Engineering Product Structural Analysis

The 5G Revolution is Here: An Inside Look at the Engineering Behind the APT (Adaptive Pole Top) Product Line.

December 12, 2019

Today, we’re going to dive in for a behind the scenes look at the inner engineering of Site Pro 1’s revolutionary new APT (Adaptive Pole Top) line of small cell products. The APT series is a modular, leveling adjusting, top pole mount line for both shrouded and unshrouded 5G and 4G applications. For this article, we’re going to look at part number APT-3X2T2290V shown in figure 1 below.

Figure 1: APT-3X2T2290V

Before we start going through the engineering however, we should probably explain the part number nomenclature; It will help you select the right part should you decide to purchase from the APT line in the future. See figure 2 below.

Figure 2: Nomenclature

Finite Element Analysis

Since the geometry has complex shapes and plastic components, Finite Element Analysis was the only means capable of capturing the physics for accurate load capacities. Therefore, the APT series was simulated computationally then physically tested.

Modeling Process

We began by building a full 3D model of the APT-3X2T2290V in Autodesk Inventor which consisted of both the plastic (ABS) shroud and structural steel components. The shroud connects into the steel from the ring plates and each ring plate is vertically stacked and connected using a mast pipe (schedule 80 pipe 2.5). The bottom ring plate allows for easy level adjustment at the threaded rod connection. The APT line can attach to poles of up to 18 inches in outer diameter. For the analysis, the smallest pole size (8 inch OD) was utilized.

Once the CAD was complete, the model was converted and exported into ANSYS Workbench to analyze the maximum load capacity.

ANSYS Analysis

The shroud was meshed using shell elements with a defined thickness of 1/8 of an inch. Since the thickness is drastically lower than the other two dimensions, the shell element assumption is valid. Figure 3 shows the shell element mesh. All the Bolts except for the threaded rod were analyzed using beam elements. Shells and beams were used to reduce the computational run time for the simulation. The steel components were modeled as solid elements with a 3/16 inch sizing. Figure 4 shows the solid elements used on the steel. The total number of elements was 650066 and the total number of nodes was 1449525. The average element quality was 0.82.

Figure 3: Plastic shroud elements.

Figure 4: Steel component elements.

Boundary Conditions

The boundary condition applied in the model is a fixed condition at the pole stub along the base as seen in figure 5. The force applied to the shroud corresponds to TIA-REV-H loading for 150 mph ultimate wind speed at a 50 ft. elevation with an exposure class C condition. The effective projected area (EPA) for the shroud can change depending on various interpretations of the drag coefficient because the irregular shaped shroud pieces. The calculated EPA value for the shroud ranges from 12.4 square feet (sq. ft.) to a maximum of 17 sq. ft. For the purpose of this simulation, the EPA was calculated to be 16 sq. ft. Figure 6 shows the applied frontal loading across the shroud. Finally, the considered dead load of 600 lbs. was applied to the structural steel mast pipe. 100 lbs. were applied to the top cantinas pipe and 500 lbs. were applied to the antenna pipe section

Figure 5: Fixed support.

Figure 6: 150 mph wind loading.

Results

The goal for the analysis is two-fold. For this simulation, both the shroud and the steel needs to fall below their respective material yield strengths (YS) to be considered passing. The steel is rated for a 35000 psi minimum YS. The threaded rod is grade 5 J429. As you can see from Figure 7a, the Von-Mises average 18,000 psi across the structure with stress concentrations near the level adjustment. From Figure 7b at 150 mph wind speeds, the adjustment clips (the L shaped connector) are around 31000 psi. The threaded rod, which has a YS of 92,000 psi, is around 83818 psi. It’s worth noting only the clip and threaded rod closest to the wind direction is highly stressed as the two other clips are under stressed which indicates that this is the worst case wind loading direction. When the wind direction is tangential, the loading is split near evenly amongst two adjustment clips.

Figure 7a: Steel component Von-Mises stress.

Figure 7b: Steel component Von-Mises stress (detailed view).

ABS plastic has a breaking strength of 6100 psi. From the simulation, the frontal wind reaches 3000 psi on the antenna panel center with a stress concentration of 5000 psi on the shroud bolt clip connection. This suggests that 150 mph is the maximum that empty panels are able to endure. It’s worth noting that the panel is stressed because of its ability to flex which causes concavity at high wind speeds. In reality, the antenna panels will be replaced by 4G/5G antennas that attach directly into the mast pipe and thus the shroud will not see this load. Figure 7c shows the stress acting on the antenna panel which causes concavity.

Figure 7c: Shroud component Von-Mises stress.

The total deformation for both the shroud and structural steel are found in Figure 8a and Figure 8b, respectively. The deformation is relative to the size of and length of the pole stub. For a large pole of 50 ft., one would need to add the additional deflection of the pole in the wind to find the true deflection. The engineered forces as mentioned earlier are set for a maximum of 50 ft. and the pole stub is 8 in. OD with a length of 3 ft. A full pole was omitted to save computational time. Again, as previously stated the deformation on the shroud would be less if antennas were mounted versus empty panels as the concavity of the panel would not exist.

Figure 8a: Shroud component total deformation (x5 scale).

Figure 8b: Steel component total deformation (true scale).

Physical Analysis for Validation and Verification

While we won’t go in depth on the testing procedures in this article, qualitative physical testing was done in-house to help verify and validate the FEA model.

A prototype of the APT-3X2T2290V was assembled on a pole stub and pulley load cell system was applied to the top ring collar using shackles. Loading was ramped until failure. Figure 9 shows the testing failure at the clip angle and threaded-rod. Large normal loading will cause the clip and rod to bend in the direction of the wind load but tangential loads are shared between two rods. The wood pole size was larger than 8 inch OD and because the OD was wider the clip angles are flipped outwards compared to the simulation model. While the testing results are not a replication, they show that failure occurs in the same exact spots on the threaded-rod and clip angle for both physical testing and simulation. Figure 10 shows a comparison between the ANSYS Workbench simulation and the physical test. The clip angle is bent in opposite directions because of orientation, but the threaded rod exhibits the same bent profile.

Figure 9: Physical testing.

Figure 10: Physical testing vs ANSYS (x40 scale).

Conclusion

Isn’t it a beautiful sight when reality meets expectations? The small cell product line including the APT series was designed and engineered to be a universal/modular solution for 5G. The top pole mount was designed and tested for 150 mph wind loads by using FEA and physical testing. By using all of the tools at our disposal like ANSYS Workbench, we tackle not only the problems of today but the problems of tomorrow through superior product analysis.

You can learn more about Site Pro 1’s new small cell product line including the APT series and other new products by reading the new 2020-2021 Wireless Site Components Catalog or visiting the product detail page. Stay tuned for more 5G, Small Cell articles on Site Pro 1 Connection. Feel free to leave a comment below to let us know what you think.

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. Learn More