[JohnAB]

Hello,

I am simulating a water flow around a wing-type profile. I am comparing two cases:
- static wing with inlet-oulet flow, speed V.
- moving wing at speed V in static water.

First, based on your experience, could anyone give me what differences I should expect from those two simulations ?
I am trying to evaluate how accurate it is to simulate a real life moving body by a simulation of a fixed body in a moving flow. I already expect some boundary layer differences, am I right ?

Second, is there a way ton input an acceleration to my velocity inlet instead of a full speed from the beginning ?
same thing, can I have my moving overset mesh accelerating gently to full speed ?

Thank you very much!

[me3840]

There shouldn't be any difference between the two, you're just changing the frame of reference.

[JohnAB]

I still could not find how to easily input an acceleration/velocity profile at my inlet, do you know what the best way to do that is ?

thanks!

[me3840]

You can ramp it over some number of iterations with a field function if you want. Something like:

($Iteration<100)?$freestreamVelocity*$Iteration/100:$freestreamVelocity

[JohnAB]

Thanks a lot!

Is there a Help somewhere on the different variables I can use ? I am not why what I should put instead of "freestreamVelocity"...
I just want to ramp up Vx, so I set Vy and Vz to constant and equal to zero, I set Vx to fieldfunction and linked it to this field function, but not sure about what is next...

Besides, if I am using VOF model (Flatwave) because of the boundary reflection damping option, is this going to work or is the acceleration already defined by this model ?

So say I want to ramp up from 0m/s to Xm/s, should I set all initial conditions (under physics and then under regions) to 0m/s, then set the filedfunction to my inlet under regions, and then, in physics, let VOF Flatwave with Xm/s in Current ?

That is a lot of questions, but I tried a lot of combinations already and it does not accelerate nicely...

[me3840]

I said $freeStreamVelocity - this would be an additional field function you make up, which is just a constant value. When I make field functions that have inputs, I usually separate the inputs as separate field functions, that way it's very easy to change the value.

Acceleration is not really defined in CFD, the velocities are what is computed.

I'm not too familiar with the VOF flatwave, however setting the amplitude of the wave should be very similar to setting the inlet velocity with a field function.

What do you mean by accelerate nicely? It is not converging? It blows up? What are your engineering values of interest?

For VOF be sure your grid is fine enough to resolve the fluid/gas interface well, and also be sure to control your timestep such that the courant number on the interface doesn't get too high.

All of the names of the field functions can be viewed. If you go under tools>field functions and click on any function, it will have a property that contains its name to reference from any other function or report.

[JohnAB]

me3840,

thanks for the info on the additional field function, I will work on that.

What I mean by accelerate nicely is just that using VOF (I do not want any wave at input, only the water current and the air flow above it, as well as the wall reflection damping option, that is why I use VOF) I am not able to ramp the speed up to a constant value, it seems like it still wants to create a wave (even if I use the field function and 0m/s inital value, it goes from 0m/s to wave speed right away, it does not accelerate slowly to the wave speed) and use the velocity of the wave, so my acceleration would be the one of the wave, and not the ramp I want.

Basically, I have a wing partially submerged and I want to see the evolution of drag and other loads when going from 0m/s to constant speed, but I need to know the loads during the acceleration phase as well since they might be (or not) higher than the steady state value.

The grid is good, the courant number too, I spent a lot of time on that and I am now happy with my values, I have good results when steady state. Transient is the problem.

Let's say, to start simple, I forget about VOF model and do not use it. Here is the situation:

I have to fill:
- initial velocity in the physics model: 0 m/s
- initial velocity in the velocity inlet boundary: 0 m/s
- velocity at the inlet boundary: field function (actually constants = 0 along y ans z, and field function along x) you suggested.

and now for the water depth/surface, I use the field function I had when not using VOF (this one works, this is a very easy one).

Am I right so far ? I will try that and let you know, thanks!

[me3840]

Quick note, if you are doing transient, you will want to ramp the field function with $Time, not $Iteration. You will then, of course, have to set some sort of time that you ramp over.

[JohnAB]

Alright, so I got that to work and I just realized I now have a new problem:

since I apply this ramp up to my inlet (my geometry is a simple channel, with inlet, outlet, and side walls) and since the initial condition is a condition of rest (all speeds = 0m/s) this is not completely working like I would want yet: it justs create a pressure/wave at inlet since the rest of the water still is at rest.

What I want is the whole body of water ramping up from 0m/s to my final speed at the same time, not only the inlet. I want to simulate a body accelerating in the fixed channel (but instead, I make the water moving around the fixed body and channel), so I need not only the inlet, but every cell between inlet and outlet to undergo the same ramp up.

Do you know how I could make this work ?

thanks a lot!

[JohnAB]

I should probably go with the inlet and outlet flow rates, right ?
I am just worried the middle of the channel would still not move at the same speed as the boundaries and this will still generate waves and will not reproduce the motion of a moving body in a fixed channel...

[me3840]

I don't think what you want to do is very physical. I could be wrong, but in a water tunnel, there should be a pressure wave that propagates as the water moves from rest to in motion.

If you're interested in seeing if the drag is larger at this stage than at steady state, I would argue how much value there really is in that - the velocity is so low it's for sure going to be lower than the steady-state value.

You can get the pressure wave to move away some by making the domain bigger and allowing it to dissipate. You might even think about making your initial timestep large to smear out the wave. But I don't think there's any way of getting rid of it; the physics demand its presence.

[JohnAB]

thanks for your answer, I agree with you, I am just trying to find a way to represent a body that would move from rest to steady state translation in a channel where there is no water current. I want to avoid doing Overset meshing and moving body, so I was thinking there might be a way to do that just by having a fixed body and by playing on the water flow.

Say you have a boat, you want to see the bow and kelvin waves generated by that boat when it accelerates from 0 to a steady translation, how do you do that without using a moving body situation in starccm ?

[me3840]

Oh, I see what you're saying. While it's true the simulations are the same from the steady point of view I don't think they are when accelerating. Sorry, somehow I got the original question mixed up in this.

Yes, I think the only method of doing this is by moving the body. Fortunately you don't need to actually move the object or use overset. You can move the whole region.

There's a VOF wave called a flat wave you can use to simulate the position of the water. Then all you have to do is move the region across it with a motion. So there's no overset motion, and there's no real sliding mesh in the conventional sense. You're just moving the whole domain. Does that make sense?

[JohnAB]

Yes it does make sense, but the VOF flat wave is what I have tried at the beginning, but couldn't get the acceleration part working.
VOF flat wave asks for water current and air current in its properties, but it does not seems like I can put a velocity ramp up there, only the steady state value (I have used this model for steady state, and it works well). So then, where can I put my velocity ramp ? If I put it at inlet, I will end up with the same problem, only the inlet will ramp up, not the whole region. I did not find where to tell the flat wave to ramp up yet..

[me3840]

No, you will leave the flat wave as zero always.

You will be moving the domain through the flat wave. Your velocity ramp will be on the motion for the region.

[JohnAB]

Got it, thanks! I will try that.
I will probably find out by testing, but the face that used to be my velocity inlet it still the velocity inlet with the same ramp up than the one that moves the whole region, so that the inlet now acts just like a free flow face ?

[me3840]

The outer BCs are a good question. I would probably start with pressure outlet and prescribe the pressure to match the hydrostatic pressure.

[JohnAB]

I am still figuring this out, I will let you know when I get it to work, but thanks a lot!

I am also trying the moving mesh (overset) because I want to see what will happen at both ends of my domain. I am having the same kind of issue there:

I want my body to start from a 0m/s velocity, then reach steady state motion, then decelerate to 0m/s. Simple translation along x-axis, nothing more.

A simple field function like the one you gave me above should do it ? How do I then add the deceleration part ?
I am sorry it may sound super easy to do but it still have trouble to make it work.. is there a manual for the field function language ? There is nothing about that in the Starccm+ help...

Thanks a lot!