CFD simulation of complex rotor equipment using FloEFD: Part IV – KJ-66 Micro Gas Turbine


...Published 2016-08-31


KJ-66
This blog discusses using FloEFD to predict the thrust produced by the KJ-66 micro gas turbine engine, popular among hobbiests for use in remote controlled jet aircraft. This little engine is capable of producing 75N of sustainable thrust at Max. 117,000RPM. This particular CAD model used for these simulations was obtained from www.GrabCAD.com [1].
In Parts I – III of this series we demonstrated the ease use of FloEFD to perform CFD simulations of rotating equipment using the sliding mesh approach. In this blog article we will apply another rotating approach called Averaging Rotation also available in FloEFD. The averaging approach is limited in it’s application as the flow parameters are circumferentially averaged around the volume defined as the rotating region. This approach therefore limits it’s use to purely axisymmetric bodies of rotation where there is little or no interaction between the rotor and surrounding stators or other geometries. So, naturally it is specifically useful for pumps, fans, compressors and turbines. [Take a look at Part V] for an example where such interaction is strong necessitating the sliding mesh rotation approach. The averaging approach is particularly useful for gas turbine engines like the one in question, which involves rotation of both the compressor and turbine in the same model and consequently tend to become computationally expensive, since the averaging approach can be used in stead-state analyses that can be solved in shorter time.
Since the KJ-66 engine is so popular and the performance is well known, it is a fitting model to conduct CFD simulations on in order to compare the CFD-predicted results with published performance data. This author was specifically inspired to attempt such a simulation after first reading an article entitled “Small but mighty powerful” in the Engineering Edge magazine, Vol 1, Issue 1 (2013) published by Mentor Graphics [2]. In that article the authors demonstrate how FloEFD can produce very accurate thrust predictions up to 80,000RPM with really course meshes, with slight deviation (< 10%) at 100,000RPM. So off I went and got hold of a KJ-66 micro gas turbine engine CAD model from www.GrabCAD.com and started setting up my own simulation in FloEFD to see if I could get the same results.
Lo and behold…Below follows a description of the analysis setup.
An internal analysis with averaging rotation and combustion of Kerosene as the fuel and air as oxidiser was setup. Since combustion was included a transient analysis was required. The performance graph in the operator manual[1] was generated at 1.013bar and 8°C. Accordingly, an inlet total pressure of 101.325kPa and outlet static pressure of 101.325kPa was prescribed as illustrated in Figure 1. It is assumed the performance data was generated by mounting the engine on a test bench, thus there is no relative velocity from the engine to the surrounding air. The rotating region components for the compressor and turbine are also highlighted in Figure 1. The angular speeds analysed were 40 000, 80 000 & 100 000RPM. The ignition is modeled by applying a high temperature i.e. greater than the fuel ignition temperature to a volume between the sparkplug tips, as illustrated in Figure 2, for only a brief moment (0.01s) before switching it off to let the combustion sustain itself.

BCs+RRs

Figure 1: Inlet and outlet boundary conditions with compressor and turbine rotating regions.

Combustion

Figure 2: Fuel injector inlets and spark plug ignition source.

A relatively course mesh of approximately 660,000 cells was used for the 40,000-80,000 RPM models as presented in the figure below. The mesh was refined slightly for the 100,000 RPM model to account for the increased velocities. The time step size was 0.0001s and 0.00005s respectively. The analyses were run for about 0.3-0.5 seconds of physical time until a steady state was reached. The results from the analyses are presented hereafter.

MeshSide

Figure 3: Mesh resolution – Side view.

MeshFront

Figure 4: Mesh resolution – Compressor and turbine cross-sections.

Results:
After solving for about 12 – 24 hours on a 16 core PC depending on the angular velocity, time step and physical time solved for, the results were collected and found to be quite astonishing, take a look at the comparisons below. The mass flow rates and velocities required to calculate the thrust are tabulated below. Since we use an average velocity across the inlet and outlet openings, we need to correct for the velocity profile which is not uniform and hence the average velocity is not an exact representation of the momentum flux. A momentum flux correction factor, denoted by β, is applied to account for the velocity profile. For laminar internal flow the velocity profile across a duct is parabolic and a correction factor β = 1.33 applies. For turbulent internal flow the velocity profile (time-averaged) across a duct is much closer to a uniform distribution as illustrated at the outlet of our turbine below and the correction factor ranges from β = 1.01 to β = 1.04. These factors are generally ignored for turbulent flows, but they do increase the accuracy of our calculations as shown in the table below where we report the thrust predicted both without any correction, β = 1.0 and with a correction of β = 1.04. The thrust is calculated as in the equation below.
Thrust = (βm ̇V_avg )_out – (βm ̇V_avg )_in
When we plot the mass flow rates predicted from this study to those of Mentor Graphics in their study, we see very good correlations with the expected typical mass flow rates, giving us confidence that our modelling approach was acceptable, see Figure 5 below. But what is even more impressive is when we compare the thrust predicted (including the correction factor) to the performance graph from the operator manual as in Figure 6 below.

Mass flow comparison

Figure 5: Mass flow rates comparison [2].

Thrust comparison

Figure 6: Thrust comparison [1].

This blog article is Part IV of a series of blog articles on the CFD simulation of complex rotor equipment.
Part I: LEGO Technic Aero Hawk
Part II: Apache Helicopter
Part III: Rotating Radar Dish
Part IV: KJ-66 Micro Gas Turbine Thrust Prediction
Part V: Diffusor Shock Waves in a Centrifugal Compressor

References:

[1] www.grabcad.com.

[2] “Small but mighty powerful”, Engineering Edge magazine, Vol 1, Issue 1 (2013), Mentor Graphics Corporation.


4 thoughts on “CFD simulation of complex rotor equipment using FloEFD: Part IV – KJ-66 Micro Gas Turbine

  1. Maxwell Song

    Hi, i tried to perform the same simulation under Floefd/Solid edge. However some of the models I found from grabcad has errors. May I know which model have you used? or if you have manually modified a model do you mind share it to me? I am currently undergoing an important project and the model has been a headache for me.

    Thanks !

    Reply
  2. Maxwell Song

    Hi, may I know which model did you use from GrabCAD?

    The models I found are not properly sealed, and I am still unable to perform internal simulation even after manually trying to fix them. May I know if its possible for you to share me the one that you have fixed or the one you found for this simulation you did? I am now undergoing a very important project.

    Thanks so much !

    Reply

Leave a Reply