Nei Nastran Tutorials

Problem Four: Static Analysis of a Midsurface Model

4.


4.1 Introduction In this example, you will learn to work with Femap's automatic midsurface extraction capabilities to build an idealized model of an electrical box. To work through this example, you must have a licensed copy of NEi Nastran. You will not be able to complete this example with the 300-node demo version.

The example includes the following steps: importing the geometry using the STEP interface, creating the midsurface model, meshing the model, applying loads and constraints, analyzing the model using the NEi Nastran Editor, and post-processing the results.

4.2 Pre-Process the Model To begin, you will first import the geometry and then create a midsurface model. You will then mesh the model followed by applying the necessary loads and constraints. The model will then be ready for analysis and post-processing.

NEi Nastran Version 10.1

Tutorial 4-1


4.2.1 Import the Geometry To begin the example, you will import the geometry. From the Femap Main Menu, select File, then Import, and then Femap Neutral. Go to the C:\Program Files\NEi Nastran Engine V101\Example Files\Tutorial Problems\Example Problem 4 folder and import Example Problem 4.STP In the STEP Read Options dialog box, click OK. Press the F8 key to open the View Rotate dialog box. In the View Rotate dialog box click Dimetric and then OK. In the View Style Menu (on View Toolbar), choose Wireframe

.

4.2.2 Create the Midsurface Model You will now create the midsurface model and delete the original solid. Once the midsurface has been generated, you will need to do some additional cleanup work on the geometry before you can mesh it. To create the midsurface, use the automatic midsurface capability.


Tutorial 4-2


Zoom and rotate the part to get a better view of the points you will be picking to designate the “Target Distance” for midsurfacing.

Now, from the Femap Main Menu, choose Geometry, then Midsurface, and then Automatic. In the Select Entities – Select Surfaces to Mid-Surface dialog box, click Select All and then OK. This opens the Mid-Surface Tolerance dialog box. Move the cursor to the Graphics window and then press Ctrl+D. The Ctrl+D command lets you determine the distance for the target thickness. The software uses this value to determine which surfaces to use to place a midsurface between. The target thickness should be slightly larger than the largest distance between the planes on the solids that you want to midsurface. If the target thickness is too low, the midsurfaces will not be created. If the target thickness is too high, some midsurfaces will be created between the wrong surfaces. Once you press Ctrl+D, a Locate – Define Location to Measure From dialog box appears. In this dialog box, click on the Methods button and choose On Point.


Tutorial 4-3


This opens the On Point – Define Location to Measure From dialog box. Now click on point A as shown in the figure below and click OK.

Now pick point B and click OK again. The Mid-Surface Tolerance dialog box appears again with the Target Thickness value of approximately 4.92, now click OK.


Tutorial 4-4


4.2.3 Delete the Solid You will now delete the original solid. Go to Delete in the Femap Main Menu and select Geometry, and then Solid. In the Entity Selection – Select Surface(s) to Delete dialog box, type 1 into the ID field and then click OK, and then OK again to confirm the delete. From the View Style Menu (on the View Toolbar), choose solid look like the one below.


. Your model should now

Tutorial 4-5


4.2.4 Cleanup the Geometry To create a more accurate model, you must trim each rib, and then delete the top portion. Start by trimming all of the ribs. Go to Geometry in the Femap Main Menu, then Midsurface, and then Trim with Curve. This opens the Select Surfaces/Solid to Trim dialog box. Here, pick one of the eight ribs (see C in the figure below) and then click OK.


Tutorial 4-6


The Entity Selection – Select Line(s) to Trim With dialog box opens and you want to pick the curve on the lower portion as shown in the above figure. After you select that curve, click OK, and repeat this process for the remaining seven ribs. The curve now cuts through the surface.

Now that the ribs are all separated, you will delete the top portion of each rib. Go to Delete (in the Femap Main Menu), then Geometry, and then Surface. This opens the Entity Selection – Select Surface(s) to Delete dialog box. Now choose the top half of the ribs (see D in the figure below), then click OK, and OK again to confirm the delete.


Tutorial 4-7


The top half of the ribs has been deleted and should look like the figure below.

You have to intersect the ribs with the walls of the electric box to make this one solid. To do this, go to Geometry (in the Femap Main Menu), then choose Midsurface, and then Intersect.


Tutorial 4-8


In the Entity Selection – Select Surfaces/Solids to Automatically Intersect dialog box, click the Select All button and then OK. You are now ready to mesh your model.

4.2.5 Mesh the Model The first step in meshing the model is to assign mesh attributes for the different surfaces. If the correct attributes are not assigned, the results will not be correct. Next, set the size for the mesh, and then finally, mesh the midsurface. Begin by assigning the mesh attribute to the surfaces. Go to Geometry (in the Femap Main Menu), then choose Midsurface, and then Assign Mesh Attributes. In the Entity Selection – Select Surfaces to Assign Attributes dialog box, click the Select All button and then OK. This will bring up the Define Material – ISOTROPIC dialog box, click on Load, then pick AISI 4340 Steel and then click OK in all of the dialog boxes. When asked to Consolidate Properties by Thickness select Yes, and click OK to use the default Plate Thickness Tolerance. If midsurfaces are created manually using commands such as Geometry, Surface Offset or Geometry, Surface, Extrude, the surfaces do not have mesh attributes. You must manually assign mesh attributes by creating or assigning existing properties using the correct thickness. Now set the mesh size to the default value and mesh the model. Go to Mesh (in the Femap Main Menu), then choose Mesh Control, and then Size on Surface. This opens the Entity Selection – Select Surface(s) to Set Mesh Size. Click the Select All button, then OK twice (you will use the default mesh size), and then Cancel when it prompts you to select more surfaces. Again, go to Mesh, this time choose Geometry, and then Surface. This opens the Entity Selection – Select Surfaces to Mesh. Click the Select All button and then OK. In the Automesh Surfaces dialog box click OK.


Tutorial 4-9


Your meshed model should now look like the figure below once you have turned off the geometry and nodes (in the View Options – press Ctrl+Q):


Tutorial 4-10


4.2.6 Apply the Constraints You will now set up the constraints on the holes at the bottom of the part. Go to Model (in the Femap Main Menu), then Constraint, and then On Curve. In the New Constraint Set dialog box, give the set a Title such as Pinned and click OK. The Entity Selection – Enter Curve(s) to Select dialog box appears and you need to select all eight curves that make up the four bottom holes in the electrical box. Once you have picked all eight, click OK. You may want to rotate the model and zoom in on the corners of the model to make selection of these curves easier. While in a command you can use the middle mouse button to rotate the model as well as the Zoom and Previous Zoom icon on the View Toolbar. In the Create Constraints on Geometry dialog box, click the Pinned – No Translation radio button and then OK. When Femap prompts you to select more curves for constraints, click Cancel.

To see the nodes on which the loads and constraints are applied, use the Model, Load, Expand and Model, Constraint, Expand commands.

4.2.7 Apply the Load To load the model, you will apply a pressure to the surface at the back of the electrical box. Start by going to Model from the Femap Main Menu and choose Load, and then On Surface. In the New Load Set dialog box, create a Title for your load such as Pressure and click OK. In the Entity Selection – Enter Surface(s) to Select dialog box enter 129 in the ID field and click OK. Surface 129 is the middle surface at the back of the part.


Tutorial 4-11


In the Create Loads on Surfaces dialog box, select Pressure as the type of load and set the value to -1. Your dialog box should look as the one above. Once this is set, click OK. Click Cancel when it prompts you to create another load. Your model should look like the model below.


Tutorial 4-12


4.3 Run the Analysis Before you solve the model using the NEi Nastran Editor, you must create the analysis set. Go to Model from the Femap Main Menu and select Analysis. Click on New to create a new analysis set. For the Analysis Program, choose 31..NEi Nastran and for Analysis Type, choose 1..Static.

Click OK, and then Analyze. Give it a file name Example Problem 4 and then click Write to begin the analysis.

4.4 Post-Process the Results For this analysis, you will display deformation and stress contours. Push the F5 key to open the View Select dialog box. Click the Deform radio button in the Deformed Style field, and the Contour radio button in the Contour Style field. Now click on the Deformed and Contour Data button. In the Select PostProcessing Data dialog box under the Output Vectors field change the Deformation to 1..TOTAL TRANSLATION and the Contour to 7026..SHELL MAJOR PRINCIPAL TOP and then click OK in all of the dialog boxes.


Tutorial 4-13


Rotate the model so you can see the back.


Tutorial 4-14


Notice how you can see the plate top stress contour on both faces of the plate elements. Now change the contour options to display double-sided planar contours. If you select a standard top or bottom plate vector for contouring, as you did above, Femap can automatically contour both top and bottom stresses on the same point. Press the F5 key to open the View Select dialog box. Click on the Deformed and Contour Data button, and in the Select PostProcessing Data dialog box, click the Contour Options button. In the Select Contour Options dialog box, click the Elemental radio button in the Contour Type field and click the Average radio button in the Data Conversion field as well as check the Use Corner Data. In the Other Options field, check the Double-Sided Planar Contours.

Click OK in all dialog boxes. Notice that the display has changed. The contour now shows plate top major principal stress on the top face of the plate elements and plate bottom major principle stress on the bottom face of the plate elements.


Tutorial 4-15


Rotate the model to look at the back.

Notice how the contour on the back of the part shows plate top major stress.


Tutorial 4-16


To more easily see double-sided results, change the view to show the element thickness. To do this, press the F6 key to open the View Options dialog box. In this dialog box, click Element – Orientation/Shape in the Options field. In the Element Shape field, click Show Fiber Thickness.

Now click the Tools and View Style radio button and choose Filled Edges in the Options field. Uncheck the Draw Entity box and then click OK. You can also toggle the "Filled Edges" on and off very easily using the View Style menu located on the View Toolbar. Simply select Filled Edges from the View Style menu to turn them off, then select the command again to turn them back on at any time. Notice that the stress is now shown through the element thickness.


Tutorial 4-17


This is the end of the example. Save your model.


Tutorial 4-18

Nei Nastran Tutorials

Recommend Documents