Simcenter Nastran graphs

For Simcenter Nastran solutions, as your solve progresses, one or more graphs showing progress or convergence are generated. You can view graphs as they are generated in real time, or you can review all graphs at the completion of the solve.

• To view the graphs in real time, in the Solution Monitor, choose Graphs .

• To locate the graphs when the solve is complete and the Solution Monitor is closed, right-click the solution and choose Browse. The graphs are saved as PNG files.

Sparse Matrix Solver graph

This graph is available for all solutions that employ the sparse matrix solver.The number of equations completed displays at the top of the Sparse Matrix Solver page, and the graph plots the number of completed equations against the number of supernodes processed. A supernode is a group of columns in the sparse matrix data structure.Sparse Matrix graph

Iterative Solver Convergence graph

This graph is available when you perform a linear statics analysis (SOL101) using the iterative solver. The current iteration and load number are displayed at the top of the Iterative Solver Convergence page, and the graph plots the convergence value against the iteration number. The solution is complete when the convergence value falls within the convergence tolerance.

Contact Analysis Convergence graph

This graph is available when you perform a linear statics analysis (SOL101) with contact.The number of contact changes and the current load number are displayed at the top of the Contact Analysis Convergence page, and the graph plots the percentage of contact changes against the iteration number. The solution is considered converged when the number of contact changes falls below the value of Allowable Contact Changes specified in the Contact Parameters modeling object.Contact Convergence graph

Eigenvalues Extraction graph

This graph is available when you use the Lanczos method to extract eigenvalues for normal modes analysis. Supported solutions include SOL 103 Real Eigenvalues, SOL 103 – Response Dynamics, SOL 105 Linear Buckling, SOL 111 Modal Frequency Response, and SOL 112 Modal Transient Response.The number of eigenvalues extracted is displayed at the top of the Eigenvalues Extraction page, and the graph plots the number of eigenvalues extracted against the number of shift points. The extraction is considered complete when the number of eigenvalues meets or exceeds the number requested.

DOF curve graph

This graph is available when you perform a direct or modal response analysis. Supported solutions include SOL 108 Direct Frequency Response, SOL 109 Direct Transient Response, SOL 111 Modal Frequency Response, and SOL 112 Modal Transient Response.For SOL 108 Direct Frequency Response and SOL 109 Direct Transient Response, the page title displays the node number and direction. By default, this represents the first DOF in the l-set. For more information, see Displacement Vector Sets in the Simcenter Nastran Basic Dynamic Analysis User's Guide.Note: To monitor a DOF other than the first DOF in the l-set, specify the grid number and degree of freedom using the MGRID and MDOF parameters in the PARAM bulk data entry or case control command.For SOL 111 Modal Frequency Response and SOL 112 Modal Transient Response, the page title displays the modal displacement for the first mode.The current time or frequency and the current amplitude are displayed at the top of the page, and the graph plots the amplitude against time or frequency. When time or frequency equals 0, the solution is complete.

Nonlinear History graph

This graph is available when you perform a nonlinear analysis. Supported solutions include SOL 106 Nonlinear Statics, SOL 153 Steady State Nonlinear Heat Transfer, SOL 601,106 Advanced Nonlinear Statics, and SOL 601,129 Advanced Nonlinear Transient.The current iteration and subcase are displayed at the top of the Nonlinear History page, and the graph plots the load factor against the iteration number. The solution is considered complete when the iteration error falls within the defined error tolerances.

Load Step Convergence graph

This graph is available when you perform a nonlinear analysis. Supported solutions include SOL 106 Nonlinear Statics, SOL 601,106 Advanced Nonlinear Statics, and SOL 601,129 Advanced Nonlinear Transient.The current time step and specified absolute convergence tolerance values are displayed at the top of the Load Step Convergence page. To generate the graph, all convergence tolerance values are normalized to 1.0, and the graph then plots the normalized convergence ratios for each convergence criterion against the iteration number. The solution is considered complete when all convergence ratios fall below 1.0.

Contact / Materials status

This set of graphs is available when you perform a SOL 402 nonlinear analysis. These reports display the number of plastic, creep, or damaged elements, or the number of nodes in contact.The Number of Creep Elements graph displays the evolution of creep elements during the analysis, which is useful when you want to know the total number of elements for which the creep started, or how the number of creep elements changes as the solution converges.

Convergence

This set of graphs is available when you perform a SOL 402 nonlinear analysis.Time steps displays the time steps, the elapsed time, and the number of Newton iterations that were used to make the solution converge.Convergence criteria displays the SOL 402 convergence criteria that you set in the Nonlinear Control Parameters - Subcase modeling object.Force (TESF), whose threshold is set by Relative Force Tolerance (PRCR) Force (TESE), whose threshold is set by Relative Energy Tolerance (PRCE) Displacement (TESQ), whose threshold is set by **Relative Displacement Tolerance (PRCQ)**Cumulative Iteration displays the cumulative iterations versus time.

Energy

This graph is available when you perform a SOL 402 nonlinear analysis. The Energy evolution graph displays the work done by internal forces, the work done by external forces, and, for dynamic subcases, the kinematic energy.

Note:

If you created a Report simulation object to monitor nodal displacement, velocity, or acceleration, the graph appears in the Graphs list with the name you gave it in the Report dialog box. For more information, see Displaying graphs in the Solution Monitor using the Report simulation object.

How do I

Solve the model

Adjust advanced solver options

Disable or enable the Solution Monitor

Browse to results files

Set up an Update Agent for use with Product Template Studio

Learn more

Solving models

Analysis Job Monitor

Checking analysis quality

Solution Monitor

Batch solving

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Simcenter Nastran graphs, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });