Because this is a fairly large model with a time consuming analysis, and for the sake of simplifying this example, it has been semi-automated for you. This is done to help speed up the study of this exercise. However, all the steps necessary to reproduce the results manually are indicated if you desire.

To begin, start up Pre & Post or MSC Patran and open a new database, giving it the name knuckle. (Any Analysis Preference will do for this analysis, but leave it at MSC Nastran when asked.) Initially you will need these files copied over from the central installation area to a clean, empty working directory: knuckle.out, knuckle*.nod, knuckle.nod_tmpl. (There are 12 .nod files where * = 1 through 12.)

This has been automated by running a session file (a file full of commands to be executed). Copy the file knuckle.ses to your directory and then from the File | Session | Play command select the file and click Apply. Answer Yes to any questions. Playing this session file accomplishes the following which you can do manually if you wish:

The entire model should have appeared in the graphics screen including the loading devices. The neutral file that you read in the previous step contained some convenient groups called KNUCKLE_ONLY and SURFACE_NODE. Post the KNUCKLE_ONLY group from Group | Post; select KNUCKLE_ONLY and click Apply. Only the knuckle itself should appear in the viewport now.

These groups were created automatically for you, however we digress a bit here to teach you how to easily create some convenient groups for subsequent fatigue analysis. These techniques are especially helpful with large solid models. This discussion is not crucial to the successful completion of this exercise. You may skip to the next step if you wish.

To create a group of external elements, thus removing all internal elements use the list functionality - Tools | List | Create. Set the Model to FEM, the Object to Element, and the Method to Attribute. The Select Mechanism will appear from which you should select the Elements with free faces option.

Graphically surround all element of the model using the mouse by clicking and dragging from the top left corner down to the bottom right corner. All the elements with free faces will be selected. Click the Apply button to add these elements to the List A form, then on the List A form press the Add to Group... button. On the form that appears, give a new group name such as Surface_elements and click the Apply button. Press Cancel to close the form. A new group now exists with only the external elements.

Because fatigue damage usually only initiates on the surface of components, it is helpful to have a group of surface nodes only. The previous group we made only contains elements. By creating groups with only the surface nodes we can speed up the analysis by eliminating nodes from the analysis in which we are not interested.

With the Create List form still open, set the Object to Node and the Method to Association. The Association should be set to Element Face and the Target List needs to be set to “B” (or you can Clear the List A contents). Now before proceeding, go to Group | Post and post only the group you just created, Surface_elements. Cancel the Group form when have accomplished this.

Now on the Create List form, set the focus (click the mouse) in the Element Face databox. The Select Mechanism will appear again from which you should select Free face of element. Then surround the entire model (by clicking and dragging with the mouse) as you did before to select all free faces. Click the Apply button. The List B form will fill with the nodes associated to the free faces. Add these nodes to the group Surface_elements. Now you have a group with only the external elements and the external nodes of the model.

Cancel the Create List form to close it down.

Open the Results application and plot the stresses from any of the result cases. Make plots of the von Mises stress for load cases 7, 8 and 9 in turn. Note how the individual load cases cannot be relied upon to predict the fatigue hot spots.

Specifically plot the Z component stresses and note that they are very close to zero over the majority of the model except at the loading points as would be expected. (A good look at these stresses would reveal model quality.) The results are surface resolved stresses, meaning the two major principal stresses lie in the plane of the surface with the third principal stress being zero (normal to the surface). This is important for models with solid elements especially given that 99% of cracks initiate on the surface. The principal stresses correspond to the X, Y, and Z component stresses.

The main reason that we need surface resolved stresses is for the biaxiality analysis to properly calculate the biaxiality ratio which will be discussed later in this example. Without surface resolved stresses it would be difficult, if not impossible, to assess the multiaxial stress state of the component.

Many FE analysis codes will calculate surface resolved stress or may give you the option to do so. The best approach is to first assess the magnitude of the out-of-plane component to determine if the stresses are already surface resolved. If you find that you need to resolve your stresses, MSC Fatigue can do this for you with a couple of easy steps. Physically the out-of-plane stresses must be zero (unless subject to some sort of hydrostatic pressure).

Although this is not necessary for this example, to have MSC Fatigue surface resolve your stresses for you during a fatigue analysis you must first create a vector file (for coordinate transformations).

Before submitting your fatigue job, open the Job Control... form. The Calculate Normals option is an essential precursor to running the biaxiality analysis with a solid model if you know your results are not surface resolved (z-normal is not zero). This routine determines surface normals at each surface node, and writes them to the file jobname.vec. MSC Fatigue detects the presence of this file and uses it to define a local coordinate system at each surface node that has its z-axis normal to the surface. The stress results in the fatigue analysis input file are then written in this coordinate system, permitting the software to carry out a biaxiality analysis in the x-y plane only.

Do not run this unless you have some time to spare because of the size of this model. (Besides the stresses are already surface resolved.) A graphical depiction of a normal vector calculation is shown to the side.

During the fatigue analysis translation surface resolved stress tensor files are created with the name jobname_lc#.nod where the # is the load case number. There will be one file for each load case in the fatigue analysis setup. You can read these .nod files back into the database exactly as described earlier (using the jobname.nod_tmpl file) to evaluate the success of the surface stress resolution (by plotting the Z component stress from these files).