Analysis

Analytical Modeling Comparison ANSYS vs. RISA 3D: Part One

Imagine, staring at intricate CAD drawings while scratching your head. Trying to figure out where to begin structurally analyzing something with so many complicated shapes. With both limited time and resources, what are your options? Should you approximate the geometry to standard sizes? Most would say their options are limited.

Industry standards consist of widely used software such as RISA-3D which provides a fast and low cost solution for standard shaped structures, however, in today’s world, these software applications cannot always adequately encompass a growing array of eccentric structures. Therefore, other methods such as Finite Element Analysis (FEA) are necessary. Unfortunately, FEA such as ANSYS licensing can be expensive which limits the amount of industrial usage.

At Site Pro 1, both RISA-3D and ANSYS Workbench are at the forefront of analysis, which supports the innovation of product design. By cultivating the strengths between each method, we reduce design time, lower costs and provide exemplary engineering product support.

By now you are asking, “What are these strengths?” and “Is it really useful to use both?” or “How well does RISA-3D perform against ANSYS Workbench?”. Let us find out together!

Model Setup

We begin by creating a simple wall mounting structure similar to the SBWM-HD using several different methods for the purpose of comparison. The simulation software applications RISA-3D and ANSYS Workbench 18.1 were both utilized. The wall mount is comprised of two cantilevered flat bar plates (3”x4”x0.5”) that attach on the ends of a 2.0” schedule 40 pipe (2-3/8” OD x 6’-0”). Figure 1 depicts the geometry described above. Additionally, both plate and pipe material are comprised of A36 grade steel. The FEA model omits any realistic connections such as welds and bolts to allow for direct comparison between both modeling software applications. Only a solid-shell elements model is presented because all combinations of solid-shell, and beam elements were tested.

Five methods were modeled for comparison between both software applications. Theoretical calculations are based off on a 2-dimensional frame structure. The RISA-3D model was analyzed in multiple ways in an attempt to cover the various ways one would model a wall mount structure using the software. The reaction forces on both plates and deflection located center of pipe are listed in Table 1 and Table 2, respectively.

There are 5 methods of comparison used for this analysis:

1. Hand calculations using a 2-dimensional frame with fixed-fixed boundary conditions.
2. RISA-3D wall mount made of all beam structures.
3. RISA-3D wall mount made using beam and plate elements.
4. RISA-3D wall mount made using RIGID links instead of flat plate.
5. ANSYS wall mount made using solid-shell elements.

The ANSYS model was meshed with solid elements for the plate and shell elements for the pipe. The number of nodes in the simulation are 63,026. The number of elements in the model are 38,344 and the average element quality is 0.99. Solid elements were meshed with a 0.0625” mesh sizing to avoid locking effects due to bending and shell elements were meshed with 0.25” sizing. The CAD in the model was created using Autodesk 2016.

The boundary conditions between all models remains constant. Each model has a fixed connection on top and bottom of the plate with a wind force of 1500 lbs and a vertical load of 750 lbs located at the center of the mast pipe. No eccentric loading was considered. Member forces were calculated using TIA-222-REVG loading. (180 mph wind speeds, 400 ft elevation, exposure class C)

Results

Based on the method of superposition, the reaction forces for an indeterminate frame were solved for the wall mount geometry mentioned. Figure 4 shows the controlling wind and weight forces applied along with their respective reactions on the frame structure. Table 1 lists the reaction forces for every case and Table 2 lists the deflection at the center of the pipe between all the cases.

Figure 5 shows both the unity-bending in the RISA-3D models and the Von-Mises stresses for the ANSYS model. When three beams are utilized in the RISA model, the plates are failing and pipe is near capacity. When modeling the plates using plate elements, the pipe is failing but the plates only depict localized stress concentrations. When modeling the pipe and omitting the plates with Rigid links, the pipe is well under capacity. The ANSYS model shows that the only area failing are local stress concentrations at the unrealistic connections between the pipe and plate. Figure 6 and 7 show the ANSYS model and the localized stresses that occur on the plates. Figure 8 shows the localized Von-Mises stresses for the RISA-3D plates. Figure 9 depicts the deformation at a scale of 20 times actual scale with the RISA-3D plate model depicting the largest center pipe deflection. Table 2 details the deflection for each case.

The theoretical frame closely matches the all beam model in both deflection and joint reactions, which is logical since both models are using the same base equations for analysis. The percent difference between mid-pipe joint deflection is 5.7% and 10% for joint reaction. However, both the theoretical and the all beam are drastically different from the ANSYS model by nearly 75%. The theoretical model and the all beam model assume full moment transfer; however, the ANSYS model clearly shows large bending on the top plate, which causes inadequate moment transfer to the fixed end.

A moment release was added to account as a pseudo 6th case to try and replicate the ANSYS reactions. The reaction forces of the sixth case are near identical with the ANSYS model as the percent difference is 2%; however, the deflection at the center point is over 44% percent different. The moment released all beam most closely relates to the ANSYS reactions.

The plate RISA model and the fixed structure both inadequately capture the deflection and reaction forces. The rigid links underestimate the deflection and evenly divides the forces on the top and bottom plate, which is unrealistic, but the pipe strength in the rigid model is within 2% percent difference on the mid-section compared to the ANSYS stress levels. The plate model has a stress field similar to ANSYS as seen comparing Figure 7 and Figure 8 as the stress concentrations yield a similar distribution of Von-Mises stresses; however, the pipe in Risa-3D is failing by more than ANSYS because the plate system overestimated deflection which causes extra stress induced on the pipe.

Based on the results between all the RISA-3D models, replicating the ANSYS FEA is not an easy feature while using RISA-3D. To adequately match the ANSYS Workbench, one would need to use all of the RISA-3D variations to piece together the results. ANSYS is a powerful tool, the localized stress fields shown allow for not only a far more accurate analysis but detailed as well. Table 3 lists the strengths and weaknesses between each program.

Conclusion

RISA-3D and ANSYS Workbench are at the forefront of our analysis, which supports the innovation of product design. By cultivating the strengths between each method, we decrease design time, lower costs, and provide exemplary engineering product support.

Based on the results between all the RISA-3D models, replicating the ANSYS FEA is not an easy feature while using RISA-3D. To adequately match the ANSYS Workbench, one would need to use all of the RISA-3D variations which is insufficient for addressing uniquely complicated designs.

In part 2 of this series, we will spotlight the SBWM-HD using some of the same methods presented in the above article.

Joseph Trimble

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.