Dear all,

I am trying to run a 2D simulation of flow past a moving heart valve, using a 2D unstructured compressible FV solver. The problem set-up basically consists of a straight channel containing the moving valve. At the inlet I impose the velocity components and the temperature, while at the outlet I impose the pressure. However I am experiencing problems with reversed flow at the outlet (the problem remains even if the length of the outlet is increased). How do I define the boundary conditions at the outlet in this case?

In addition, the magnitude of the specified velocity at the inlet varies with time and at a certain period in the simulation is negative (i.e. flow out of the domain at the inlet). How do I deal with the boundary conditions at the inlet in this case?

I would be grateful if you could point me in the direction of any references which may help with this subject.

Kind Regards

Neil Forsythe

I have a colleague who faced similar problems in his simulation of aortic blood flow. At inlet his velocity is a function of time and flow goes out of domain at inlet for some period. The negative flow at outlet just indicates that your simulation is conserving mass flow rate and nothing more. An explicit method (for time) reduces this problem but does not eliminate it. But time taken for explicit method is too much. The point: As long as your outlet boundary is away from your region of interest, do not worry.

Thanks for your help on this matter

Neil

I would worry about both boundaries, out of principle, regardless how far away they are from the valve. In internal flow you cannot simply remove the boundary from the domain and then expect that everything is going to be fine. This is a priviledge of external flow problems. I cannot stress enough that the correct treatment of boundaries is very important in internal flow problems, be it blood flow through a valve or air flow through a turbine.

It seems obvious that neither of your in/out boundary conditions is actually satisfied. The reverse flow at the inlet surely contradicts the velocity you specified. Usually, we do not prescribe the velocity itself, but instead use total pressure, total temperature and the direction of the velocity (flow angles).

At the outlet, the reverse velocity again contradicts your boundary condition. Prescribing only pressure, you basically assume only one characteristic entering the domain. However, this is not the case if you have reversed flow. However far you move the boundary, the condition is still wrong, the mass flow may be wrong and your result meaningless, as it may not even converge. Not only that, but the position of your boundary will naturally affect the solution if you simply prescribe the pressure, even if the boundary condition was correct and there was no reverse flow.

In general: The most appropriate way to deal with this problem is to use characteristic boundary conditions. You may check if such method is available with your software. If you are writing the boundary conditions yourself, or if you would like to know more about it, look up Mike Giles on google. His approach (and others') is pretty much standard in internal flow computations. I would be surprised if your (commercial?) code didn't have the option of characteristic (or non-reflecting) boundary conditions.

Good luck.

I know the problem of reversal flow at pressure outlet boundaries in compressible flows. I am not expecting that blood could be compressible, but perhaps the same tricks works: - Use "total pressure" instead of "static pressure" as outlet boundaries. - set up your initial pressure a little bit higher than the pressure boundaries. So the flow is forced ourwards. So you can get a good start of the run for transient calculations to. The calculation don't need so much time to get a the real time dependend results. - problems in inlet boundaries can be handeled with stagnation boundaries and transmassive boundaries.

All this you can read on http://www.adapco-online.com, than "feature arcticles" -> "compressible flow".

Hubert,

how can the total pressure at the outlet be obtained a priori? It's often not available from experiments (unlike the "ambient" static pressure), and is probably one of the parameters to be determined by the CFD calculation. With zero flow losses and zero work its identical to the inlet total pressure, but neither is generally the case.

The stagnation boundary described on the cd-adapco site is meant to be used for the inlet only, not for the outlet.

Mani, Hubert

Thanks for your contributions

To clarify a few points about my original message, reverse flow occurs at the inlet because I want to impose it there (it is a pulsatile inlet condition where the velocity is negative for a portion of the flow pulse)

The code I am using is an in-house code, so unfortunately doesn't have the option of applying characteristic boundary conditions. Would the characteristic boundary conditions allow reverse flow at both the inlet and the outlet to take place without the need for specifying any other variables at either of these boundaries?

Neil

Are you using a compressible code or an incompressible code? You have called it compressible but this would be unusual. If compressible what do you do about acoustic waves and resolving/controlling them? Is this the first attempt at a very low Mach number flow with the code?

Before determining appropriate boundary conditions it is necessary to know what form of the fluid equations are being solved. Compressible flow and incompressible require different boundary conditions. The latter should be relatively straightforward for the problem you describe, the former probably very difficult but would depend on the details of the code.

Andy,

It is a compressible code which I am using, as I don't have access to an incompressible code which has all the functionality I need (ALE, local remeshing). When running the test case, the temperature was lowered to "artificially" increase the mach number back to within the compressible range, thus avoiding the problems associated with running the compressible code a low Mach number.

Neil

OK so it is definitely a compressible code. You need to apply appropriate time dependent compressible boundary conditions. Someone mentioned Mike Giles' approach but this:

Kevin Thompson, ``Time-Dependent Boundary Conditions for Hyperbolic Systems, II'', J. Comp. Phys., 89, 439-461 (1990)

T. J. Poinsot and S. K. Lele, ``Boundary Conditions for Direct Simulations of Compressible Viscous Flows'', J. Comp. Phys., 101, 104-129 (1992)

is probably simpler to work with in your case with the flow going every which way and your need to chop and change between which variables are specified and which determined from within the solution as the flow reverses.

Unsteady compressible boundary conditions are not straightforward and the only practical way of getting round it is to move the boundary a long way from where things are changing and set a simple robust condition like a specified upstream total pressure + flow angle and a downstream static pressure. You will then have problems with acoustic waves but, in your case, you should be able to add a kludge to damp them since the details of the thermodynamic state is wrong anyway.

> (it is a pulsatile inlet condition where the velocity > is negative for a portion of the flow pulse)

I see. So your inlet condition is quite complex. It might still be better to provide unsteady total pressure and total temperature variations instead of prescribing the velocities. It often helps to think what you would do in an experiment (i.e. in the real world), and then emulate that with CFD. It is very hard to impose a certain mass flow directly. What you would rather do is to provide a plenum with a given total pressure fluctuation and let the pulsating mass flow develop itself. You can control the pressure fluctuation to achieve the velocities that you need. I would keep that in mind as an alternative to what you are doing right now.

>The code I am using is an in-house code

That's actually good news! So you can implement any boundary condition you like.

A characteristic boundary condition (like the one by Giles or any other that was suggested in another reply) in principle can take care of any situation. However, the number (and type) of variables that you need to impose from outside the boundary very much depends on the direction of the flow (inside/outside the domain). There is unfortunately no remedy for this basic principle, because it's strongly connected to the nature of the hyperbolic equations. That's why I was trying to say: Prescribing only pressure at the outlet is not sufficient for the locations where you get reverse flow. You understand that reverse flow at the outlet is actually "inlet" and must be treated as such. (Likewise, reverse flow at the inlet is really "outlet".) That poses a problem when most variables at the outlet are simply not known.

A lot of people would suggest to move your boundary away from trouble. However, if you do that you have to be aware that your boundary condition (e.g. the exit pressure) should change accordingly. For example if you were to extend the downstream tube, you would most likely need to apply a different pressure, in order to achieve the correct pressure at the original exit position. It's possible to do that in the hope that further downstream you will not have reverse flow and your boundary condition becomes simpler. Basically, what you are doing is to provide an arbitrary extension to your domain in order to simplify your boundary, while retaining control over the pressure at the original boundary position.

You see that this practice is kind of arbitrary, especially concerning the extended geometry and the flow direction, acceleration and so on, which you will impose aside from the pressure, depending on that arbitrary geometry. Nevertheless, somebody might prefer this quick fix to get any solution at all. I would generally not recommend it, unless you know exactly what you're doing and you have no alternative.

Mani:

Yes, that's a point, you are right when you don't have the stat. pressure at the outflow boundary, but you must have any information about the pressure in your domain. You can switch the inflow boundary to pressure and the outflow to massflow (or Velocity), but this is numerically very unstable. One death you must die.

I think I don't understand you right: When you know the static pressure you will know the total pressure (roughly) too, because you have information about flow cross section density temperature (roughly is good enough), and massflow. So you can calculate the dynamic pressure 1/2 dens v².

There is somthing more with the total pressure boundary, but I am currently not sure to explain it right. Read the artical for compressible flows on www.adapco-online.com.

Yes stagnation boundry is for inlet, but you have described problems with inflow boundries.

Yes, at the inlet, stagnation BCs are pretty much standard procedure at least in compressible flow. I misunderstood you as trying to use it for the outlet, where you often do not know total pressure, density, temperature or anything else than the static pressure.

I think the key point in this problem of "reversed" flow is really to understand the meaning of "inflow" and "outflow" and applying the appropriate boundary conditions locally, for each grid cell.