Workshop 2-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 2 Roof Truss Subjected to Point Loads (Top and bottom members welded,cross. - презентация

1 Workshop 2-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 2 Roof Truss Subjected to Point Loads (Top and bottom members welded,cross braces are connected by pin joints)

2 Workshop 2-2 NAS101 Workshops Copyright 2001 MSC.Software Corporation Roof Truss Subjected to Point Loads (cont.)

3 Workshop 2-3 NAS101 Workshops Copyright 2001 MSC.Software Corporation Roof Truss Subjected to Point Loads (cont.) Figure 1-1

4 Workshop 2-4 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop # 2 (cont.) 1. Model description a.Simply supported at left end, roller at right end. b.Treat it as two dimensional structure. c.Apply point loads at grid points 2,4, and 6 as shown in Figure 2-1. d.Top (1,2,3,4) and bottom (9,10,11) are steel members and are welded together. e.Cross braces are made of wood and are connected with pin joints. f.See Table 2-1 for element properties. g.See Table 2-2 for material properties. h.See Table 2-3 for cross-sectional properties.

5 Workshop 2-5 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop # 2 (cont.)

6 Workshop 2-6 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop # 2 (cont.)

7 Workshop 2-7 NAS101 Workshops Copyright 2001 MSC.Software Corporation n Suggested Exercise Steps: 1. Copy previous PATRAN workshop db file:w1. db to another name called w2. db 2. Open the PATRAN database and bring in the w2. db 3. Create new material properties for steel and for pine 4. Create properties for BAR elements. 5. Create sectional properties using beam library 6. Redefine the elements of 1,2,3,4 and 9,10,11 as the bar elements. 7. Apply loads and boundary conditions to the model. 8. Submit the model to MSC.Nastran for analysis. 9. Post-Process results using MSC.Patran.

8 Workshop 2-8 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 1. Material: Create /Isotropic/ Manual Input Create the material pine. a.Create / Isotropic / Manual Input. b.Type in pine for the Material Name. c.Click on the Input Properties button to bring up the Input Option window.(see table2-2) d.Enter 1.76E6 for the Elastic Modulus,and put in value for density, thermal coefficient of expansion,and referenced temperature. e.Click OK to return to the main material menu. f.Click Apply.

9 Workshop 2-9 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 1A. Material: Create /Isotropic/ Manual Input/Failure Create the failure limit. a.Click on the Input Properties again b.Click on the Constitutive Model changed to Failure button to bring up the Input Option window. c.Enter 1900 for the Tension Stress limit d.Enter 1900 for the compression stress limit e.Click OK to return to the main material menu. f.Click Apply.

10 Workshop 2-10 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 1B. Material: Create /Isotropic/ Manual Input Create the material steel. a.Create / Isotropic / Manual Input. b.Type in steel for the Material Name. c.Click on the Input Properties button to bring up the Input Option window.(see table2-2) d.Enter 2.90E7 for the Elastic Modulus,and 0.32 for Poisson ratio. Also put in values for density, thermal coefficient of expansion,and referenced temperature. e.Click OK to return to the main material menu. f.Click Apply.

11 Workshop 2-11 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 1C. Material: Create /Isotropic/ Manual Input/Failure Create the failure limit. a.Click on the Input Properties again b.Click on the Constitutive Model changed to Failure button to bring up the Input Option window. c.Enter for the Tension Stress limit d.Enter for the compression stress limit e.Enter for the shear stress limit f.Click OK to return to the main material menu. g.Click Apply.

12 Workshop 2-12 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2. Element Properties: Create /1D/ Beam Create the element properties. a.Create / 1D / Beam. b.Enter steel_a as the Property Set Name. c.Click on the Input Properties button. d.Click on the steel in the Material field on the bottom section of the Input Properties window. e. Put the cursor in the [Section Name] and click on the Beam Library,the window pop up is shown on next page

13 Workshop 2-13 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2A. Beam library: Create /Standard Shape/NASTRAN standard Create the beam cross sectional using IBEAM. a.Enter section_a as the Section Set Name. b.Click on Ibeam button. c.Input H,W1,W2,t,t1,t2 as d.8,3,3,0.5,0.5,0.5 e.Click on Calculate/Display, then you will see the following section diagram on the next page f.Click OK

14 Workshop 2-14 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 2B: Display the Beam cross sectional area

15 Workshop 2-15 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2C. Element Properties: Create /1D/ Beam Once the section is created,you can go back to the previous menu. a.Once you have created section_a, then you can select the Bar Orientation as,click OK b.Click inside the box Select Members,and pick element 9:11 c.Click Add and APPLY to close the form You will see a warning message regarding overwriting the properties for element 9,select YES for ALL button

16 Workshop 2-16 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3. Element Properties: Create /1D/ Beam Create the element properties. a.Create / 1D / Beam. b.Enter steel_b as the Property Set Name. c.Click on the Input Properties button. d.Click on the steel in the Material field on the bottom section of the Input Properties window. e. Put the cursor in the [Section Name] and click on the Beam Library,the window pop up is shown on next page

17 Workshop 2-17 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3A. Beam library: Create /Standard Shape/NASTRAN standard Create the beam cross sectional using IBEAM. a.Enter section_b as the Section Set Name. b.Click on Ibeam button. c.Input H,W1,W2,t,t1,t2 as d.6,3,3,0.5,0.5,0.5 e.Click on Calculate/Display, then you will see the following section diagram on the next page f.Click OK

18 Workshop 2-18 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 3B: Display the Beam cross sectional area

19 Workshop 2-19 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3C. Element Properties: Create /1D/ Beam Create the element properties. a.Once you have created section_b, then you can select the Bar Orientation as,click OK b.Click inside the box Select Members,and pick element 9:11 c.Click Add and APPLY to close the form You will see a warning message regarding overwriting the properties for element 1,select YES for ALL button

20 Workshop 2-20 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3D. Element Properties: Modify /1D/ Rod Modify-1D-Rod a.Click on rod b.Click on Modify Properties button, and select Material pine c.Click OK,and APPLY

21 Workshop 2-21 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4A. Loads/BCs: Modify/ Displacement/Nodal Modified the boundary condition for the model. a.Modified / Displacement / Nodal. b.Click on dof456 c.Click on the Modify Data. d.Enter for the Rotations field. e.Click OK. f.Click on Modify Application Region button. g.Select FEM as the geometry filter.. h.Select Node 1:7 (all the nodes) for the Application Region. i.Click Add. j.Click OK. k.Click Apply. Because we have bar elements in this model, and therefore we have to allow the bending in this model by removing rotation in Z from previous pin model.

22 Workshop 2-22 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4B.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

23 Workshop 2-23 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5. Analysis: Analyze/ Entire Model/Full Run Submit the model for analysis. a.Analyze / Entire Model / Full Run. b.Click on the Solution Type. c.Select LINEAR STATIC as the Solution Type. d.Click OK. e.Click Apply.

24 Workshop 2-24 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6. Analysis: Attach XDB/ Result Entities/ Local Attach the XDB result file. a.Attach XDB / Result Entities / Local. b.Click on Select Result File. c.Select the file called w2. xdb d.Click OK. e.Click Apply.

25 Workshop 2-25 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 7 (cont.) Results: Create/Quick Plot Create a Quick Plot of the results. a.Create / Quick Plot. b.Select SC1 result case. c.Select Displacement, Translational for the Deformation Result. d.Click Apply. Note: Maximum Deformation is 7.06E-2. These information appear at the lower right hand corner of the plot.