Transient test for intake
I am currently using star to design a manifold for a single cylinder ATV engine, and I would like to be able to set up my outlet pressure as either a function of time, or to vary with a table. I have tried an implicit unsteady simulation with a cosine function at the pressure outlet, and with a table of time vs pressure values.
With the cosine function the mass flow dropped consistently for the first few time steps as pressure increased, which was the opposite of what I expected to happen. Then, after the first 3 time steps the mass flow would level off and not change any more.
Is the implicit unsteady with a field function the proper way to test the effect of the variation in pressure waves throughout the intake, or is there a better way to test this? Also, is there an easy way to animate the velocity vector field for a test like this, or will I be better off to set up an autosave at each time step?
Anyway, for me it sounds like a guy at a garage, talking to a car mechanic:
"My car makes a strange noise, what's wrong?" And the mechanic still doesn't know whether it's the gear box, the engine, the wheels, the brakes, the front-seat passenger or only the HiFi system which makes the strange noise.
So can you please give us some more information? Do you run compressible or incompressible? What about your time step size, is it reasonable? Have you double checked your field function? Create a report and monitor the value provided by the field function as time advances. Will it give a reasonable value for all time? How much does your mass flow rate drop? 1%? 10%? 10 000%? After how many time steps did you decide the mass flow levels off? 10 time steps? 10 billion time steps? etc...
To see the effect of pressure waves, you have to run it unsteady and compressible. There is no better way (except maybe some 1D codes like power GT or something similar). To set the outlet condition with a field function is fine. It is one of several common ways.
For your animation, it might be possible to hardcopy the scene every time step and put together an animation with an external program (like windows movie maker, virtualdub or any other programm of your preference). To set up an autosave every time step has one big advantage: You can access the data of every time step after the run. But it has a huge disadvantage: You can completely fill your harddisk within a few timesteps, as the amount of data can reach incredible high values! Have you ever thought about this? And although it's possible, it's not very convenient to access the stored data as you would have to open every saved sim-file seperately.
So my advice: Hardcopy the scenes
What I meant to say was that the pressure drop increases, ie goes from -5000pa to -10000pa. I had some problems in my time steps and the syntax of my field function, which were giving me the issues. Your post helped out tremendously with finding the little mistakes in my setup. My models are set up as Implicit unsteady, Turbulent, K-epsilon turbulence, Coupled flow, ideal gas.
My only other issue is that I am having trouble with getting my solutions to converge on the more complex 3D cases in steady state. I have tried changing the under-relaxation factors for K-Epsilon Turbulence, and K-Epsilon turbulence viscosity, as well as changing the turbulence intensity wherever possible, and attempting to set reasonable initial conditions. Are there any other factors that I could try and change so that my simulations will converge? I have used 0.3 for the relaxation factor for K-Epsilon turbulence, and 0.4 for K-Epsilon turbulent viscosity, and changed the turbulence intensity to 0.1. Are these values reasonable?
I have also been able to make the simulations work if I do a 2D planar view of the geometry. Would it be acceptable to use a 2D simulation in order to compare geometry in a more time efficient manner?
The most important question is: How do you judge convergence or not-convergence of your simulation? Don't look only at the residuals, also monitor some engineering data, like pressure drop, mass flow, velocities etc.
When running steady state and the simulation doesn't converge, no matter what you are doing, it might be due to an unsteady nature of the flow. There might be some vortices or some oscillation of the flow. In this case, average your data over some iterations (and accept a more or less significant error) or run unsteady.
When it's neccessary to change the urf for turbulence, it's likeley to be neccessary to change urf for velocity and pressure as well. But first check the nature of the flow, when it's unsteady, you will NEVER get a "converged" solution when running steady. And my maxim is: When it's neccessary to reduce urf to very low values when using only standard models (e.g. no Eulerian multiphase etc.), something is wrong with the simulation. A slight reduction of urf is okay. A heavy reduction is just a try to cure some symptoms of a messed simulation. Find the reason for the problems instead, that's more efficient.
Turbulence intensity of 0.1 doesn't sound too bad. That's a common assumtion, it shouldn't mess up your simulation.
I can't judge wheter running in 2D is reasonable or not. It depends on your geometry.
For example, running an airfoil in 2D is a good option to compare different airfoils, as the flow on a stretched wing (ideal case would be an infinite wing) is nearly 2-dimensional. It would be no good choice on a car, as the nature of the flow is highly 3-dimensional (a car is nearly as high as wide). So you have to post a picture of your geometry or judge on your own if the flow in your manifold is more or less 2-dimensional.
When not, maybe you can check for symmetry planes and run ony a half model?
|All times are GMT -4. The time now is 02:02.|