Workshop 1-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 1 Pin-joint Truss Subjected to Point Loads. - презентация

1 Workshop 1-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 1 Pin-joint Truss Subjected to Point Loads

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

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

4 Workshop 1-4 NAS101 Workshops Copyright 2001 MSC.Software Corporation Problem Description: a.Connected by pin joints b.Simply supported at left end, roller at right end c.Treat it as two dimensional structure d.Wood material A = 5.25 in 2 E = 1.76E6 psi =.3 tension allowable =1900 psi compression allowable = 1900 psi e.Apply point loads at grid points 2,4, and 6 as shown in Figure 1-1

5 Workshop 1-5 NAS101 Workshops Copyright 2001 MSC.Software Corporation n Suggested Exercise Steps: 1. Create a finite element model of the truss members. Create a finite element mesh. (GRID and CROD) 2. Define material properties. (MAT1) 3. Define element properties and apply them to the model. (PROD) 4. Apply loads and boundary conditions to the model. 5. Submit the model to MSC.Nastran for analysis. 6. Post-Process results using MSC.Patran.

6 Workshop 1-6 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create all the nodes for this model a.Create / Node / Edit. b.Input [0 0 0] for this first node c.Click Apply. Step 1. Finite Element: Create /Node /Edit

7 Workshop 1-7 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 1A: Repeat previous steps to create all the following nodes: NODELocation:[ ] 2144,72,0 3192,0, , 144, , 0, , 72,0 7576, 0, 0

8 Workshop 1-8 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 1B: Turn On the label on the screen Show Label

9 Workshop 1-9 NAS101 Workshops Copyright 2001 MSC.Software Corporation a.Create element edit b.Change the shape to Bar c.Click inside the Node 1 box and place your cursor on the screen and Select node 1 and node 2 to create the first element Step 2 (cont). Finite Element: Create /Element /Edit

10 Workshop 1-10 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 2A: Add more rod elements: from element 2 to 4

11 Workshop 1-11 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 2B: Add more rod elements: from element 5 to 8

12 Workshop 1-12 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 2C: Add more rod elements: from element 9 to 11

13 Workshop 1-13 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3. Material: Create /Isotropic/ Manual Input Create the material aluminum. a.Create / Isotropic / Manual Input. b.Type in mat for the Material Name. c.Click on the Input Properties button to bring up the Input Option window. d.Enter 1.76E6 for the Elastic Modulus and 0.3 for Poisson Ratio. e.Click OK to return to the main material menu. f.Click Apply. d c

14 Workshop 1-14 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3A. Material: Create /Isotropic/ Manual Input/Failure Create the failure limit. a.Click on the Input 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.

15 Workshop 1-15 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4. Element Properties: Create /1D/ Rod Create the element properties. a.Create / 1D / Rod. b.Enter rod as the Property Set Name. c.Click on the Input Properties button. d.Click on the mat in the Material field on the bottom section of the Input Properties window. e.Enter 5.25 as the cross sectional area. f.Click OK. g.Select element 1:11 for the Application Region.(pick the 1D element icon) h.Click Add. i.Click Apply.

16 Workshop 1-16 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter clamp as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 1 for the Application Region. i.Click Add. j.Click OK. k.Click Apply.

17 Workshop 1-17 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5A. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter dof456 as the New Set Name. c.Click on the Input Data. d.Enter for the Rotations field. e.Click OK. f.Click on Select Application Region. 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.

18 Workshop 1-18 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5B. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter rightside as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 7 for the Application Region. i.Click Add. j.Click OK. k.Click Apply.

19 Workshop 1-19 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5C.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

20 Workshop 1-20 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6. Loads/BCs: Create/Force /Nodal Apply distributed load to the model. a.Create / Force / Nodal b.Enter horizontal as the New Set Name. c.Click on the Input Data button. d.Enter in the Force field. e.Click OK. f.Click on Select Application Region button. g.Select FEM as the Geometry Filter. h.Select Node 2,4,6 for the Application Region. i.Click Add, and OK. j.Click Apply.

21 Workshop 1-21 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6A. Loads/BCs: Create/Force /Nodal Apply distributed load to the model. a.Create / Force / Nodal b.Enter vertical as the New Set Name. c.Click on the Input Data button. d.Enter in the Force field. e.Click OK. f.Click on Select Application Region button. g.Select FEM as the Geometry Filter. h.Select Node 2,4,6 for the Application Region. i.Click Add, and OK. j.Click Apply.

22 Workshop 1-22 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6(cont.) Loads/BCs: Create Distributed Load You can see the combine load value of 1985 on the screen. This load is equal to p= (1500**2+1300*2)

23 Workshop 1-23 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 7. 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 1-24 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8. 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 w1. xdb d.Click OK. e.Click Apply.

25 Workshop 1-25 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8 (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 5.13E-1. These information appear at the lower right hand corner of the plot.