Fourier Multi Harmonic and 3D Coupling dialog box

Use this dialog box to create a simulation object that connects a 2D axisymmetric mesh edge with a 3D solid element face on a cyclic symmetry portion of a structure, or on a full 360-degree representation of the structure.

You can use the Fourier Multi Harmonic and 3D Coupling simulation object in a Simcenter Nastran Structural analysis (SOL 402 Multi-Step Nonlinear Kinematics) and Rotor Dynamics analysis (SOL 414,101, SOL 414,103, SOL 414,110, SOL 414,111, or SOL 414,129). For SOL 414,103, the Fourier Multi Harmonic and 3D Coupling is supported when the computation option is Eigenvalues.

Name
Name	Sets the name of the simulation object. The name appears in the Simulation Object Container and the Information window.
Description	Sets the description of the simulation object. The description appears in the Information window.You can use Cut , Copy , and Paste commands to copy and paste the description.
Destination Folder
Simulation Object Container	Specifies the folder in the Simulation Navigator in which to store the simulation object. The list includes the root container and existing folders that you created using the New Folder command. Examples of a root container include Load Container, Constraint Container, and Simulation Object Container.
Folder Manager	Displays a hierarchical list of existing folders. To create a new folder, right-click any level of the hierarchy and choose New Folder.
Source Region
Edge Region	Lets you select the element edge region of the 2D Fourier mesh to couple with the 3D mesh. The nodes of the edge are glued to the faces of the 3D mesh. Select an existing edge region or click Create Region to create a new edge region. For more information, see Working with reusable regions.To filter a long list of edge regions, click More Options to display options for searching and filtering the rotor regions.
Target Region
Surface Region	Lets you select the element faces of the 3D mesh to couple with the 2D Fourier mesh. Select an existing surface region or click Create Region to create a new surface region. For more information, see Working with reusable regions.To filter a long list of edge regions, click More Options to display options for searching and filtering the rotor regions.
Connection Nodes
Connection nodes are virtual nodes that are created on the faces of the 3D elements. They are used to create contact between the 2D and 3D meshes. The goal is to generate enough virtual nodes (contact) for the analysis to be effective, but not to over constrain the model by creating too many virtual nodes.
Virtual Nodes Generated	Specifies the method for determining the density of virtual nodes.By NumberLets you set the number of virtual nodes to create.By Distance Between NodesLets the software determine the number of virtual nodes based on the distance between nodes. Select this option when the length of the arc on which the nodes are to be glued is very different between the one closest to the axis of revolution and the one furthest away.For information on how the software generates the virtual nodes, see FMH3D in the Simcenter Nastran Quick Reference Guide.
Virtual Nodes Number (N)	Appears when Virtual Nodes Generated is set to By Number.Sets the number of virtual nodes to evenly space along the arc defined by the variation angle.For example, if the face of the 3D sector has 5 circumferentially equidistant nodes, a good number of virtual nodes is 4.
Distance Between Virtual Nodes Number (DIST)	Appears when Virtual Nodes Generated is set to By Distance Between Nodes.Sets the distance between adjacent virtual nodes as measured along the arc defined by the variation angle.
Automatic Angles Computation	Lets the software compute the initial (ANGLEI) and variation (ANGLED) angles. The initial and variation angles determine the location on the 3D mesh where the virtual nodes can be placed.You can retrieve the computed initial and variation angles from the .f06 file.When you clear this check box to add the initial and variation angles manually, do not include the borders of the 3D sector. For example, if the 3D sector is one of 52 sectors, each sector angle is 6.9° (360°/52 = 6.9°), so the sector starts at -3.45° and ends at 3.45°. To omit the borders in the initial and variation angles:Set Initial Angle (ANGLEI) to 3.21°.Set Variation Angle (ANGLED) to 5.32°, which is approximately 75% of the sector angle (6.9°).If you are connecting to a full 3D model, you can let the software compute the initial (ANGLEI) and variation (ANGLED) angles, or you can define a variation of 360 degrees.
Initial Angle (ANGLEI)	Appears when the Automatic Angles Computation check box is cleared.Sets the sweep angle in the circumferential direction that begins at the 2D edge region and ends at the beginning edge of the 3D surface region.
Variation Angle (ANGLED)	Appears when the Automatic Angles Computation check box is cleared.Sets the sweep angle in the circumferential direction that begins at the location determined by the initial angle and ends at a location near the ending edge of the 3D surface region.As a best practice, specify Variation Angle (ANGLED), such that it subtends 67-75% of the full angular sweep of a cyclic symmetric sector and it does not include both the beginning and ending edges of the cyclic symmetric sector.
Tolerance
The tolerance distances determine the area on the 3D mesh where the software can generate the virtual nodes.
Normal Search Distance (SDISN)	Sets a distance threshold such that when the normal distance between the virtual node and the 3D element face is less than the distance threshold, the software creates a glue connection between the virtual node and the 3D element face.
Tangential Search Distance (SDIST)	Applicable when a virtual node lies beyond the projected area of the 3D surface region.Sets a distance threshold such that when the tangential distance between the virtual node and the 3D element face is less than the distance threshold, the software creates a glue connection between the virtual node and the 3D element face.

These options are available when you click More Options .
Find	Lets you search for an object by typing the full name of the object. For example, to find a group named ABC_group, you must type ABC_group into the search box.After typing the name, press Enter or click Find . If the object is found, it is selected automatically.
Filter by Name	Lets you filter the list by the names of the objects. This filter supports wildcards. The default wildcard of * displays all entries in the list. For example, to filter the list to display every object with a name starting with the letter "a," enter a* as the filter string.
Filter by Label	Lets you filter the list by the names or labels of the objects. This filter supports wildcards. The default wildcard of * displays all entries in the list. For example, to filter the list to display every object with a name starting with the letter "a," enter a* as the filter string.

Learn more

Modeling axisymmetry (SOL 414)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Fourier Multi Harmonic and 3D Coupling dialog box, 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 } });