Generating specific component output for elements and nodal sums of forces and moments (Simcenter Nastran)

When you request output for element stress, strain, or force, Simcenter Nastran computes all of the components for the stress, strain, or force output. Similarly, when you request nodal (grid point) output for force and moment, Simcenter Nastran sums all the forces and moments for all of the contributing elements. Both of these output requests can result in large .f06 files and a large number of post-processing views, especially if you are interested in the same output requests for multiple load cases. Navigating through the .f06 file and post-processing views can be very time consuming. To help you target just the element or nodal output requests that you want, you can use the monitor point modeling objects:

• To request output for specific components of element stress, strain, or force, use the Monitor Point – Element Monitor output request. For example, you can request only the normal X stresses on a hexahedral element.In the .f06 file, Simcenter Nastran outputs the results in a table titled STRUCTURAL INTERNAL MONITOR POINT LOADS (MONPNT2).Tip: If you want to search for the table name in the .f06 file, add spaces between the letters (S T R U C T U R A L I N T E R N A L M O N I T O R P O I N T L O A D S). Otherwise, you can search for MONPNT2, or the Monitor Point Identification name or label you assign to the monitor point modeling objects that you create.

• To request output for summed nodal (grid point) forces and moments at a specified, integrated load point, use the Monitor Point – Sums Grid Point Forces output request. For example, you can request the summed forces and moments around a point for only a node, or a node and contributing elements attached to the node.In the .f06 file, Simcenter Nastran outputs the results in a table titled STRUCTURAL INTEGRATED FREE BODY MONITOR POINT LOADS (MONPNT3). Tip: If you want to search for the table name in the .f06 file, add spaces between the letters (S T R U C T U R A L I N T E G R A T E D F R E E B O D Y M O N I T O R P O I N T L O A D S). Otherwise, you can search for MONPNT3, or the Monitor Point Identification name or label you assign to the monitor point modeling objects that you create.

You can further control the results output by limiting it to specific subcases. To control the results output, you use the Monitor Point Type to Output option, which adds a MONITOR case control command to the Simcenter Nastran .dat input file. You can specify this option for all subcases on the Case Control page in the Solution dialog box or for an individual subcase in the Solution Step dialog box.

With this targeted output, you can more easily examine and interpret large amounts of output data in the .f06 file. This may help you to detect problems such as, for example, an unintentional loading path in your model that might otherwise go unnoticed. You can also import the file into your own proprietary post-processor.

For more information on the Simcenter Nastran bulk entries used for monitoring points, and for an input file example that you can import into Pre/Post, see Monitoring results in the Simcenter Nastran User’s Guide.

Where do I find it?

Creating a Monitor Point – Element Monitor or Monitor Point – Sums Grid Point Forces modeling object

Application	Pre/Post
Prerequisite	A Simulation file as the work part and the displayed partSimcenter Nastran as the specified solverOne of the following as the specified analysis type:StructuralAxisymmetric StructuralVibro-AcousticOne of the following as the specified solution type:SOL 101 Linear Statics – Global Constraints (Structural or Axisymmetric Structural analyses)SOL 101 Linear Statics – Subcase Constraints (Structural or Axisymmetric Structural analyses)SOL 103 Real Eigenvalues (Structural or Vibro-Acoustic analyses)
Command Finder	Modeling Objects
Location in dialog box	Modeling Objects Manager dialog box→Type list

Controlling results output of the monitor point requests with the Monitor Point Type to Output option

Application	Pre/Post
Prerequisite	A Simulation file as the work part and the displayed partSimcenter Nastran as the specified solverOne of the following as the specified analysis type:StructuralAxisymmetric StructuralVibro-AcousticOne of the following as the specified solution type:SOL 101 Linear Statics – Global Constraints (Structural or Axisymmetric Structural analyses)SOL 101 Linear Statics – Subcase Constraints (Structural or Axisymmetric Structural analyses)SOL 103 Real Eigenvalues (Structural or Vibro-Acoustic analyses)
Simulation Navigator	Right-click an active solution or solution step→Edit
Location in dialog box	Solution dialog box→Case Control pageSolution Step dialog box→Properties group

How do I

Request output for specific components of element stress, strain, and force (Simcenter Nastran)

Request output of sum of nodal forces and moments at an integrated load point (Simcenter Nastran)

Learn more

Requesting output for Nastran analyses

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Generating specific component output for elements and nodal sums of forces and moments (Simcenter Nastran), 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 } });