김경종
25 KiB
Requesting detailed adaptive mesh smoothing printout
You can activate detailed printout of adaptive mesh smoothing in Abaqus/Standard. The output includes information about the magnitude of the maximum displacement and the node and degree of freedom where the maximum displacement increment occurs during each mesh sweep. It also provides the node numbers at which geometric feature changes occur. By default, only a summary is output.
Input File Usage: *PRINT, ADAPTIVE MESH=YES or NO
Abaqus/CAE Usage: Adaptive mesh output to the message file is not supported in Abaqus/CAE.
Monitoring a degree of freedom in the message file
You can write the current value of a specified point and degree of freedom to the message file. This information can be used to monitor the progress of the solution. The information will also be written in the status file (see below). You can control the frequency at which the value is printed in the message file. The default frequency is 1 (or 10 in a direct cyclic analysis).
Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value.
Input File Usage: *MONITOR, NODE=node_number, DOF=dof, FREQUENCY=N
The node and degree of freedom being monitored can be changed from step to step by repeating the *MONITOR option. The node and degree of freedom specified in the last occurrence of this option in a step will be used for that step.
Abaqus/CAE Usage: Step module: Output→DOF Monitor: Monitor a degree of freedom throughout the analysis, click Edit to select the point, Degree of freedom: dof, Print to the message file every N increments
In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step.
The Abaqus/Explicit message file
In Abaqus/Explicit the message file contains messages if potential problems are detected during an analysis. You can control the output of diagnostic messages for each step (see “Explicit dynamic analysis,” Section 6.3.3, and “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1). A portion of the diagnostic information in the message file is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3).
The status file
The status file (job-name.sta) is a text file that contains information about the progress of an analysis.
The Abaqus/Standard or Abaqus/CFD status file
The Abaqus/Standard or Abaqus/CFD status file contains a single 80-character record for each increment and is updated upon completion of each increment of an analysis. This record is written directly to secondary storage immediately at the completion of the increment. Therefore, the status file can be examined as the analysis job is executing, thus providing a monitor of the progress of the analysis. Other than specifying that a degree-of-freedom variable be monitored in the status file in Abaqus/Standard (as described below), the information written to the Abaqus/Standard or Abaqus/CFD status file cannot be controlled.
The Abaqus/Explicit status file
In Abaqus/Explicit the status file (job-name.sta) contains, by default, mass and inertial properties for the model, initial stable time increment information, a synopsis of the progress of the analysis including total accumulated CPU usage and the current time increment size, and an estimate of the memory required to process each step. You can control additional output including the total kinetic energy, the energy balance, the identifiers of the elements with the smallest stable time increments, and the percent change in total mass of the model due to mass scaling.
The frequency at which summary increments are written to the Abaqus/Explicit status file depends on the duration of the analysis in CPU minutes and the amount of output specified in the analysis. The following list provides general guidelines for when a summary increment will be written to the status file.
Summary information will generally be written:
• Each time restart information, field output to the output database, or results file output is written.
• Once per increment if the problem requires fewer than 20 increments.
• 20 times during the step for a short analysis (less than 40 CPU minutes).
• Every 2 CPU minutes for an analysis longer than 40 CPU minutes.
A degree-of-freedom variable can be monitored in the status file while the analysis is running. You can also write additional diagnostic information to the status file (see “Explicit dynamic analysis,” Section 6.3.3, and “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1, for details). A portion of the diagnostic information in the status file, including information for each summary increment, is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3).
Errors that can be detected only while packaging the data for Abaqus/Explicit or during analysis are also written to the status file.
Input File Usage: *PRINT
The *PRINT option can appear only once within a step definition.
Abaqus/CAE Usage: Step module: Output→Diagnostic Print
Requesting kinetic energy output
By default, the kinetic energy for the model is written to the status file. This output is written periodically throughout the step. You can choose to include or exclude the kinetic energy output for each step.
Input File Usage: *PRINT, ALLKE=YES or NO
Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Allke
Requesting total energy output
By default, the energy balance is written periodically throughout the step. You can choose to include or exclude the energy balance output for each step.
Input File Usage: *PRINT, ETOTAL=YES or NO
Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Etotal
Requesting output of the critical element
By default, the number of the element with the current minimum stable time increment and its value are output to the status file. This output is written periodically throughout the step. You can choose to include or exclude the critical element output for each step.
Input File Usage: *PRINT, CRITICAL ELEMENT=YES or NO
Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Crit. Elem.
Requesting output of the change in the total mass
You can write the percent change in total mass of the model due to mass scaling to the status file for each step. This output is written periodically throughout the step. The percent change in total mass is printed by default only if mass scaling is present in the model.
Input File Usage: *PRINT, DMASS=YES or NO
Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Dmass
Monitoring a degree of freedom in the status file
You can write the current value of a specified point and degree of freedom to the Abaqus/Standard status file. The value of the point and degree of freedom being monitored will appear in the status file for every increment written during the analysis.
When a degree of freedom is monitored in the Abaqus/Standard status file, the same information is written to the message file (see above), but the specified frequency has no effect on the output to the status file.
Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value.
Input File Usage: *MONITOR, NODE=node_number, DOF=dof
The node and degree of freedom being monitored can be changed from step to step by repeating the *MONITOR option. The node and degree of freedom specified in the last occurrence of this option in a step will be used for that step.
Abaqus/CAE Usage: Step module: Output→DOF Monitor: Monitor a degree of freedom throughout the analysis, click Edit to select the point, Degree of freedom: dof
In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step.
Alternate output formats in Abaqus/CFD
By default, when you request output in Abaqus/CFD, the output is sent to the output database file. However, you have the option of selecting alternate file formats for field and history output. History output can be sent to files in comma-separated values (CSV) format instead of the output database formats.
You request the field and history output in the same manner as described in “Requesting output to the output database.” To select an alternate output format, you set the field and history options on the command line when you run an Abaqus/CFD analysis. For more information, see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2.
History output in CSV format
The comma-separated values (CSV) format is a text-based output format. The format of the CSV text file consists of one or more comment lines followed by one line of comma-separated data per history output frame. Comments in the CSV file begin with the character #. Each column in the CSV file has a comment that describes the mesh location, the part instance, and the output request label. Possible values for mesh locations are node, element, or surface. Vector output requests also include the component; i.e., 1, 2, or 3.
This format uses file extension csv. History output in the CSV format creates one file per output request label per step. Additional files are created if the job is run in parallel and the set associated with the history output request is split between processors due to the domain decomposition. In this case there will be one file per processor on which the set is present. The files are named job_outputrequest_rank_step-number.csv, where rank is a number ranging from 0 to one less than the number of CPUs.
Input File Usage: Use the following command line option to write history output to an alternate file format in Abaqus/CFD:
\mathbf { a b a q u s j o b } { \mathbf { - } } j o b { \mathbf { - } } n a m e { \mathbf { \ b i s t o r y { = } } } \mathbf { c s v }
Abaqus/CAE Usage: You cannot select an alternate format for history output in Abaqus/CAE.
Requesting output in multiple steps
In general, output requests apply to the step in which they are given and to all subsequent steps until they are respecified. However, output specifications for linear perturbation steps (available only in Abaqus/Standard; see below and “General and linear perturbation procedures,” Section 6.1.3) are treated independently of output requests for general analysis steps and apply only to a continuous sequence of linear perturbation steps.
Database output, printed output, and results file output are independent output modes in Abaqus; therefore, changing the specification for one form of output does not affect the other forms.
General analysis steps
The default output requests are used in the first general analysis step of an analysis unless you redefine them. For subsequent general analysis steps, the definition of each form of output from the previous general step is maintained unless you redefine it.
Linear perturbation steps
The default output requests are used in the first of any sequence of linear perturbation steps unless they are redefined in that step. If a subsequent linear perturbation step is defined without an intermediate general analysis step, the definition of each mode of output from the previous perturbation step is maintained unless you redefine it. If an intermediate general step is defined, the default output requests are again used in the linear perturbation step unless they are redefined in that step.
Element matrix output in Abaqus/Standard
In Abaqus/Standard you can write element stiffness matrices and, if available, mass matrices for each step to a file. For heat transfer elements the operator matrices are written if stiffness matrix output is requested.
Element matrix output is available only for elements without internal nodes (unless those nodes have no active degrees of freedom) and with no acoustic or internal degrees of freedom. Examples of elements for which element matrix output is prohibited include acoustic, pipe, elbow, frame, gap, and interface elements as well as axisymmetric elements with Fourier modes. Element matrix output is not available for elements with coupled fields such as coupled temperature-displacement elements and pore pressure elements. For incompatible mode and hybrid elements, stiffness matrix output is prohibited while mass matrix output is available. A substructure matrix output request is used to write a substructure’s reduced stiffness matrix, mass matrix, and load case vectors to a file (see “Defining substructures,” Section 10.1.2).
Element matrix output cannot be requested in a mode-based dynamic analysis (response spectrum, steady-state dynamic, modal dynamic, or random response). However, it can be requested in the eigenfrequency extraction analysis that precedes the mode-based dynamic analysis to output the mass and stiffness matrices.
The element matrices are written without the effects of nodal conditions; therefore, boundary conditions, concentrated loads, and the effects of multi-point constraints are not included in this output. The degrees of freedom are always in the global directions, even if a local coordinate system
(“Transformed coordinate systems,” Section 2.1.5) has been defined at nodes associated with the element.
You must select the element set for which output is requested. For models defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1), element numbers written with element matrix output are internal numbers generated by Abaqus/Standard. A map between internal numbers and the original element numbers and part instance names is provided in the data file.
Writing the element matrices to the results file
By default, element matrix output records are written to the Abaqus/Standard results file. The record formats for the results file are described in “Results file output format,” Section 5.1.2. The file can be written in binary or ASCII format based on the file format you specify (see “Controlling the format of the results file in Abaqus/Standard” above).
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=element_set, OUTPUT FILE=RESULTS FILE
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Writing the element matrices to a user-defined file
You can write the element matrices to a user-defined file. The file name should not include an extension; the extension .mtx will be added. (See “Input syntax rules,” Section 1.2.1, for the syntax of userspecified file names.)
The format of the output file is compatible with the linear user element (see “User-defined elements,” Section 32.17.1).
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED, FILE NAME=output_file_name
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Writing the element matrices to the data file
You can write the element matrix records to the Abaqus/Standard data file.
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Including distributed loads
You can choose to write the load vector from distributed loads on the elements. By default, the load vector is not written.
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, DLOAD=YES or NO
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Controlling the frequency of element matrix output
You can control the frequency at which element matrix output will be written by specifying an output frequency in increments. By default, the element matrices will be output every increment (equivalent to an output frequency of 1). Specify an output frequency of 0 to suppress output of the element matrices. Unless the output is suppressed, the matrices will always be written at the last increment of a step.
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, FREQUENCY=N
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Writing the stiffness or operator matrix
You can choose to output the stiffness matrix (or operator matrix in heat transfer elements). By default, the stiffness (operator) matrix is not output.
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, STIFFNESS=YES or NO
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
Writing the mass matrix
You can choose to output the mass matrix. By default, element mass matrices are not output.
Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, MASS=YES or NO
Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE.
User-defined output variables in Abaqus/Standard
In Abaqus/Standard output quantities can be defined as functions of any element integration point variable listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, by using user subroutine UVARM. Then, output variable UVARMn can be requested for output to the data file, the results file, or the output database.
User-defined state variables in Abaqus/Standard
In Abaqus/Standard you can allocate solution-dependent state variables and define them in user subroutines defining material behavior, as well as user subroutines FRIC, UEL, and UINTER (see “User subroutines: overview,” Section 18.1.1). Output variable SDVn can be requested for output of these state variables to the data file, the results file, or the output database. For user-defined elements output variable SDVn cannot be requested for output to the output database.
Postprocessing with Abaqus/CAE
Abaqus/CAE provides interactive graphical postprocessing from the Abaqus output database file in the Visualization module (also licensed separately as Abaqus/Viewer). Capabilities include model and deformed shape plotting, contour plotting, vector plotting, X–Y plotting, and animation.
Data needed for restart in Abaqus/Standard are contained in several files that are generated when you request that restart data be written for an analysis: the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files. “Restarting an analysis,” Section 9.1.1, describes the writing of restart data in more detail.
In Abaqus/Standard you can extract output from the restart data and write it to new data (.dat), results (.fil), and output database (.odb) files using a postprocessing analysis procedure. If the original analysis included user subroutines, the postprocessing analysis procedure requires the specification of the user subroutines. The data, results, and output database file output requests are defined as described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3. The output requests should be defined exactly as they would be in an analysis, except that:
- The output frequency specification has no meaning and is, therefore, ignored (unless you are recovering additional output from a previous direct cyclic or low-cycle fatigue analysis). Instead, you specify each increment at which output is to be generated in the postprocessing procedure definition.
- No default output is provided to the output database. Furthermore, model information, such as boundary conditions, is not written to the output database.
- Element set energy information cannot be recovered since it is not written to the restart file.
- Output is not available for procedures that do not support restart; for example, linear perturbation procedures.
The element sets and node sets that are defined for the analysis can be used for defining output sets during the postprocessing procedure. Additional sets can also be defined for the postprocessing procedure. You specify the step number in the restart file from which output is required. You cannot obtain results at the beginning of a step (see below).
Input File Usage: *POST OUTPUT, STEP=step_number
When the *POST OUTPUT option is used, it must appear as the first option in the input file. No data lines from the analysis input file are required. This option can be repeated as often as necessary to obtain further output. Since *POST OUTPUT is a purely postprocessing procedure, analysis options must not appear in the input file.
Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE.
Recovering additional output from a direct cyclic analysis
If you use this postprocessing technique to recover additional output from a previous direct cyclic analysis (see “Direct cyclic analysis,” Section 6.2.6), you must specify the iteration number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original direct cyclic analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal
strains at each time increment in the original direct cyclic analysis since the results file is not stored in the restart analysis database.
Input File Usage: *POST OUTPUT, STEP=step_number, ITERATION=iteration_number
There are no data lines associated with this option if the ITERATION parameter is specified.
Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE.
Recovering additional output from a low-cycle fatigue analysis
If you use this postprocessing technique to recover additional output from a previous low-cycle fatigue analysis (see “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7), you must specify the cycle number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original low-cycle fatigue analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal strains at each time increment in the original low-cycle fatigue analysis since the results file is not stored in the restart analysis database.
Input File Usage: *POST OUTPUT, STEP=step_number, CYCLE=cycle_number
There are no data lines associated with this option if the CYCLE parameter is specified.
Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE.
Example
A job can be submitted using the following input file. The analysis for which restart data were written must be specified when you submit the job (using the oldjob parameter of the Abaqus execution procedure). This example creates a new data (.dat) file containing tabular data. The first two tables will contain data from increments 5 and 10 of Step 1 and will give the reaction forces of the nodes in the set CLAMP, which was defined when the analysis was run. The next table will contain data from increment 3 of Step 2 and will give displacements from the new node set TIP that is defined in this postprocessing analysis.
*HEADING
*POST OUTPUT, STEP=1
5, 10
*NODE PRINT, NSET=CLAMP
RF,
*POST OUTPUT, STEP=2
3,
*NSET, NSET=TIP
1200, 1203, 1205
*NODE PRINT, NSET=TIP
U,
The following example input file recovers additional output from a previous direct cyclic analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Iteration 5 of Step 1, followed by data from each increment in Iteration 10 of Step 1:
*HEADING
*POST OUTPUT, STEP=1, ITERATION=5
*OUTPUT, HISTORY
*ELEMENT OUTPUT, ELSET=ELIST
S,E
*POST OUTPUT, STEP=1, ITERATION=10
*OUTPUT, HISTORY
*ELEMENT OUTPUT, ELSET=ELIST
S,E
The following example input file recovers additional output from a previous low-cycle fatigue analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Cycle 5 of Step 1, followed by data from each increment in Cycle 10 of Step 1:
*HEADING
*POST OUTPUT, STEP=1, CYCLE=5
*OUTPUT, HISTORY
*ELEMENT OUTPUT, ELSET=ELIST
S,E
*POST OUTPUT, STEP=1, CYCLE=10
*OUTPUT, HISTORY
*ELEMENT OUTPUT, ELSET=ELIST
S,E