FE model and boundary conditions

In Response Dynamics, a finite element (FE) model represents the physical model of the structure. In general, you define the geometry, material properties, mesh, and boundary conditions as you would for other structural solution types. This topic discusses some special considerations for creating the FE model for Response Dynamics.

Note:

For more information about defining the finite element model, see Meshing and Boundary conditions.

Supported element types for Response Dynamics

Some responses (functions or results) can be evaluated only at certain types of elements. When meshing your FE model, be sure to choose the proper element types for the responses you want. The tables below show the element types supported for different response functions and response results.

To evaluate these response function types...	Use these element types
Nodal displacements, velocities, and accelerations	Any (these functions are not related to elements)
Nodal reaction forces	Any (these functions are not related to elements)
Element forces	Beam elements (CBEAM, CBAR)Rod elements (CROD)Spring elements (CBUSH, CELAS2)
Unaveraged nodal stresses	Beam elements (CBEAM, CBAR)Rod elements (CROD)Thin shell elements (CQUAD4, CQUAD8, CTRIA6, CTRIA3, CTRIAR, CQUADR)Solid elements (CTETRA(10), CTETRA(4), CHEXA)
Unaveraged shell stress resultants	Thin shell elements (CQUAD4, CQUAD8, CTRIA6, CTRIA3, CTRIAR, CQUADR)

Special boundary conditions for Response Dynamics

Type	Description
Enforced motion location	The location of an enforced motion excitation on the model. This is a location only; you define the actual excitation after you solve the solution. The solver generates constraint modes, equivalent attachment modes, and effective masses based on the defined enforced motion locations.You can create enforced motion locations in the Constraints container in the Simulation Navigator.
Nodal Force location	The location of a nodal force excitation on the model. This is a location only; you define the actual excitation after you solve the solution. The solver generates attachment modes based on the defined nodal force locations.You can create nodal force locations in the Loads container in the Simulation Navigator.
Static offset load	For Transient events, a constant load for scaling the results (for example, a gravity load for use with concentrated mass elements, or a distributed wind load on the structure). The static results from this subcase will be added to the computed dynamic results.Create static offset loads in the Subcase – Static Offset container in the Simulation Navigator. After you solve the solution and create an event, the Static Offset node appears in the Simulation Navigator under the event node. You can exclude the static offset results from the response evaluation by right-clicking the Static Offset node and choosing Deactivate.
Stress stiffening load	Differential stiffness accounts for the stiffening or softening of a structure from loading. You can apply pre-loads for the differential stiffening of any structure. The differential stiffness is computed based on the displacements from the static loads. Relative to the unloaded stiffness, the differential stiffness can be significant for structures that are thin in one or two dimensions and have axial or membrane loads.The solver uses the pre-loads to augment the unloaded stiffness for the normal mode calculations. It calculates the differential stiffness and combines it with the unloaded linear stiffness, and then uses the combination for the normal modes eigenvalue problem. [ Kl ] = linear stiffness matrix [ Kσ ] = stress stiffness matrix λi = ωi2 = natural frequencies squared (eigenvalues) [ M ] = mass matrix {ψi} = mode shapes (eigenvectors)You can create differential stiffening loads in the Subcase – Stress Stiffening container in the Simulation Navigator.Depending on the structure and loading, the effect of the stress stiffening can be significant. For example, consider a plate with a tensile membrane load applied in subcase 2. This will stiffen the plate, and the bending modes will be higher than if there were no stress stiffening load. You would simulate this effect if there is to be some type of constant load applied with your dynamic loads, and you want to consider any stiffening effect of that load.
Dynamic load	A load that you scale after solving the solution. The solver generates a load set and distributed attachment modes for each dynamic load. You can then assign a scaling function when you create an excitation. Dynamic loads are necessary for applying distributed-load excitations and can also be used as static excitations in a Quasi-Static analysis event.You can create dynamic loads in the Subcase – Dynamics container in the Simulation Navigator.

How do I

Define Static Offset and Stress Stiffening

Define Dynamic loads for distributed-load excitations

Specify excitation locations

Learn more

Enforced motion and nodal force locations

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

FE model and 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 } });