6.3. Example: Spectrum Analysis (GUI Method)

In this example problem, you determine the seismic response of a beam structure. This problem is similar to VM70 in the Mechanical APDL Verification Manual.

 

6.3.1. Problem Description

A simply supported beam of length , mass per unit length m, and section properties shown in Problem Specifications, is subjected to a vertical motion of both supports. The motion is defined in terms of a seismic displacement response spectrum. Determine the nodal displacements, reactions forces, and the element solutions.

 

6.3.2. Problem Specifications

The following material properties are used for this problem:

E = 30 x 106 psi
m = 0.2 lb-sec2/in2

The following geometric properties are used for this problem:

I = (1000/3) in4
A = 273.9726 in2
= 240 in
h = 14 in

 

6.3.3. Problem Sketch

Figure 6.2: Simply Supported Beam with Vertical Motion of Both Supports

Simply Supported Beam with Vertical Motion of Both Supports
Response Spectrum
Frequency, HzDisplacement, in.
0.10.44
10.00.44

 

6.3.4. Procedure

 

6.3.4.1. Set the Analysis Title

  1. Select menu path Utility Menu> File> Change Title.

  2. Type the text "Seismic Response of a Beam Structure" and click on OK.

 

6.3.4.2. Define the Element Type

  1. Select menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.

  2. Click on Add. The Library of Element Types dialog box appears.

  3. Scroll down the list on the left to "Structural Beam" and select it.

  4. Click on "2 Node 188" in the list on the right.

  5. Click on OK. The Library of Element Types dialog box closes.

  6. Click on Options in the Element Types dialog box.

  7. Select Element Behavior K3 : Cubic Form. Click on OK.

  8. Click on Close in the Element Types dialog box.

 

6.3.4.3. Define the Cross-Section Area

  1. Select menu path Main Menu> Preprocessor> Sections> Beam> Common Sections. The BeamTool dialog box appears.

  2. Enter 71.6 for B and 3.82 for H. Click on Apply.

  3. Click on Close to close the BeamTool dialog box.

 

6.3.4.4. Define Material Properties

  1. Select menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.

  2. In the Material Models Available window, click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.

  3. Enter 30E6 for EX (Young's modulus), 0.30 for PRXY (Poisson's ratio), and then click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.

  4. Click on Density. A dialog box appears.

  5. Enter 73E-5 for DENS (density), and click on OK.

  6. Select menu path Material> Exit to remove the Define Material Model Behavior dialog box.

 

6.3.4.5. Define Keypoints and Line

  1. Select menu path Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.

  2. Enter 1 for keypoint number.

  3. Click on Apply to accept the default X, Y, Z coordinates of 0,0,0.

  4. Enter 2 for keypoint number.

  5. Enter 240,0,0 for X, Y, and Z coordinates, respectively.

  6. Click on Apply.

  7. Enter 3 for keypoint number.

  8. Enter 0,1,0 for X, Y, and Z coordinates, respectively.

  9. Click on OK.

  10. Select menu path Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.

  11. Click on "keypoint numbers" to turn keypoint numbering on.

  12. Click on OK.

  13. Select menu path Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Straight Line. A picking menu appears.

  14. Click on keypoint 1, and then on keypoint 2. A straight line appears between the two keypoints.

  15. Click on OK. The picking menu closes.

 

6.3.4.6. Set Global Element Density and Mesh Line

  1. Select menu path Main Menu > Preprocessor > Meshing > Size Cntrls > ManualSize > Global > Size. The Global Element Sizes dialog box appears.

  2. Enter 8 for the number of element divisions and click on OK. The Global Element Sizes dialog box closes.

  3. Select menu path Main Menu> Preprocessor> Meshing> Mesh Attributes> All Lines. The Line Attributes dialog box appears.

  4. Click on Pick orientation keypoint(s) and click on OK. A picking menu appears.

  5. In the graphic window, click once on the keypoint 3 and click on OK.

  6. Select menu path Main Menu> Preprocessor> Meshing> Mesh> Lines. A picking menu appears.

  7. Click on Pick All. The picking menu closes.

 

6.3.4.7. Set Boundary Conditions

  1. Select menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. A picking menu appears.

  2. In the graphics window, click once on the node at the left end of the beam.

  3. Click on OK. The Apply U,ROT on Nodes dialog box appears.

  4. In the scroll box of degrees of freedom to be constrained, click once on "UY" to highlight it.

  5. Click on OK.

  6. Repeat steps 1-3 and select the node at the right end of the beam.

  7. In the scroll box of degrees of freedom to be constrained, click once on "UX." Both "UX" and "UY" should be highlighted.

  8. Click on OK. The Apply U,ROT on Nodes dialog box closes.

  9. Select menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes box dialog appears.

  10. In the scroll box for Norml symm surface is normal to, scroll to “z-axis” and click on OK.

 

6.3.4.8. Specify Analysis Type and Options

  1. Select menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears.

  2. Click on "Modal" to select it and click on OK. The New Analysis dialog box closes.

  3. Select menu path Main Menu> Solution> Analysis Type> Analysis Options. The Modal Analysis dialog box appears.

  4. Click on "Block Lanczos" as the mode-extraction method (MODOPT).

  5. Enter 3 for the number of modes to extract.

  6. Enter 1 for the number of modes to expand (MXPAND).

  7. Click on the Calculate elem. results dialog button (MXPAND) to specify YES.

  8. Click on OK. The Modal Analysis dialog box closes, and the Block Lanczos Modal Analysis dialog box appears. Click OK to accept the default values.

 

6.3.4.9. Solve the Modal Analysis

  1. Select menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.

  2. Carefully review the information in the status window, and then click on Close.

  3. Click on OK on the Solve Current Load Step dialog box to start the solution.

  4. When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.

 

6.3.4.10. Set Up the Spectrum Analysis

  1. Select menu path Main Menu> Solution> Analysis Type> New Analysis. The New Analysis dialog box appears, along with a warning message that states: "Changing the analysis type is only valid within the first load step. Pressing OK will cause you to exit and reenter SOLUTION. This will reset load step count to 1." Click on CLOSE to close the warning message box.

  2. Click on "Spectrum" to select it, and click on OK. The New Analysis dialog box closes.

  3. Select menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Settings. The Settings for Single-point Response Spectrum dialog box appears.

  4. Select "Seismic displac" in the scroll box as the type of response spectrum.

  5. Enter 0,1,0 for excitation direction into the excitation direction input windows and click on OK.

 

6.3.4.11. Define Spectrum Value vs. Frequency Table

  1. Select menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Freq Table. The Frequency Table dialog box appears.

  2. Enter 0.1 for FREQ1, enter 10 for FREQ2, and click on OK.

  3. Select menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Spectr Values. The Spectrum Values - Damping Ratio dialog box appears.

  4. Click on OK to accept the default of no damping. The Spectrum Values dialog box appears.

  5. Enter 0.44 and 0.44 for FREQ1 and FREQ2, respectively.

  6. Click on OK. The Spectrum Values dialog box closes.

 

6.3.4.12. Select Mode Combination Method

  1. Select menu path Main Menu> Solution> Load Step Opts> Spectrum> Single Point> Mode Combine. The Mode Combination Methods dialog box appears.

  2. Select SRSS as the mode combination method.

  3. Enter 0.15 for the significant threshold.

  4. Select displacement for the type of output. Click OK. The Mode Combination Methods dialog box closes.

 

6.3.4.13. Solve Spectrum Analysis

  1. Select menu path Main Menu> Solution> Solve> Current LS. The Solve Current Load Step dialog box appears, along with a status window.

  2. Carefully review the information in the status window, and then click on Close.

  3. Click on OK on the Solve Current Load Step dialog box to start the solution.

  4. When the solution is finished, a dialog box stating "Solution is done!" appears. Click on Close.

 

6.3.4.14. Postprocessing: Print Out Nodal, Element, and Reaction Solutions

  1. Select menu path Main Menu > General Postproc > Results Summary. The SET Command listing window appears.

  2. Review the information in the listing window, and click on Close. The SET Command listing window closes.

  3. Select menu path Utility Menu> File> Read Input From. The Read File dialog box appears.

  4. From the right side of the Read File dialog box, select the directory containing your results from the scroll box.

  5. From the left side of the Read File dialog box, select the Jobname.mcom file from the scroll box.

  6. Click on OK. The Read File dialog box closes.

  7. Issue a PRNSOL,DOF command.

  8. Issue a PRRSOL,F command.

 

6.3.4.15. Exit Mechanical APDL

  1. In the Mechanical APDL Toolbar, click on Quit.

  2. Select the save option you want and click on OK.

You have completed this example analysis.