Controlling compaction of boundary conditions

In the Abaqus environment, you can control how the software compacts loads and constraints that you define in one step and then propagate to subsequent steps. Compacting loads provides a more structured input file (.inp) because the file does not contain redundant information. For example, the software does not write node or element information in the step definitions. Therefore, it is much easier to manage the file, such as manually add missing keywords.

The software compacts the loads that belong to the Abaqus concentrated (*CLOAD) and distributed (*DLOAD) load families. The following table shows the loads per family.

CLOADs		DLOADs
Force		Pressure
Moment		Hydrostatic Pressure
Bearing		Centrifugal Pressure
Torque		Gravity
Bolt-preload (force on 1D and force on 3D)

To set the compaction, use the Compact when Propagated check box in the Customer Defaults dialog box. It corresponds to the OP parameter in Abaqus boundary conditions.

• If you clear the Compact when Propagated check box, all boundary conditions defined in a previous general analysis step remain active in subsequent steps. You can modify the existing boundary conditions or add new ones. This is how previous releases worked and it is the default behavior in the current release. It corresponds to OP=MOD.

• If you select the Compact when Propagated check box, the software removes all previously applied boundary conditions in a step, and requires that you specify new ones, including boundary conditions that you want retained. This corresponds to OP=NEW.

Exporting reused node sets as one set

The Compact when Propagated check box also controls how the software exports Abaqus node sets (NSETs) that you reuse in different Temperature Load boundary conditions.

For example, if you reuse the node set group GroupFaceRight in two different Temperature Loads (Temperature1 and Temperature4) in two different steps, the software does the following depending on how you set the check box:

• When you select the Compact when Propagated , the software exports the node set as a single node set, GroupFaceRight, in both steps. **% ====== STEP NUMBER 1 ====== **% ... **%Comment Temperature(1) (tempLoad) **% *TEMPERATURE GroupFaceRight, 1.500000E+02 ... **% ====== STEP NUMBER 2 ====== **Temperature(4) (tempLoad) **% *TEMPERATURE, OP=NEW GroupFaceRight, 7.500000E+01 ...

• If you clear the check box, the software exports the node set as two separate NSETs named for the temperature in which they are referenced. In this case, Temperature1 and Temperature4. **% ====== STEP NUMBER 1 ====== **% ... **%Comment Temperature(1) (tempLoad) **% *TEMPERATURE LOAD_Temperature(1), 1.500000E+02 ... **% ====== STEP NUMBER 2 ====== **% **%Comment Temperature(4) (tempLoad) **% *TEMPERATURE, OP=NEW LOAD_Temperature(4), 7.500000E+01 ...

Importing simulations with propagated boundary conditions

Use the Import compact LBC if propagated check box in the Import Simulation dialog box to control how the software imports boundary conditions that you define in one step and propagate to subsequent steps. When you select this check box, Pre/Post creates the appropriate load or constraint in the step and then applies it to subsequent steps.

For example, if the Abaqus input file contains a *CLOAD that propagates to subsequent steps, Pre/Post creates the appropriate load, such as a force, and applies that force to the subsequent steps.

Where do I find it?

Customer defaults

Prerequisite	Abaqus solver
Command Finder	Customer Defaults
Location in dialog box	Simulation→Pre/Post→Abaqus→ Formatting tab→ Compact when Propagated check box

Export a simulation file

Application	Pre/Post
Prerequisites	A Simulation file as the work part and the displayed partAbaqus as the specified solver
Menu	File→Export→Simulation

Import a simulation file

Application	Pre/Post
Menu	File→Import→Simulation

How do I

Create Abaqus conventional formulation shell elements

Learn more

Creating transition hybrid meshes

Abaqus attributes for time-dependent fields

Control parameters for Abaqus analyses

Monitoring nodes to gauge the progress of a solution (Abaqus)

Customizing Abaqus input files with user-defined text

Restarting Abaqus analyses

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Controlling compaction of boundary conditions, 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 } });