Fretting Fatigue

The fretting fatigue module in FRANC3D/NG is a specialized add-on to the regular version of the program. It consists of the menu items and dialog boxes or wizard panels that are described below.

Step 1: The top menu bar in FRANC3D/NG includes a Fretting menu item, which has a number of sub-menu items below it, Figure A.1. The user must first Read model datainto FRANC3D/NG. Either ANSYS cdb or ABAQUS inp files can be read. The input files should contain regions of elements differentiated by material id as well as node sets that define the master and slave contact surfaces (and possibly edge-of-contact node sets).

Figure A.1 Main menu bar in FRANC3D/NG includes Fretting (left panel) and this menu has seven sub-menu items (right panel).

 The program reads the input file and then prompts the user to select the regions based on material id, Figure A.2 – top left. The user can choose to color the regions using different colors. The next wizard panel, Figure A.2 – top right, asks for the node set that is the master contact surface. More than one node set can be selected. The next wizard panel, Figure A.2 – bottom left, asks for the node set that is the slave contact surface. Again, more than one node set can be selected. The last wizard panel, Figure A.2 – bottom right, asks for the node set that is the edge-of-contact. If there is not a well defined edge-of-contact, the user does not have to choose any of the node sets. Selecting Finishwill cause the program to finish reading all the data and to display the model, Figure A.3.

Figure A.2 Finite element input file filter panels allow the user to select material regions, master and slave contact surfaces, and the edge-of-contact node set.

Figure A.3 Example model read into FRANC3D/NG with material regions colored.

Step 2: The next step is to Read disp/stress/strain, Figure A.4 – left panel. The program can read the analysis results data for the above (uncracked) model, which should include nodal displacements, stress, strain and contact status. Up to three load cases can be defined, Figure A.4 – right panel. For a typical fretting test specimen, loading is often applied in three steps. First the normal pressure is applied, then a positive shear load is applied followed by a negative shear load. The three load cases enable the RAI-Q parameter to be computed (actually only the first two load cases are necessary and we assume Qmin=0). We cannot compute the RAI-Q parameter if there is only one load case and no clearly defined edge-of-contact. (The Qparameter is based on the relative (shear) displacement at the edge-of-contact.)

The user is prompted to enter the file names for the load cases (this wizard panel is not shown). For ANSYS, the user specifies the .dsp file names and the program then attempts to read the .str, .stn and .cnt files assuming the same file name prefix.

Figure A.4 Fretting menu – with Read disp/stress/strain… highlighted (left panel) and the first wizard panel (right panel), which defines the number of load cases.

 Step 3: Once the analysis results are read, FRANC3D/NG redefines the contact surfaces and the edge-of-contact based on the contact conditions from the first load case. The user can display these items using the Display contact surface… menu item, Figure A.5. The Display dialog, Figure A.6, allows one to highlight contact surfaces (top left panel of Figure A.6), nodes that are in contact (top right panel of Figure A.6), edge-of-contact nodes (bottom left panel of Figure A.6), and the local bases at the edge-of-contact nodes (bottom right panel of Figure A.6).

Figure A.5 Fretting menu – with Display contact surface… highlighted.

Figure A.6 Fretting Display dialog allows the user to display the contact surface (top left panel), the nodes in contact (top right panel), the edge-of-contact nodes (bottom left panel) and the local bases at the edge-of-contact nodes (bottom right panel).

Step 4: The next step is the computation of the fretting parameters and the subsequent calculation of number of cycles to fretting crack nucleation. The Fretting crack nucleation… menu item, Figure A.7 – left panel, leads to the wizard panel shown in the right panel of Figure A.7. For this example, all of the fretting parameter models are active because we read three load cases and the results included stress and strain (as well as displacement and contact status).

Figure A.7 Fretting crack nucleation… sub-menu item (left panel) leads to the Fretting Crack Nucleation wizard (right panel).

Based on the Equivalent stress selection, the wizard panel shown in the top left panel of Figure A.8 is displayed. The first panel allows the user to set the fitting parameters to compute the number of cycles from the computed equivalent stress. It also allows the user to Do averaging of the stress and strain near the node(s) of interest. The top right panel of Figure A.8 shows the edge-of-contact nodes with blue spheres about each node. The averaging occurs based on the size of the sphere. We sample points in the region of interest and within the sphere region. The lower left panel of Figure A.8 shows one of these nodes and spheres in more detail. The green marker is the corresponding contact point on the “slave” surface. The black line indicates the region and the radius of the sphere. Selecting Nexton this panel, leads to the panel shown in the bottom right of Figure A.8. This panel allows the user to display the node ids and to color contour the values for number of cycles (to fretting crack nucleation).

Figure A.8 Fretting Crack Nucleation wizard panel (top left) based on the Equivalent Stress option. The top right and lower left panels show the region in which stress/strain averaging occurs if the user selects this option in the first panel. The bottom right panel shows the final wizard panel with number of cycles contoured.

Step 5: If the number of cycles to fretting crack nucleation indicate an initial crack location, the user can choose to automatically extract a sub-volume from the full model so that discrete crack growth simulations can be performed. The left panel of Figure A.9 shows this sub-menu item highlighted, which leads to the dialog shown in the right panel of Figure A.9. The user can choose the size of the region to extract as well as the region from which the elements will be extracted. In this example, material region 4 is shaded and this is the region selected for element extraction.

Figure A.9 Extract subvolume… sub-menu item (left panel) and the Subvolume Extraction dialog (right panel).

The elements within the extraction ‘box’ can be saved to a local (.cdb or .inp) file and the remainder of the full model can be saved to a global (.cdb or .inp) file. The cut-surface element facet nodes are collected into a component called “cut-surface” and these can be retained when reading the cdb files into FRANC3D/NG, Figure A.10. The local model is automatically imported back into FRANC3D/NG and is ready for discrete crack insertion.

Figure A.10 Local subvolume model (left panel) and the remaining global model (right panel) showing the retained mesh facets on the cut surfaces.

文章分类 应用案例