Cracks, sharp edges, and holes: no, this article does not pertain to the stressful road conditions in the Midwest after a long winter season. While the three prior mentioned are all causes of stress risers (and in more ways than one) to engineers, they are a serious design concern as they can drastically reduce the life of a structure typically through fatigue.
Traditionally, one would calculate stress concentration factors theoretically by using charts  and factoring that into the overall limit state design. With today’s technology, one can analyze structures with finite element analysis to help identify and locate such stress risers.
In this article, we are going to model a Valmont Site Pro 1 equivalent standoff arm cantilevered using finite element software ANSYS and RISA 3D to compare results and investigate stress concentrations.
The 36 inch square tube standoff arm was modeled in both ANSYS workbench and RISA-3D. The dimensions of the square tube are 4x4x3/16. Linear-elastic and isotropic A36 grade steel was utilized in both analyses and the weld material was E70. The ANSYS model includes both ½ inch end-plates and ¼ inch welds. The ANSYS model was meshed using tetrahedral solid elements with refinement on the welds; 215,000 total mesh elements were created.
The controlling wind load, 90 degrees, was determined by a parametric study of load cases using TIA-222-Rev G codes. Fixed supports were applied to the bolt holes in the ANSYS model. The maximum design load was 1,800 lbs of tangential wind and 900 lbs of vertical load. The RISA-3D model omits end-plates and a fixed support was applied on the end node. The RISA-3D model Figure 1a and figure 1b depict the boundary conditions in each respective program. Figure 1c depicts the tetrahedral mesh.
Figure 2a and figure 2b detail the ANSYS stress results from the analysis. The maximum equivalent stress occurs at the toe of the corner welds and between the plate and square tube as shown in figure 2b. In FEA, singularities  (infinite stress) can occur in areas that have high stress concentration. To check for singularities, a mesh independence study was accomplished.
The nominal stress calculated in the ANSYS model was 34,500 psi. By dividing the maximum stress of 98,927 psi by the nominal, a stress concentration factor (K) of 2.85 was calculated.
In the RISA-3D model, the capacity of the square tube is at 85% as shown in figure 3. Unity is a ratio of actual stress to allowable. The stress on the square tube in RISA-3D is 27,500 psi. To calculate the theoretical stress concentration factor, the idealized flat bar in bending was utilized from figure 4. The theoretical stress concentration factor was calculated to be 2.2 by using the geometry ratios r/d of 0.0625 and D/d of 2.125. The stress concentration calculated using Risa-3D and the theoretical stress concentration factor equates to 60,500 psi. The percent difference between the ANSYS model and RISA-3D model is 39%.
Total deformation at the end of the cantilever arm from the ANSYS model was 0.168 inches as shown in figure 5a. The deformation at the end of the cantilever for the RISA model was 0.16 inches as shown in figure 5b. The deformation between the two models was agreeable as the percent difference was 5%.
The ANSYS model predicts a higher stress concentration than the RISA-3D model under worst case loading conditions. The ANSYS model equivalent stress was 60% greater than the RISA model prediction (39% percent difference) while the deformation between both models were within 5% agreeance. The ANSYS model locates the highest stress concentration between the corners of the square tube and plate at the weld toe.
By modeling the structure in both software, we are able to compare results between traditional analysis techniques and those of finite element analysis and utilize this data to enhance our products for maximum strength and durability.
 Pilkey, W. D., Pilkey, D. F., & Peterson, R. E. (2008). Petersons stress concentration factors. Hoboken, NJ: John Wiley.
 Abbey, T. (2017, August 15). Dealing with Stress Concentration and Singularities. Retrieved from http://www.digitaleng.news/de/dealing-stress-concentrations-singularities/
Joseph Trimble graduated from Purdue University-Northwest with a Master of Science in Mechanical Engineering in 2016. While a graduate student, he worked as a researcher utilizing numerical methods such as finite element analysis for structural and fluid dynamic analyses. Learn More