10.2.1.2. Generation of Input File

The user gets input files to make an rfi file following steps.

10.2.1.2.1. CMS Analysis (Mechanical APDL)

This section explains how to build FE model and analyze it with CMS method.

The example model is 2D rectangular model. The model can be meshed as shell 63 element with Element edge length option. Shell 63 elements have Real Constant with thickness, 0.05. Steel material is used in this model.

../_images/image04516.png

Figure 10.11 Target model

  1. Select Mechanical APDL Product Launcher on the popup menu and specify working directory and job name.

    ../_images/image04616.png

    Figure 10.12 ANSYS launcher

  2. Select Structural on the Preferences for GUI filtering

    • Preferences for GUI filtering

      • Preferences > Structural

    ../_images/image04717.png

    Figure 10.13 Preference for GUI filtering

  3. Select Element Type, Real Constants

    • Element type

      • Preprocessor > Element Type > Add/Edit/Delete > Add… > Shell 63 > OK > Close

    ../_images/image04818.png

    Figure 10.14 Set Element Type

    • Enter Real Constants

      • Preprocessor > Real Constants > Add/Edit/Delete > Add > OK

      • Set shell thicknesses I, J, K, L as 0.05

    ../_images/image04915.png

    Figure 10.15 Real constant for shell element

    • Thickness

      • Thickness is important parameter for shell element. Ansys do not support Real Constant for some shell element.
        At the time, thickness can be define using shell section.
    ../_images/image05015.png

    Figure 10.16 Create Sections for Shell Element

  4. Enter Material property

    • Material property

      • Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic > Specify material number as 1 > OK

      • Fill in the Young’s modulus(70e9 \(N/m^2\)), Poisson’s ratio(0.33), density(2710 \(kg/m^3\)) > OK

    ../_images/image05116.png

    Figure 10.17 Material Property

  5. Create rectangular geometric entity

    • Create Rectangle by Dimensions

      • Preprocessor > Modeling > Create > Areas > Rectangle > By Dimensions > OK

      • Fill the x1, x2, y1, & y2 as 0.0, 0.0, 1.0, & 1.0 > OK

    ../_images/image05218.png

    Figure 10.18 Rectangle by Dimensions

  6. Create area meshing using Mesh Tools

    • Use line set to define element edge length.

      • Preprocessor > Meshing > MeshTool > Size Controls > Lines > Pick All > OK > SIZE element edge length(0.1) > OK

    ../_images/image05315.png

    Figure 10.19 Line set with Element edge length

    • Mesh model

      • Mesh Tool > Mesh > Select model > OK

    ../_images/image05419.png

    Figure 10.20 Meshed Rectangular geometric entity

    ../_images/image05514.png

    Figure 10.21 Mesh Result

  7. Define Interface nodes

    • Select> Component Manager

    • Create Component

      • Create from ‘Nodes’

      • Check ‘Pick entities’

      • Name new component ‘INTERFACE’

    • Select interface nodes on FE model

    ../_images/image05615.png

    Figure 10.22 Create new component

    ../_images/image05714.png

    Figure 10.23 Select Interface nodes

  8. Define Parameter

    • Parameters> Scalar Parameters

    • Input the number of modes like ‘NMODES=10’

    • Accept it

    ../_images/image05815.png

    Figure 10.24 Set the number of modes

  9. Read RecurDyn’s input file for CMS analysis

    • File> Read Input from

    • Read ‘RecurDyn_AnsysCMS.MAC’

      • This macro input file is included in the following folder.

      • ‘<Install Dir>\Toolkits\Flexible input files\ANSYS’

    ../_images/image05915.png

    Figure 10.25 Created files

  10. Check the result files.

  11. The four files must exist in work folder.

    • genCMS.rst

    • genCMS.mp

    • genCMS.emat

    • genCMS.cm

Caution

  • The user can perform the CMS(Component Mode Synthesis) analysis in ANSYS. CMS allows the user to derive the normal modes and static correction modes at once from ANSYS. It is difficult to perform CMS analysis by the provided steps of ANSYS. So, it is strongly recommended that the user performs CMS analysis with the provided macro file (RecurDyn_AnsysCMS.MAC). This macro file is included in <Install Dir>\Toolkits\Flexible input files\ANSYS\RecurDyn_AnsysCMS.MAC.

  • If ANSYS does not generate the element matrices file automatically, use the EMATWRITE command. If the user uses the macro file, this command is not needed.

  • If ANSYS does not generate the file included in material information automatically, the user should type the MPWRITE command in the solution menu. If the user uses the macro file, this command is not needed.

Note

The sample model is supported in <Install Dir>\Toolkits\Flexible input files\ANSYS directory.

10.2.1.2.2. CMS Analysis (Workbench)

This section explains how to build FE model and analyze it with CMS method in Workbench.

The example model is 2D rectangular model.

  1. Select Modal analysis in Analysis Systems.

    ../_images/image06015.png

    Figure 10.26 Modal analysis system

  2. Create a geometry for FE model.

    • Enter DesignModeler program in the popup menu on Geometry.

    ../_images/image06115.png

    Figure 10.27 Popup Menu on Geometry

    • Create a rectangle geometry in DesignModeler.

    1. Activate Sketching Toolboxes by clicking Sketching page next to Modeling page. Create a 1m*1m rectangle on XY Plane by using Draw and Dimensions feature.

    2. Create a surface from the sketch by using Surfaces From Sketches.

    3. Generate the geometry by using Generate.

    ../_images/image06217.png

    Figure 10.28 DesignModeler

  3. Create a FE model and Analysis.

    • Enter Edit… on the popup menu on Model.

    ../_images/image06316.png

    Figure 10.29 Popup Menu on Model

    • Define the thickness of the surface geometry as 0.05.

    • Define the material as Structural Steel.

    ../_images/image06415.png

    Figure 10.30 Setting the thickness

    • Mesh the surface geometry.

    1. Set the element size as 0.1 by using Body Sizing.

    2. Set the mesh type as all quad in Automatic Method.

    3. Mesh with Generate Mesh.

    ../_images/image06515.png

    Figure 10.31 Mesh the surface geometry

  4. Define interface nodes.

    • Create a Remote Point to define interface nodes.

    1. Set four vertices as Geometry

    2. Set X, Y, and Z Coordinate as -0.1, 0.5, and 0.

    3. Set Rigid Behavior in Definition

    ../_images/image06617.png

    Figure 10.32 Setting Remote Point

    • Insert a Command to define the name for the remote point.

      “MASTER_1=_npilot”

    ../_images/image06716.png

    Figure 10.33 Command for Remote Point

    • Create a Point Mass to define mass element.

    1. Set Scoping Method as Remote Point.

    2. Set Remote Points as the created Remote Point.

    3. Set the mass as 1-e6 in Definition

    ../_images/image06817.png

    Figure 10.34 Setting Point Mass

  5. Solve Modal Analysis

    • Define Analysis Settings

      • In order to include strain shape and stress shape, check Output Controls.

      ../_images/image06917.png

      Figure 10.35 Analysis Settings

    • Solve

    ../_images/image07017.png

    Figure 10.36 Performing Modal Analysis

  6. Select Mechanical APDL in Component Systems

    ../_images/image07113.png

    Figure 10.37 Mechanical APDL in WorkBench

  7. Create a MAC file.

    • Insert a command for CMS analysis.

    1. Edit the macro input file contents provided by RecurDyn. The file is in <Install Dir>\Toolkits\Flexible input files\ANSYS folder.

    2. NMODES and CM parameters should be inputted.

      “NMODES=10”

      “nsel,s,,,MASTER_1”

      “CM,INTERFACE,node”

    3. Save the modified file

    ../_images/image07210.png

    Figure 10.38 Edited MAC file

  8. Solve CMS Analysis.

    • Assign Model setting

    • Add created MAC file

    ../_images/image07312.png

    Figure 10.39 CMS Analysis setting

    • Solve

    ../_images/image0748.png

    Figure 10.40 Performing CMS Analysis

  9. Check the result files.

    • The file is in <ProjectFolder>dp0APDLANSYS

    • The four files must exist in this folder.

    • genCMS.rst

    • genCMS.mp

    • genCMS.emat

    • genCMS.cm

Note

For accurate analysis, Distribute Solution option should be turned off in Mechanical program.

../_images/image0758.png