the 3D depth direction is impaired.

Example of Lighting Model Parameter Setting

(12) '!color_mapping_bar_on' '!scale_marking_on' '!num_of_scales' (P2-16 P2-17 P2-18)


`!color_mapping_bar_on`	Specifies whether to display the color mapping bar. 0: off 1: on (Default: 0)
`!scale_marking_on`	set the memory status of `color_mapping_bar` 0: off 1: on (default: 0)
`!num_of_scales`	Specifies the number of memory. (default: 3)

Example of Color Mapping Bar Display

(13) `!font_size` `!font_color` `!backgroud_color` (P2-19 P2-20 P2-21)

Specifies the background color and character font.

Example of Background and Font Setting

Figure 7.4.15: Example of Background and Font Setting

(14) `!data_comp_name`, `!data_comp`, `!data_subcomp` (P3-1, P3-3, P3-4)

Specifies the physical values of the isosurface to be visualized when surface_style=2.

Example of data_comp, data_subcomp and data_comp_name Setting

Figure 7.4.16: Example of data_comp, data_subcomp and data_comp_name Setting

(15) `!method` (P4-1)

When specifying the surfaces and cut end, specifies the setting method of the surface.

!surface_num =2
!surface
!surface_style=3
!method=5
!coef=0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 1.0, -0.35
!color_comp_name = temperature

Figure 7.4.17: Example of Setting Method

Accordingly, the cut end of the plane surface z = 0.35 and z = -0.35 will be visualized.

Analysis Control Data

Analysis Control Data

Outline of Analysis Control Data

Input Rules

Analysis Control Data

Header List of Computing Control Data

(1) Control data common to all analyses

Example of Analysis Control Data

Description of Header

1-1 !VERSION

1-2 !SOLUTION, TYPE=STATIC

1-3 !WRITE, VISUAL

1-4 !WRITE, RESULT

1-6 !ECHO

1-8 !END

(2) Static analysis control data

Example of Static Analysis Control data

Description of Header

2-1 !STATIC

2-2 !MATERIAL

2-2-1 !ELASTIC, TYPE=ISOTROPIC

2-3 !BOUNDARY

2-3-1 !SPRING

2-4 !CLOAD

2-5 !DLOAD

2-9 !TEMPERATURE

2-10 !REFTEMP

2-11 !STEP

(3) Eigenvalue analysis control data

Example of Eigenvalue Analysis Control Data

Description of Header

3-1 !EIGEN

2-3 !BOUNDARY (Same items an in Static Analysis)

(4) Heat conduction analysis control data

Example of Heat Conduction Analysis Control Data

Description of Header

4-1 !HEAT

4-2 !FIXTEMP

4-3 !CFLUX

4-4 !DFLUX

4-5 !SFLUX

4-6 !FILM

4-7 !SFILM

4-8 !RADIATE

4-9 !SRADIATE

(5) Dynamic analysis control data

Example of Dynamic Analysis Control Data

Description Header

5-1 !DYNAMIC

2-3 !BOUNDARY (Same items as in Static Analysis)

2-4 !CLOAD (Same items as in Static Analysis)

5-4 !COUPLE, TYPE=1

2-11 !STEP, CONVERG=1.E-10, ITMAX=20

(6) Dynamic analysis (Frequency Response Analysis) Control Data

Example of Dynamic analysis (Frequency Response Analysis)

Description of Header

5-1 !DYNAMIC

5-5 !EIGENREAD

5-6 !FLOAD

Solver Control Data

Example of Solver Control Data

Description of Header

6-1 !SOLVER

6-2

6-3

Post Process (Visualization) Control Data

Example of Visualization Control Data

Common Data List<P1-1 - P1-19>

Rendering Data List <P2-1 - P2-26>

Data List by Setting Values of surface_style

In the case of isosurface (surface_style=2)

In the case of a curved surface (surface_sytle = 3) specified by the equation of the user

Details of Analysis Control Data Parameters

Common Control Data

(1) !VERSION (1-1)

Example of Use

(2) !SOLUTION (1-2)

Parameter

Example of Use

(3) !WRITE, VISUAL (1-3)

1-1 `!VERSION`

1-2 `!SOLUTION, TYPE=STATIC`

1-3 `!WRITE, VISUAL`

1-4 `!WRITE, RESULT`

1-6 `!ECHO`

1-8 `!END`

2-1 `!STATIC`

2-2 `!MATERIAL`

2-2-1 `!ELASTIC, TYPE=ISOTROPIC`

2-3 `!BOUNDARY`

2-3-1 `!SPRING`

2-4 `!CLOAD`

2-5 `!DLOAD`

2-9 `!TEMPERATURE`

2-10 `!REFTEMP`

2-11 `!STEP`

3-1 `!EIGEN`

2-3 `!BOUNDARY` (Same items an in Static Analysis)

4-1 `!HEAT`

4-2 `!FIXTEMP`

4-3 `!CFLUX`

4-4 `!DFLUX`

4-5 `!SFLUX`

4-6 `!FILM`

4-7 `!SFILM`

4-8 `!RADIATE`

4-9 `!SRADIATE`

5-1 `!DYNAMIC`

2-3 `!BOUNDARY` (Same items as in Static Analysis)

2-4 `!CLOAD` (Same items as in Static Analysis)

5-4 `!COUPLE, TYPE=1`

2-11 `!STEP, CONVERG=1.E-10, ITMAX=20`

5-1 `!DYNAMIC`

5-5 `!EIGENREAD`

5-6 `!FLOAD`

6-1 `!SOLVER`

Data List by Setting Values of `surface_style`

In the case of isosurface (`surface_style=2`)

(1) `!VERSION` (1-1)

(2) `!SOLUTION` (1-2)

(3) `!WRITE, VISUAL` (1-3)

(4) `!WRITE, RESULT` (1-4)

(5) `!WRITE, LOG` (1-5)

(6) `!OUTPUT_VIS` (1-6)

(7) `!OUTPUT_RES` (1-7)

(8) `!RESTART` (1-8)

(9) `!ECHO` (1-9)

(10) `!ORIENTATION` (1-10)

(11) `!SECTION` (1-11)

(12) `!INITIAL_CONDITION` (1-12)

# In case of `TYPE = TEMPERATURE`

# In case of `TYPE= VELOCITY/ACCELERATION`

(13) `!END` (1-13)

(1) `!STATIC` (2-1)

(2) `!MATERIAL` (2-2)

(3) `!ELASTIC` (2-2-1)

(4) `!PLASTIC` (2-2-2)

# In case of `YIELD = MISES` (Default)

# In case of `YIELD =` Mohr-Coulomb or Drucker-Prager

(5) `!HYPERELASTIC` (2-2-3)

# In the case of `TYPE = NEOHOOKE`

# In case of `TYPE = MOONEY-RIVLIN`

# In case of `TYPE = ARRUDA-BOYCE`

# `TYPE = MOONEY-RIVLIN-ANISO`の場合

# In case of `TYPE = USER`

(6) `!VISCOELASTIC` (2-2-4)

(7) `!CREEP` (2-2-5)

(8) `!DENSITY` (2-2-6)

(9) `!EXPANSION_COEFF` (2-2-7)

# In case of `TYPE=ISOTROPIC`

# In case of `TYPE=ORTHOTROPIC`

(10) `!TRS` (2-2-8)

(11) `!FLUID` (2-2-9)

(12) `!USER_MATERIAL` (2-2-10)