Using Outlet and Inlet Boundary Conditions
 

Hey All,
Can't seem to figure out how I'm supposed to do this simulation. Currently using ANSYS CFX 15 and what I want to do is to take a simulation (which has been split up into parts to make it manageable) and run it with Cartesian velocity components for the initial run through, then use the outlet boundary conditions as inlet boundary conditions for the next iteration of the simulation. This process of using outlet as inlet will repeat somewhere between 3 and 5 times as required until I get stabilised flow/measurements.

I have done this in the past by solving the first one, opening up post, exporting boundary conditions to an excel type file, then importing that file as a boundary condition initialisation to a copy of the original cfx module and running that simulation then repeating as required. This process was very labor intensive and yeah not very efficient.

Is it possible to set something up so this happens automatically?

A seperate question then follows: Is it possible to setup a plane in the middle of my domain and use this to grab my boundary condition data? Obviously I'd have to run more simulations but a mate did tell me that this would put less restrictions on the flow conditions as compared to when you take the data from an opening (used as an outlet) which will affect the final result. Or is what he was saying wrong/not worth worrying about?

Thanks in advance
Tyler

Thanks for the link Hemen but given that this is part of my undergraduate thesis, somehow I don't think I'll be able to use/afford your services.

Can you post an image of what you are doing? I cannot think of a reason why you would do what you are suggesting.

And why is the normal translational periodic boundary not appropriate? That is the normal way to do simulations like what you describe.

http://i44.tinypic.com/2vwhd04.png

Its modelling a train with a crosswind (modelling straight into the wind is easy and much faster given that all you need is a symmetry model of the same thing).

That is exactly what I need and I didn't know you could do translational periodic boundaries. Would I be right in saying that this will effectively do the same thing and give me the end "solved" result without having to iterate?

How do you set it up to do this as well. I can work out how to setup the translational periodic boundary but it gives errors saying you've specified certain boundaries for multiple things. Once I remove the old "inlet/outlet" I no longer have an inlet as such to allow the air in. I'm assuming that in this case, I'd need to run the initial inlet/outlet simulation once, then use the domain initialisation with the periodic boundaries to iterate to get my solution. Is this right?

Thanks

You do not need the inlet or outlet, so remove them.

The translational periodic boundary can drive the flow either by specifying a pressure drop or a mass flow rate. And yes, you will not need to "iterate" to a flow rate like you described before.

Nice model by the way.

Thanks again for replying so quickly.

Just tried it and got it to work, but (and I didn't realise this) the way I have the model setup, is such that the main "inlet" and "outlet" are parallel to the XY plane. This wouldn't be a problem, but because I'm looking at crosswinds (at multiple angles) it doesn't let me specify that the flow has to be at a specified angle angle. See below

http://i58.tinypic.com/2i7oizk.png

The top boundary shown is the "inlet", the left is the smaller inlet which is actually setup as an inlet with the wind travelling at a specified speed and angle. The right is an opening and the bottom is the "outlet". With the original design, the inlet and smaller inlets were set at a particular velocity (still possible given that I can control mass flow rate) but also at a specific angle (which I will be making a parameter once its all setup). When I change the "inlet" and "outlet" to translation periodic, I can no longer specify the angle. The way I see it, I have two options as potential solutions (I'm not entirely sure if either will work for what I want).

1. Leave domain the same, use and inlet and outlet initially and then use domain initialisation with the periodic boundaries to continue the simulation
2. Adjust the domain such that the "inlet" and "outlet" are angled at the angle that I want to test and run the periodic boundaries. The second inlet will also be converted to an opening/wall. I am 80% sure this will work however if I can avoid having to have the thing remesh every time I want to run a different angle, that would be good.

Any thoughts or suggestions?

Before I answer your question I am puzzled by what you are trying to do.

If you use the translational periodic boundaries for this you are, in effect not only modelling an infinitely long train, but also modelling an infinite number of these trains running next to each other with a spacing of about 50m (based on your domain size).

Is this really what you are trying to model? Or are you trying to model just a single train in a far field condition (ie nothing else around except the ground)?

Infinitely long train in far field with only the ground to measure the drag on a single wagon. Then reiterate with various designs to see what effect different designs have to reduce the drag.

I thought so.

In that case the solution is simple. The left side is an inlet with the wind specified at whatever angle you wish to model, the front and back are a translational periodic pair and the right side is either an outlet or an opening. Obviously the bottom is the ground and the top is whatever you model the far-field sky as (slip wall, symmetry, opening).