WS3-1 WORKSHOP 3 DIRECT TRANSIENT ANALYSIS NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation

WS3-2 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation

WS3-3 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation DIRECT TRANSIENT RESPONSE n Problem Description u Using the direct method, determine the transient response of the flat rectangular plate, created in Workshop 1a, subject to time- varying excitation. This example structure is excited by 1 psi pressure load over the total surface of the plate varying at 250 Hz. In addition, a 50 lb force is applied at a corner of the tip also varying for the duration of seconds only. Use structural damping of g = 0.06 and convert this damping to equivalent viscous damping at 250 Hz. Carry the analysis for 0.04 seconds.

WS3-4 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation DIRECT TRANSIENT RESPONSE n Problem Description (cont.) u Below is a finite element representation of the flat plate. It also contains the loads and boundary constraints.

WS3-5 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation DIRECT TRANSIENT RESPONSE n Suggested Exercise Steps 1. Import the model from Workshop 1a. 2. Create a non-spatial field for the pressure load and the force load. 3. Create a time dependent load case. 4. Create the time dependent force load. 5. Create the time dependent pressure load. 6. Submit the model to MSC.Nastran for analysis. 7. Attach the.XDB results file. 8. Post Process results – create X vs Y graph of displacements.

WS3-6 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation CREATE NEW DATABASE Create a new database called ws3.db. a.File / New. b.Enter ws3 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

WS3-7 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 1. File / Import Import the model from Workshop 1a. a.File / Import. b.Select MSC.Patran DB as the Source. c.Select ws1a.db. d.Click Apply. e.Click OK when the Patran Database Import Summary appears. a b c d

WS3-8 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 2. Field: Create / Non Spatial / Tabular Input Create a Non Spatial field for the pressure load. a.Fields: Create / Non Spatial / Tabular Input. b.Enter pressure for the Field Name. c.Select Time (t) as the Active Independent Variable. d.Click Input Data. e.Click Map Function to Table. f.Type in the function, sind(250*360*t) and the values shown. g.Click Apply. h.Click OK on the table. i.Click Apply. a b c d e f g h i Note the PCL Syntax: Sind – Sine function in degrees t – time is a Patran global variable

WS3-9 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 2. Field: Create / Non Spatial / Tabular Input (Cont.) Create a Non Spatial field for the force load. a.Enter force for the Field Name. b.Select Time (t) as the Active Independent Variable. c.Click Input Data. d.Click Map Function to Table. e.Type in the function, -sind(250*360*t) and the values shown. f.Click Apply. g.Click OK on the table. h.Click Apply. a b c d e f g h

WS3-10 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 3. Load Cases: Create Create a Time Dependent load case. a.Load Cases: Create. b.Enter direct_transient for the Load Case Name. c.Select Time Dependent as the Load Case Type. d.Click Assign/Prioritize Loads/ BCs. e.Click on the Displ_constraint in the Select Individual Loads/BCS field. f.Click OK. g.Click Apply. a b c d e f g

WS3-11 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 4. Loads/BCs: Create / Force / Nodal Create the time dependent Force load. a.Loads/BCs: Create / Force / Nodal. b.Enter 50lb for the New Set Name. c.Click on the Input Data button. d.Enter for Force, and select Force for the Time/Freq. Dependent Field. e.Click OK. f.Click on Select Application Region. g.Change the Geometry Filter to FEM. h.Select the bottom right corner node for the application region. i.Click Add, and click OK. j.Click Apply. a b c d e f g h i j i

WS3-12 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 5. Loads/BCs: Create / Pressure / Element Uniform Create the time dependent Pressure load. a.Loads/BCs: Create / Pressure / Element Uniform. b.Enter pressure for the New Set Name. c.Change the Target Element Type to 2D. d.Click on the Input Data button. e.Enter -1 for Top Surf Pressure, and select Pressure for the Time/Freq. Dependent Field. f.Click OK. g.Click on Select Application Region. h.Select all the elements for the application region. i.Click Add, and click OK. j.Click Apply. a b c d e f g h i j i

WS3-13 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Analysis: Analyze / Entire Model / Full Run Submit the model for analysis. a.Analysis: Analyze / Entire Model / Full Run. b.Click on Solution Type. c.Select Transient Response. d.Change the Formulation to Direct. e.Click on Solution Parameter. f.Enter for Wt- Mass Conversion. g.Enter 0.06 for Struct. Damping Coefficient and 1570 for W3, Damping Factor. h.Click OK. i.Click OK. a b c d e f g h i

WS3-14 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Click on Subcases. b.Select direct_transient from the Available Subcases field. c.Click on Subcase Parameters. d.Click on DEFINE TIME STEPS button. e.Change Delta-T to Click Enter. f.Click OK. g.Click OK. h.Click Apply. i.Click Cancel. a c b d e f g h i

WS3-15 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Analysis: Analyze / Entire Model / Full Run (Cont.) Submit the model for analysis (cont.). a.Click on Subcase Select. b.Select direct_transient and unselect Default. c.Click OK. d.Click Apply. a b c d

WS3-16 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 7. 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 ws3.xdb. d.Click OK. e.Click Apply. a b c d e

WS3-17 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 8. Results: Create / Graph / Y vs X Create a X-Y graph of displacement results. a.Results: Create / Graph / Y vs X. b.Click on SC1:DIRECT_TRANSIENT. c.Select Global Variable as the Filter Method. d.Click Filter. e.Click Apply. f.Click Close. a b c d e f

WS3-18 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 8. Results: Create / Graph / Y vs X (Cont.) Create a X-Y graph of displacement results (cont.). a.Select Displacement, Translational for the Select Y Result field. b.Select Z Component as the Quantity. c.Click on the Target Entities icon. d.Change the Target Entity Selection to Nodes. e.Select the upper right node (node opposite where force is applied). f.Click Apply. b a c d e f

WS3-19 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation Step 8. Results: Create / Graph / Y vs X (Cont.)

WS3-20 NAS122, Workshop 3, August 2005 Copyright 2005 MSC.Software Corporation