The case study is for a regeneration gas-fired heater, designed and supplied for a project in Oman. Its design is of the vertical cylindrical type, according to the API 560 standard. The heater is equipped with a single burner and forced-draft fan. The fuel is a gas constituted of a mixture of various hydrocarbons. The main components are methane, ethane and propane: these components account for the 90% of the total mixture. The radiant section is cylindrical, and the process tubes are vertical. The fluid is distributed in four parallel passes, with 12 tubes per pass (creating a total of 48 tubes in the radiant section).
The burner is located on the floor of the chamber. It’s a staged fuel burner: a portion of the fuel and all the combustion air are mixed in a primary combustion zone, while the remaining fuel is supplied through a series of nozzles around the perimeter of the burner. Before entering the combustion chamber, the air flows through a swirler to ensure proper mixing in the primary combustion region. A picture of the burner is reported in Figure 2.
The aim of the analysis was to determine the flame length in three different operating conditions: Table 1 reports the burner heat release, the radiation duty absorbed, and the flow rates for both air and fuel for the three cases considered.
While many definitions are possible for the flame surface, for the purpose of this work, the flame was defined as the iso-surface at a temperature of 1400K.

The model was implemented by EnginSoft. Starting from the burner manufacturer’s drawings, a 3D model was created directly using ANSYS ICEM CFD, which was also used to mesh it.
Since the focus of the analysis was the flame structure, only the radiant chamber was modeled. Given the symmetries that are present, there was a possibility to analyze only a portion of the domain,. Unfortunately, the symmetries didn’t exactly match each other: there were 6 nozzle for the staged fuel, 10 for the primary fuel, 4 tube passes and 48 tubes. The only effective symmetry was a 180° portion of the domain, especially because the domain outlet was rectangular and not circular. For greater accuracy, it was better to simulate half of the radiant chamber. However, this required significant computational time.

Figure 3 - 3D models
(a) 180° model, (b) 60° model

In order to understand the effects of the periodicity of the staged fuel nozzles, two models were created: one model had a periodicity of 180°, the other 60°. In the second model, the nozzle diameter of the burner was opportunely scaled obtain the correct exit velocity. The temperature of the process fluid was also adapted to reflect the correct process duty absorption from the domain. The aim was to understand the impact of the assumptions of the simplified model on the flame height. For this purpose, both two models were solved for Case 1, and the results were compared. The two models are depicted in figure 3. The case was solved with ANSYS CFX.
The following boundary conditions were set:

• Inlets: Mass flow rate, composition and temperature were specified for both air and fuel. For the 60° model, an inlet velocity profile was set; it was determined with an independent model of the swirler.
• Outlets: gas flow exits the fluid domain. A pressure was set. An energy sink was defined in order to consider the radiant heat transfer to the shock tubes. A pressure drop was set to simulate the presence of the tubes of the convective section and set the correct air pressure at the inlets.
• Process tube walls: Heat transfer coefficient and bulk temperature were set; the temperature values are indicated in the datasheet, the wall heat transfer coefficient and tube emissivity were set in order to extract the heat duty absorbed by the tubes, as defined in table 1.
• External walls: the heat loss was simulated using a heat transfer coefficient and an outside temperature

The chemical reactions that take place in the system were explicitly simulated in order to accurately predict the temperature field in the entire system. The following reaction mechanism was included in the model:
The SST (Shear Stress Transport) turbulence model was applied. The buoyancy effect was considered. The Monte Carlo Radiation Model was applied for the radiation heat transfer.

Figure 4 - Velocity streamlines
Case 1, (a) 180° model, (b) 60° model

The Velocity streamlines are reported in Figure 4 for the 180° model and the 60° model. The typical flow pattern of a heater can be seen: the fuel and air enters at the bottom, the flue gas flows through the center of the chamber. Part of the cold flue gas flows downwards along the tubes at the periphery of the chamber. The streamline patterns are quite similar for the two models.

Figure 5 - Temperature profile
Case 1, (a) 180° model,(b) 60° model

Figure 5 reports the temperature profile at the symmetry plane for the two models: the points with the highest temperature are located in the combustion region over the burner, where the chemical reaction takes place. The coldest region is located in the lower part of the chamber at a distance from the burner: the recirculating flue gas flows downward and is cooled by the process tubes. The difference in the temperature profiles between the two models is concentrated in the lowest part of the chamber.
The iso-surface at 1400K is depicted in Figure 6.

There are some differences in the shape of the surfaces, especially at the bottom. Figure 7 reports the maximum height of an isosurface for many temperatures: at 1400K, the difference between the values predicted by the two models is limited.

Figure 6 - Isosurface at 1400K
Case 1, (a) 180° model, (b) 60° model

Figure 7 - Maximum height for iso-surfaces at given temperatures

Both values are lower than the maximum flame height for this specific heater (9 m).
The other cases were run using the 60° model. The streamlines for these cases are reported in Figure 8, while the iso-surfaces are depicted in Figure 9. The flame heights are 7.37 m and 4.83 m respectively for case 2 and 3.