Meshing of Rocket Engine Nozzles for CFD

Figure 1: Structured multi-block meshing of rocket engine nozzles.

1902 words / 9 minutes read

Introduction

The demands of the Artemis program are pushing the envelope to build larger and more powerful rockets capable of taking more than 140 tons outside the earth’s atmosphere. The SLS rocket of NASA along with the Starship of Space-X are being built with powerful rocket engines to take payloads to the moon and Mars. Designing such high-performance rocket engines is a challenge in itself and CFD is playing a major role in the design and development of these new-generation rocket engines.

For conducting effective CFD computations, generating high-quality grids in accordance with the flow physics it is intended to capture, plays a pivotal role. This means a general understanding of flow physics is essential to do gridding. It need not have to be in-depth, but an overview of the flow physics will aid in generating a good grid.

An Overview of the Rocket Nozzles and Flow Field

Flow fields generated around rocket propulsion systems are complex and fascinating. High gradient flow features like boundary layers on the rocket forebody and nozzle wall, shear layers, internal and external shocks, plume impingement and interactions, etc, all add to the complexity.

Nozzles, the end component of the propulsion system, is a critical part of a launch vehicle assigned with the responsibility to accelerate and efficiently exhaust the combusted and reactive gases according to the thrust requirements. Evolving with times, convergent-divergent nozzles are classified based on the contour of the divergent part as conical, de Laval, truncated ideal contour (TIC), and thrust optimized nozzles.

The performance of a rocket engine depends mainly on the aerodynamic design of the expansion nozzle, with the important design parameter being contour shape and the area ratio. Launch nozzles are designed optimally for a given chamber and ambient pressure conditions. However, they are also built to work in an extremely wide range of pressure regimes, with critical stress points at their lower and upper limits of operation envelope. High-performance rocket nozzles like the American SSME, the European Vulcain, or the Japanese LE-7 operate in extreme pressure ratios starting with one bar ambient pressure at sea level up to near-vacuum in the outer fringes of space.

Overexpanded and underexpanded rocket plumes — **Figure 2: a**. Overexpanded plumes of Delta 4 Heavy Pratt-Whitney engines. b. Under expansion plume from Saturn 1-B launch.

Rocket Plume Patterns

At ground level, with the ambient pressure being higher than the nozzle exit, rocket engines operate in an over-expanded condition. As they ascend, the engines start to experience declining ambient pressure. Correspondingly, the flow starts to adapt to the condition of the ambient pressure becoming equal to the nozzle exit pressure, and later gradually settle down to under expanded condition. Figure 2 shows the photographs of rocket engines under these two off-design conditions. At high altitudes, the underexpansion of the flow leads to further expansion of the gases as can be seen in the above Figure 2b.

In overexpanded plumes, the low-pressure exhaust adapts to the high-pressure ambient condition through a series of recompressing oblique shocks and expansion waves giving it the classical barrel-like structure.

Different types of shock patterns in overexpanded rocket plumes have been observed. Figure 3 shows the three classical patterns – the Mach disk pattern, the cap-shock pattern, and the shock diamond pattern.

The pattern type which develops depends on the nozzle design. In nozzles like ideal and TIC nozzles, a transition from Mach disc pattern to shock diamond pattern can be observed. In them, the flow with small overexpansion adapts to the ambient without forming a strong shock system like the Mach disc. In other nozzles forming an internal shock such as the TOC, TOP, and CTIC nozzles, the cap-shock pattern can be seen.

Overexpanded plumes - Vulcain, with cap-shock pattern, Vulcain, with classical Mach disk, RL10-A5, with regular shock reflection — **Figure 3: a.** Vulcain, overexpanded flow with the cap-shock pattern. b. Vulcain overexpanded flow with classical Mach disk. c. RL10-A5 overexpanded flow with apparent regular reflection. Image source – Ref [4].

The Occurrence of Side Loads

Also, at largely over-expanded conditions, the flow is not fully attached. The adverse pressure gradients cause the boundary layer to detach from the nozzle wall, creating a separation shock. This high Mach number separated flow continues downstream and may interact with the recompression shocks, asymmetric jet portions, or possibly with the internal shock, triggering severe lateral or side loads.

Unfortunately, these side-loads are present quite frequently, and that too at critical stages of engine start-up and shut-down operations. With the increase in demand for higher performance rocket launchers, the nozzles need to be built with a larger area ratio. But an increase in area ratio leads to a higher probability of occurrence of flow separation and side loads for a substantial part of the ascent.

Overexpanded separated flow in VOLVO S1 nozzle — **Figure 4:** Overexpande separated flow in VOLVO S1 nozzle. Image source – Ref [4].

If the lateral loads are large and persistent, severe engine breakdown could happen. Interestingly, it’s been reported that many known engines like the Space Shuttle Main Engine, the European VULCAIN engine, the Japanese LE-7A engine among others have experienced engine breakdowns due to side-loads.

No surprise, that a large part of research funding is spent in understanding the side-load phenomenon. Rightly so, as a clear understanding of flow separation in rocket nozzles is critically essential to prevent sudden engine breakdowns and also for developing reliable high-performance engines.

Over the years, CFD has played an important role in giving valuable insight into this problem. With the ability to provide data for all the pressure ratios in the operation envelope, CFD is highly regarded as an effective tool in the nozzle design cycle. In turn, the complex flow phenomena in nozzles have challenged the CFD community and have compelled them to come up with better, more robust, and accurate CFD algorithms.

Grids play a significant role in obtaining accurate results. Though gridding for nozzles may look easy at first glance, it takes a bit of effort to consciously plan and place optimal points at the right locations to obtain reliable results. So, in order to get a better understanding of the gridding requirements, in the subsequent sections of the article, we try to cover various aspects of meshing nozzles like, typical domain dimensions and grid size, regions that require refinement, etc, are discussed.

a. Typical structured multi-block grid domain for a rocket engine bell nozzle. b. Fine grid clustering near the divergent wall and around nozzle exit to capture the separated shock and Mach disk. — **Figure 5: a**. Typical structured multi-block grid domain for a rocket engine bell nozzle. b. Fine grid clustering near the divergent wall and around nozzle exit to capture the separated shock and Mach disk.

Meshing Rocket Nozzles

Meshing, Considering the Flow Physics

Grid points are usually clustered in regions of high gradients, like the nozzle wall, shock region, and shear layer. A fully resolved boundary layer is usually employed with the first grid point at the wall typically having a y+ less than one. This is a critical requirement. As temperature and pressure change abruptly in the plume boundary, using low-resolution wall function grids fail to predict the wall heat flux accurately.

A finer grid point placement is done in the axial direction to capture the birth and early growth of the shear layer and shock cell structure. Inside the divergent part, axial point distribution is concentrated in the two zones, one at the separation shock region and the other at the Mach disc region. The locations of these zones vary with the operating conditions and are shifted accordingly. When the pressure ratio is increased, the separation shock and the Mach disc moves downstream. So, relative to the pressure ratio for which computations are made, the densified regions need to be relocated. Figure 5 shows such a flow physics conscious grid generated for a pressure ratio, where the separation shock and the Mach disc are positioned near the nozzle exit.

Video 1: Structured multiblock mesh generation for a rocket engine nozzle using GridPro.

Domain Size and Typical Grid Density

For nozzle computations, the nozzle throat radius (Rt) is used as reference length and the domain size is calculated relative to it. Typically, the outlet is kept at 80-90 Rt downstream of the nozzle exit, while radially the farfield domain is placed at 70-80 Rt from the nozzle central line.

For a baseline grid, typically 300*100 grid points are used to discretize the flow domain inside the nozzle covering the chamber, throat, and divergent part. Outside the nozzle also, a similar grid size of 300*100 amounting to 30,000 is used. These are typical numbers for a baseline grid and refinements as specified in the above paragraphs to capture flow separation and Mach disks are added on top of this.

Important Aspects to Take into Consideration While Meshing

1. Accurate capturing of the nozzle exit lip with fine mesh is essential, as there will be a small amount of flow entrainment from the outside external flow into the nozzle, which also influences the flow structure inside the nozzle. Also, usually, small vortices sit near the nozzle lip as shown in Figure 6. A dense grid around the nozzle exit lip will help in capturing these subtle flow physics.

**Figure 6:** Flow separation vortices and external flow entrapment near the nozzle lip. Image source – Ref [6].

2. Grid should be refined outside the nozzle exit also, at least for 3-4 times the length of the divergent part of the nozzle.

**Figure 7:** Refined grid beyond the nozzle exit.

3. The domain size and refinement region are relative to the pressure ratio for which computations are made. The above values are good when most of the dominant flow physics like shock, Mach disc extra are inside or just outside the divergent portion of the nozzle within one or two times divergent length.

But the plume dimensions change with altitude. At high altitudes where under-expansion happens, the plume becomes bigger and bigger as seen in Figure 8 below. In such cases, the domain and grid refinement region need to be extended.

**Figure 8:** Change in plume size with altitude for rocket engine nozzles. Image source – Ref [1].

Comparison of Results Obtained from Structured and Unstructured Grids

Published data points to the fact that CFD does better prediction with structured grids than with unstructured grids for rocket nozzles, both in terms of flow feature capturing and solution accuracy. Nozzle shocks appear sharper in the contours of structured grids than those on unstructured grids. Also, the structured grids on the 2D-axisymmetric case and full 3D nozzle case predict better axial-thrust performance than those on unstructured counterparts.

**Figure 9:** Mach contours on adapted grids for rocket engine nozzles. a. Unstructured grid. b. Structured dominant grid. Image source – Ref [5].

It is observed that computed specific impulses on unstructured grids are consistently predicted lower than those with structured grids. This is probably due to grid density and edge alignment. A NASA paper published in the Journal of Propulsion and Power reports that even when the unstructured grids have double the total cell count, the effective grid density tends to be lower than that for a structured grid. Further, the author says that the accuracy of two tetrahedral cells is approximately equivalent to that of one hexagonal cell. So, the increased cell count just makes the runs computationally expensive without bringing in the benefit of increased solution accuracy, negating the primary reason for going with increased cell count in the first place.

These observations hint that structured grids are more favorable both with respect to accuracy and computational efficiency for such cases which have high gradient flow physics.

Parting Thoughts

Flow physics changes with pressure ratio in bell nozzles. Meshing in tune with the possible flow phenomena developing helps in generating an optimal grid with fewer iterations. With the prevalence of high gradients, the CFD codes are more susceptible to blow-ups if the right kind of grid with optimal grid density is not generated.

The gridding suggestions presented in the article can be a good starting point to generate a mesh for rocket nozzles. Tools in GridPro like the auto core generation helps to rapidly build an axis-aligned topology with less effort and powerful tools like enrichment and nesting can help in doing local refinement as per need.

One simple approach can be, to get a baseline structured grid with the auto-core tool, and later depending upon the pressure-ratio the computations planned, local refinement can be made using enrichment and nesting. In this way, an optimal grid can be generated, tailor-made to that pressure ratio with less effort.