MUG ANALYSIS
MSC visualNastran Tutorial
Clarkson University
Andy StrongMUG ANALYSIS
MSC visualNastran 4D tutorial
Part One: Opposing Force Stress Analysis
1) Open visualNastran 4D (vN4D).
From the Start Menu Select: All Programs, MSC.visualNastran Desktop, MSC.visualNastran 4D.
Figure 1: MSC visualNastran 4D icons
2) Import mug model (mug.stp).
From the File menu select open and brose to the location of mug.stp. From the Specify length unit pull down menu, select in. Click Open.
Figure 2: Open window
3) Verify the model.
Right click on the mug model and choose Properties from the pull down menu. Select the Geometry tab. Verify that the model Width, Length and Height are 4.84in, 3.25in, and 4.5in respectively.
Figure 3: Properties window
4) Set the units.
From the World menu choose Display Settings. Open the Display Settings tab if it is not and select Units. From the Unit System pull down menu, select English(slugs).
Figure 4: Display Settings window
5) Add an FEA mesh to the model.
Right click the model and choose Properties from the pull down menu. Select the FEA tab and check the Include in FEA checkbox. Click the mesh button, wait for the mesh solver, and check the Show mesh checkbox.
Figure 5: Properties, FEA window
Your model should look something like figure 6.
Figure 6: Model with mesh applied
This is a poor mesh representing this model, so we will change the FEA properties. In the FEA tab change Default mesh size to 0.125 and click Apply. Click Mesh and wait for the mesh solver to finish. Your model should now look like Figure 7. Obtain a printout of this. Uncheck the Show mesh checkbox and close the properties window.
Figure 7: Model with updated mesh
5) Set the model material.
Right click the model and select Properties from the pull down menu and select the Materials tab. Under Material Properties click Change. From the Material pull down menu select Glass and click OK. Close the properties window.
6) Apply forces to the model.
From the Insert menu select Force (or select the force icon ). Click on the model near the top (see figure 8) to apply a force. Rotate the model (middle mouse button or F4) and apply a second force (select Insert, Force, and click).
Figure 8: Forces applied on either side of model
Rotate (middle mouse button or F4) the model so you can see both forces:
Figure 9: Position of left and right forces
Right click on the green arrow representing the left force and choose Properties from the pull down menu. Under the Appearance tab change the Name to Left Force. Under the Structural Load tab change X, Y, and Z to 0, 100, and 0 respectively.
Figure 10: Force properties window
Repeat this for the right force, but give it the name Right Force and use 0,-100, and 0 for the X, Y, and Z components.
7) Position the forces.
In the left multi-menu select Object Browser. Click the + box on Left Force and Right Force to expand them.
Figure 11: Location of Object Browser
Right click on the red coord under the Left Force expansion and choose Properties from the pull down menu. Under the Position tab (Pos) set X, Y, Z, Rx, Ry, and Rz to 0, -1.63, 4, 90, 0, and -180 respectively. Repeat this for the Right Force coord and set X, Y, Z, Rx, Ry, and Rz to 0, -1.63, 4, 90, 0, and 0 respectively. The forces should now be centered and directly opposing each other as in figure 12.
Figure 12: Coord properties window
8) Run Stress Finite Element Analysis.
To run the FEA solver, click the Solve FEA button (be sure it is set to stress analysis by selecting the small carrot button to the right of the Solve FEA). This will generate a single frame FEA solution and map it in color to the model. In order to display the proper stress values, go to the World pull-down, then select Display Settings, FEA Display, and Contour Data. On the right side of the window select Stress and then change from von Mises to MAX_PRINCIPAL.
Figure 13: Location of Solve FEA button
Figure 14: FEA Stress solution
Save your analysis as MUG1.WM3. Be careful not to over-write this file in the next two sections. Obtain a printout of these results.
Part Two: Applied Thermal Analysis
Open MUG1.WM3 and Save As MUG2.WM3.
Delete the two blue cords (red in Object Browser) by clicking on them and press Delete (Answer Yes when asked if you want to erase the FEA results). The two green force arrows should delete with them automatically.
The thermal analysis is more processor intensive (in its current state) so we will use a larger mesh on the model. Right click on the model; choose Properties from the pull down menu. Under the FEA tab, change Default Mesh Size to 0.25, press apply and then Mesh. Close the Properties window.
1) Add the Thermal Toolbar
From the World menu choose Display Settings. Expand the Preferences + box and select Toolbars. Check the Thermal check box (if it’s unchecked) and press apply and close. The thermal toolbar should appear in the upper window.
Figure 15: Thermal Toolbar
2) Add a Prescribed Temperature.
Double click on the Prescribed Temperature button and click on the inner surfaces of the mug (inside edge, bottom, and fillet between them).
*note: Double-clicking a constraint puts the constraint selection into "sticky mode" for continuous selection of multiple surfaces. Press escape to turn sticky mode off.
Figure 16: Mug with temperature applied to inside surfaces
In the Object Browser, right click on each of the prescribed temperature constraints and select Properties. Select the Temperature tab and change the Prescribed Temperature to 200ºF for each constraint.
Figure 17: Object Browser
3) Add a Convective Heat Flux.
Double click on the Convective Heat Flux button and click on the outer surfaces of the mug (outside shell, bottom, handle and fillets between them). Press escape to exit sticky mode.
Figure 18: Mug with temperature and convection constraints applied
4) Run the Thermal FEA Solver
Click the small carrot button next to the Solve FEA button and select Thermal from the pull down menu.
Figure 19: Changing analysis type
Click the Solve Thermal FEA button. This will generate a single Thermal FEA frame solution and map it in color to the model.
Figure 20: FEA Thermal Solution
Here we can see that this mug filled with a liquid at 200ºF will be about 100ºF on the outside of the mug and about 85ºF on its handle.
Save your analysis as MUG2.WM3. Be careful not to over-right this file in the next two sections. Obtain a printout of these results.
Part Three: Applied Thermal Stress Analysis
Open MUG2.WM3 and Save As MUG3.WM3.
Part Two gave us an example of the heat flow through the mug when a temperature is applied to the inside of the mug and convection into air occurs on the outside of the mug. In the next part, we will apply a temperature to the entire mug and look at the internal stress.
1) Adjust applied temperatures
Press Control-F to delete the current FEA results. In the Object Browser select all of the temperature constants (,) and delete them.
2) Set up temperature stress analysis
Highlight the mug by clicking on it. In the lower left corner of vN4D, there is a properties checkbox listing. Scroll through this menu, find Heat, and check its checkbox. When you do this, the Properties window for the mug should automatically pop up with the Heat tab selected.
Figure 21: Heat Properties
Under Temperature-Induced Stress check the Use the body temperature in a stress analysis checkbox. Enter a value of 200 degrees for current temperature, and 77 degrees for Stress-free temperature. Close the properties window.
...
raga76