Controlling the Nastran iterative solver

For certain Nastran solution sequences, you can use an iterative solver.

• In Simcenter Nastran, you can choose between a global iterative and an element iterative solver.

• In MSC Nastran, you can use a global iterative solver.

Both the Nastran global and iterative solvers are supported in Pre/Post.

Global iterative solver

In Pre/Post, you can use the global iterative solver in Simcenter Nastran and MSC Nastran SOL 106, 108, 111, and 153 analyses. With the global iterative solver, the software assembles the system stiffness matrix.

Element iterative solver

The element iterative solver is supported by Simcenter Nastran in SOL 101, and 401 analyses only. You can include contact conditions in SOL 101 analyses with the iterative solver. With the element iterative solver, the software works entirely from the element matrices. Use of the element iterative solver yields typical run time improvements of 4x to 6x compared to the global iterative solver. Additionally, the element iterative solver uses significantly less disk space. These performance gains are most noticeable with models composed of mostly solid elements.

There are several restrictions for using the element iterative solver. For example, the element iterative solver does not support superelements or inertia relief. For a complete list of these restrictions, see remark 2 for the ITER entry in the Simcenter Nastran Quick Reference Guide.

For more information, see Iterative Solutions in the Simcenter Nastran Numerical Methods User's Guide and Contact Conditions with the Element Iterative Solver.

Configuring the Nastran iterative solver in Pre/Post

In Pre/Post, when you create a Nastran solution type that supports the iterative solver, you can select the Global Iterative Solver or the Element Iterative Solver option on the General Page of the Create Solution dialog box. When you export or solve the solution:

• If you select the Global Iterative Solver option, the software specifies ITER = YES on the NASTRAN statement in your input file.

• If you select the Element Iterative Solver option, the software specifies both ELEMITER = YES and ITER = YES on the NASTRAN statement in your input file.

Optionally, you can create either an Element Iterative Solver or Global Iterative Solver modeling object to modify any of the default options for the iterative solver, such as the maximum number of iterations. The options in the Element Iterative Solver Options and Global Iterative Solver Options dialog boxes correspond to the fields on the ITER bulk data entry. If you do not create an Element Iterative Solver or Global Iterative Solver modeling object, the software uses the defaults for the ITER bulk data entry.

For more information, see Element Iterative Solver dialog box (Nastran) and Global Iterative Solver dialog box.

Learn more

Simcenter Nastran and MSC Nastran environments

Previewing Nastran solver syntax

Allocating DBset size

Modeling thermal strain in a Nastran analysis

Printing bulk data in your results file

Customizing a Nastran input file with user defined text

Look up more details

Simcenter Nastran and MSC Nastran boundary conditions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Controlling the Nastran iterative solver, 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 } });