IPENZ Engineers New Zealand

HOME > publications > engineering-NZ > volume53-1998 > 1998-04-apr > manufacturing

Applied Computing</h3>   How Do I Know It's Right? <HR>Don Campbell is a director of Matrix Applied Computing Ltd, Auckland A difficult question for any engineer, not just those using Finite Element Analysis. It always reminds me of the Calvin and Hobbes cartoon where Calvin asks his father how bridges are designed, and is told that they build it, drive heavier and heavier trucks over it until it breaks, then weigh the last truck and rebuild the bridge with that weight limit! As discussed in the last article (NZE December 1997), errors in the finite element model can be introduced by oversimplifying the analysis and ignoring non-linear effects. Errors can also be introduced through loads and/or boundary conditions that poorly approximate the "real world". However, even for well-defined linear static analysis work, modelling errors can be introduced by an analyst's oversight. This article discusses how an analyst goes about verifying their model _ if necessary this can be done by another analyst providing a peer review. Check A fundamental check in meshing is examining the model for free edges: regions where adjoining elements don't share common nodes. Most modern mesh generation software allows the analyst to check this, and equivalence these coincident nodes. However, this process can trap the unwary analyst who believes that simply increasing the equivalencing tolerance will fix this problem every time: if adjoining surfaces have dissimilar mesh densities as in Figure 1, just equivalencing can't fix this _ the analyst must ensure that the surface edges have a common node spacing, or use multipoint constraints along the problem edge. A large equivalencing tolerance can potentially cause the collapse of elements with edges smaller than the tolerance, or cause elements to become highly skewed. As mentioned in one of my earlier articles, shell models assume that the plate thicknesses are small relative to the model dimensions. The analyst must remember that the shell elements model the midplane of the physical plates _ something that needs to be considered before creating any geometry. Shell elements also typically have five degrees of freedom (DOF) per node (no in-plane "drilling" DOF), as compared to a beam element's six and a solid element's three (no rotational DOFs). This requires care when creating a model that combines these element types. Simply connecting a shell mesh to a solid mesh will imply no moment transfer at the mesh boundary _ easily seen when examining the deflected shape. Examining the deformed shape should be a matter of course for any analysis, particularly if symmetry has been used. The analyst must check that the model is indeed satisfying the boundary conditions that he/she believes to have been imposed. The result of omitting such a boundary condition is that essentially only half the structure is being analysed! Another issue that arises is the necessity to halve loads and plate thicknesses applied along a symmetry plane. Plate thicknesses can be checked by contouring element thickness. Examination of the magnitude of deflection will indicate potential errors in the value of Young's modulus. Material properties are difficult to check visually and must be rigorously checked especially for dynamics, centrifugal loading etc, where many an analyst has used incorrect units. For these types of problems, sticking to SI units is a wise choice. Hand calculations Models involving the use of shell elements and pressure loads must have their element normals checked as a positive pressure typically points in the direction of the element normal. Elements with reversed normals (to the rest of the model) will also have the direction of the pressure load reversed. A mixed system of element normals will also lead to confusion in results interpretation for shell elements where the inside surface of some elements will be adjacent to outside surfaces of other elements. It is good practice to look at the total resultant load and compare it against hand calculations. There will typically be some small discrepancy due to the finite element model being facetted, but errors larger than 2-5 percent usually imply modelling problems. Another modelling consideration with pressure loads is whether the load at a cut in the model needs to be reacted, for example the vessel/nozzle intersection shown in Figure 2. If the axial pressure load in the nozzle is eventually reacted at a constraint, this tensile force (equal to pressure times the area of the nozzle) must be applied where the model has been cut. Another problem that can occur in pressure vessel analyses is out-of-roundness, where, perhaps due to mesh refinement, some nodes no longer lie on the vessel radius. This has the effect of introducing a "flat" into the shell, which can be difficult to spot _ can you see it in Figure 3? However, examination of the deflected shape quickly shows up the error, as in Figure 4. This example shows the importance of the analyst critically examining output: "trust but verify!" The final example illustrates a results post-processing trap: comparing a plate clamped at one edge with a load applied to the another with a stiffener as in Figures 5 and 6. Our engineering judgement tells us that a stiffener in this orientation should have a minor effect, but the results shown in Figure 6 show a spurious decrease in the plate stresses around the stiffener. This is due to the post-processor averaging the stresses in the plate and stiffener, artificially lowering the stress in the plate. This is avoided by not averaging across the plate boundaries, as in Figure 6. Verify, verify, verify Most of the modelling time nowadays should be spent in verifying results, as modern tools have made creation of the model a much simpler process. Answers should be checked against analytic solutions in regions of the model where an approximate analytic solution is applicable. This can often be achieved by extending a model to include a region removed from complicating influences such as stiffeners, boundary conditions and load application areas. However, there is a limit on how far hand calculations can be taken: we have found simplifying assumptions made about the stiffness of parts of the structure in these can lead to quite large discrepancies with the finite element results. Experience has shown that providing that the finite element model has been checked as above, it provides a better solution for the "model". Hopefully this article has supplied the basis for a list of model checks to be carried out, both before and after the analysis. In a subsequent article I will discuss the issue of verifying a valid finite element analysis against "the real world" _ the ultimate test of knowing that it's the right answer! <HR> </td> </tr> <tr> <td width="30"><img src="/ipenz/images/front/1x1tr.gif" alt="Blank space" width="30" height="50"></td> <td width="160" valign="top" align="left"><img src="/ipenz/images/front/1x1tr.gif" alt="Blank space" width="160" height="50"></td> <td width="20"><img src="/ipenz/images/front/1x1tr.gif" alt="Blank space" width="20" height="50"></td> <td width="400" align="left" valign="top" class="bodya"><img src="/ipenz/images/front/1x1tr.gif" alt="Blank space" width="400" height="50"></td> <td align="right" valign="top" width="250"> </td> </tr> </table> <div id="footer"> © 1996 - 2010 IPENZ </div> </div> </body> </html>