3-Member Truss
Step 1 - Create a new Patran database.
1) Click on New from the File menu or from the Defaults Toolbar as shown.
2) Type the name of the new database as 3_Member_Truss and click OK.
3) In the Approximate Maximum Model Dimensions box, input 10.0. Click OK.
Step 2 - Create the geometry of the 3-member truss using the information from the problem statement.
1) Under the Geometry tab, click on Points and select XYZ.
2) Input the following point coordinates and click Apply after each point: [0 0 0], [0 10 0], and [-10 0 0]. There are no units in Patran, and therefore it is important to stay consistent in units.
3) Under the Geometry tab, click on Curves and select Point.
4) With Auto Execute checked, click on Point 1 then Point 2, Point 1 then Point 3, and Point 2 then Point 3.
Step 3 - Create the isotropic material: Elastic Modulus = 30E6
1) Under the Properties tab, select Isotropic.
2) Input steel as the Material Name and then select Input Properties .
3) Input 345 as the Thermal Conductivity. Click OK and Apply.
Step 4- Create a 1D Rod physical property and apply the isotropic material to the model.
1) Click on Rod under the 1D Properties section.
2) Input Truss as the Property Set Name and then click on Input Properties .
3) Click on Select Material and select steel. Enter 3.14 as the Area. Click OK.
4) Click on Select Application Region and then click on the Select Members box. Screen pick the curves. Click Add, OK then Apply.
Step 5 - Create boundary conditions: Apply the Displacement Constraint.
1) Under the Load/BCs tab, select Displacement Constraint.
2) Input New Set Name as the ClampAB, and click on Input Data. .
3) Enter Translations as <0,0,0> and Rotation as <0,0, > . Click OK.
4) Click on Select Application Region click on the Select Geometry Entries box. In the selection toolbar, select Node. Screen select the bottom nodes. Click Add, OK then Apply.
5) Repeat this process to create ClampC that contrains rotation in the x and y-direction on node C but does not contrain translation (the Translation box should be < , , >).
Step 6 - Apply the forces shown in the problem statement.
1) Click on Force. Enter New Set Name as Force and click on Input Data.
2) Enter <100,-200,0> as the Force and click OK.
3) Click on Select Application Region
4) Now,Click on the Select Geometry Entries box. In the selection toolbar, select Node. Screen select the Node as shown. Click Add, OK then Apply.
Step 7 - Create a finite element mesh with a Global Edge Length of 10.
1) Under the Meshing tab, click on Object as Mesh and Type curve.
2)Set the Topology to BAR2. Click on the Curve List box and screen select the all curve. Set the Global Edge Length to 10. Click on Apply.
3) Set Action to Equivalence and click Apply (This will eliminate duplicate nodes at the intersection of two curves).
Step 8 - Run a steady state analysis using MD Nastran.
1) Under the Analysis tab, select Entire Model. Ensure that the Job Name box is filled with a name and click Apply.
Step 9 - Attach results file, then create fringe plot. Record the displacement and stress induced in the truss.
1) Click on XDB under the Access Results submenu. .
2) Ensure the appropriate Job Name is selected and click Apply.
3)Under the Results tab, select Fringe/Deformation.
4) Plot Displacement, Translational. Set Quantity to X Component. Click Apply. Repeat for Y Component.
Analytical Solution - Verify the results by calculating the analytical solution.
Substitute: P=100 lb, L=1 in, E=30e6 psi, A=3.14 in2 in the above equation.
Results: U3 = 6.183 X 10-5 inches V3 = -3.185 X 10-5 inches MD Nastran results for U3 = 6.187298E-05 inches MD Nastran results for V3 = -3.184716E-05 inches
(You can open the '3_Member_Truss.f06' file with Notepad to view your results)
