WS18-1 WORKSHOP 18 MODAL TRANSIENT ANALYSIS OF THE TOWER MODEL WITH SEISMIC INPUT NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation. - презентация

1 WS18-1 WORKSHOP 18 MODAL TRANSIENT ANALYSIS OF THE TOWER MODEL WITH SEISMIC INPUT NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation

2 WS18-2 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation

3 WS18-3 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation MODAL TRANSIENT ANALYSIS OF TOWER n Problem Description u The purpose of this exercise is to use the Modal Transient analysis on a tower to simulate the response from an earthquake. The El Centro earthquake data will be used as the seismic input to the tower, and it will be applied to the bottom of the tower via a RBE2 element. The analysis will have a 1 % modal damping applied to the model.

4 WS18-4 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation MODAL TRANSIENT ANALYSIS OF TOWER n Problem Description (cont.) Seismic Input

5 WS18-5 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation MODAL TRANSIENT ANALYSIS OF TOWER n Suggested Exercise Steps 1. Import the tower geometry from a Nastran Input File. 2. Create a Non Spatial Field by importing seismic_input.xyd. 3. Change the range to 400 points. 4. Create a load case called earthquake. 5. Apply an acceleration to the base of the tower using the seismic_input field. 6. Submit the model to Nastran for analysis. 7. Attach the XDB results file. 8. Create a XY Graph of the results.

6 WS18-6 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation CREATE NEW DATABASE Create a new database called earthquake.db. a.File / New. b.Enter earthquake as the file name. c.Click OK. d.Choose Default Tolerance. e.Select MSC.Nastran as the Analysis Code. f.Select Structural as the Analysis Type. g.Click OK. a b c d e f g

7 WS18-7 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 1. File / Import Import the model from a Nastran Input File. a.File / Import. b.Select MSC.Nastran Input as the Source. c.Select enf111. bdf and click Apply. d.Click OK when the Nastran Input File Import Summary appears. b c a c d

8 WS18-8 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 2. XY Plot: Create / XYWindow Create Non Spatial field. a.Fields: Create / Non Spacial / Tabular Input. b.Enter seismic_input for the Field Name. c.Click Input Data… d.Click Import/Export… e.Select seismic_input.csv. f.Click Apply. g.Click OK. h.Click Apply. a b c d e f g h

9 WS18-9 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 3. XY Plot: Create / Curve (Cont.) Create Non Spatial field. a.Fields: Show. b.Click Specify Range… c.Change the No. of Points to 400. d.Click OK. e.Click Apply. f.Click Unpost Current XYWindow. a b c d

10 WS18-10 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 5. Load Cases: Create Create a Time Dependent load case called earthquake. a.Load Cases: Create. b.Enter earthquake for the Load Case Name. c.Change the Load Case Type to Time Dependent. d.Click on Assign/Prioritize Loads/BCs button. e.Select Displ_spc1.1 from the Select Individual Loads/BCs box. f.Click OK. g.Click Apply. a b c d e f g

11 WS18-11 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Loads/BCs: Create / Acceleration / Nodal Apply the seismic input onto the tower structure. a.Loads/BCs: Create / Acceleration / Nodal. b.Enter seismic_input for the New Set Name. c.Click on Input Data button. d.Enter 9.81 for the Scale Factor. e.Enter for the Trans Accel, and select seismic_input field in the Time/Freq. Dependence box. f.Click OK. g.Click Select Application Region. h.Change the Geometry Filter to FEM. i.Select the Independent Node of RBE2 in the Select Nodes field. j.Click Add and Click OK. k.Click Apply. a b c d e h i j j k g f

12 WS18-12 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Loads/BCs: Create / Acceleration / Nodal (Cont.)

13 WS18-13 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Analyze / Entire Model / Full Run Submit the model for analysis. a.Analysis: Analyze / Entire Model / Full Run. b.Enter earthquake analysis for the Job Name. c.Click on Solution Type. d.Select TRANSIENT RESPONSE. e.Make sure the Formulation is Modal. f.Click OK. a b c d e f

14 WS18-14 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Click on Subcases. b.Select earthquake from the Available Subcases box. c.Click on Subcase Parameters. d.Click on DEFINE TIME STEPS. e.Enter the value and setting as shown in the table. f.Click OK. a b c d f e

15 WS18-15 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Select Struct. Damp. (G) from the pull down menu. b.Click on DEFINE MODAL DAMPING. c.Click Add Row. d.Enter the values shown in the table. e.Click OK on both forms. a b c d e e

16 WS18-16 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Click on Output Request. b.Select Accelerations from the Select Result Type box. c.Click OK. d.Click Apply. e.Click Cancel. a b c d e

17 WS18-17 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Click on Subcase Select. b.Click on Default in the Subcases Selected box to unselect the Default subcase. c.Click on earthquake in the Subcases For Solution Sequence box. d.Click OK. e.Click Apply to submit the model to Nastran for analysis. a c d e

18 WS18-18 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 8. Analysis: Access Results / Attach XDB / Result Entities Attach the XDB result file. a.Analysis:Access Results / Attach XDB / Result Entities. b.Click on Select Results File. c.Select earthquake_analysis.xdb. d.Click OK. e.Click Apply. a b c d e

19 WS18-19 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 9. Results: Create / Graph / Y vs X Create a graph of displacement versus frequency. a.Results: Create / Graph / Y vs X. b.Click on earthquake result case. c.Click on Filter. d.Click Apply. e.Click on Close. a b c d e

20 WS18-20 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 9. Results: Create / Graph / Y vs X (Cont.) Create a graph of displacement versus frequency (cont.). a.Select Acceleration, Translational. b.Change the option for Quantity to X Component. c.Click on Target Entities Icon. d.Select one of the corner nodes on the top of the tower that carries a lumped mass. e.Click Apply. a c d e b

21 WS18-21 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation Step 9. Results: Create / Graph / Y vs X (Cont.)

22 WS18-22 NAS122, Workshop 18, August 2005 Copyright 2005 MSC.Software Corporation