Compression on a Two Column Structure
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 two_columns and click OK.
Step 2 - Create the geometry of the columns using the information from the problem statement.
1) Under the Geometry tab, click on Point and select XYZ.
2)Input the following point coordinates and click Apply after each point: [0 0 0], [0 10 0], and [0 -10 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, and Point 1 then Point 3.
Step 3 - Create the isotropic material: elastic modulus of 10×106.
1) Under the Properties tab, select Isotropic.
2) Input Material as the Material Name and then select Input Properties .
3) Input 10×106 as the Elastic Modulus. Click OK and Apply.
Step 4- Create a 1D surface physical property and apply the isotropic material to the model.
1) Click on Rod under the 1D Properties section.
2) Input Top_Column as the Property Set Name and then click on Input Properties.
3)Click on Select Material and select Material. Enter 1.5 as the Area. Click OK.
4) Click on Select Application Region and then click on the Select Members box. Screen pick the top curve. Click Add, OK then Apply.
5) Repeat the above steps for the bottom curve except input Bottom_Column as the Property Set Name and enter 2 as the area.
Step 5 - Create boundary conditions: Constrain all degrees of freedom along the bottom of the structure.
1) Under the Load/BCs tab, select Displacement Constraint.
2) Input fixed_end as the New Set Name and then click on Input Data.
3) Input <0,0,0> for Translations (to prevent any translational movement), but leave the Rotations blank, < > (to NOT prevent any rotational movement). Click OK.
4) Click on Select Application Region and then click on the Select Geometry Entries box. Screen select Click Point 3. Click Add, OK then Apply.
Step 6 - Create the load of 10000 lb to the top of the structure.
1) Click on Force under the Nodal section.
2) Input top_load and click on Input Data.
3) Input <0,-10000,0> as the Force. Click OK.
4) Click on Select Application Region and then click on the Select Geometry Entries box. Screen select Point 2. Click Add, OK, then Apply.
Step 7 - Create a mesh seed and a finite element curve mesh.
1) Under the Meshing tab, click on Uniform Mesh Seeds.
2)Set the Number of Elements to 1, and with Auto Execute checked, select each curve.
3) Under the Meshing tab, click on Curve Meshers.
4) Click on the Select Curve List box. Screen click both curves using the Shift key. Click Apply.
5) Set Action to Equivalence and click Apply (This will eliminate duplicate nodes at the intersection of the two curves).
Step 8 - Run a steady state analysis using MSC 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 and deformation plots. Record maximum displacement and stresses.
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 Displacements, Translational and Displacements, Translational. Click Apply.
Analytical Solution - Verify the results by calculating the analytical solution.
1) Results:
From the equation below: u2 = -0.005 inches From the equation below: u3 = -0.01167 inches
MD Nastran results: u2 = -0.005 inches MD Nastran results: u3 = -0.01167 inches
(You can open the 'two_columns.f06' file with Notepad to view your results)
The answers are identical.
