[Trev0r]

Hey everyone, this is my first post so I'll try to be as concise as possible for you but I apologise if it's a bit long winded as I'm not too sure what to include so you can help out.

I'm trying to model artery bifurcations using idealised geometries and so far the simulation is steady state with rigid walls and I have prescribed a fully developed parabolic velocity profile at the inlet using a CEL expression. I'm going to be adding progressively more complexity (transient inlet flow waveforms and non-Newtonian viscosity models) to the model to make it more representative but for now I've hit a snag in describing the outlet boundary conditions.

In general the outlet static pressures can be treated as linear functions of the flow rates through them (accounting for the resistance of the arteries downstream and outside the domain of the simulation). I tried to model this using the following CEL expressions applied to the pressure outlets:

Pressure1=resistance1*areaInt_z_Coord1(w)@Outlet1
Pressure2=resistance2*areaInt_z_Coord2(w)@Outlet2

resistance1 and resistance2 are predefined constants. Coord1 and Coord2 are local coordinate systems centred at the outlet faces with the z axes perpendicular to them. Basically static pressure=resistance*flowrate

I set up monitors to watch these expressions converge during the solution process. I'm under the impression that at the end of each iteration the static pressures at the outlets are recalculated according to these formulas and updated ready for the next iteration. However it quickly became apparent that the values for static pressure at the outlets in the converging and converged solution do not equal the flow rate x resistance like in equations I set above.

In fact checking the flow rate through the outlets with the function calculator in CFD post and then multiplying that value by the predefined resistance that I set gives a vastly different static pressure to the one CFD post is reporting in the solution???

For example in one trial run shown in the attachments i've provided I set both resistances to and the resultant flow rates through outlet1 and outlet2 were converged at and respectively. This should have therefore resulted in the static pressures at the outlets being and . The actual static pressures reported at the outlets in CFD post are and . When I evaluate my two expressions in CFD post they give me the values I expect yet these are not the values applied to the outlets?

In summary my outlet CEL expressions are having an affect on the outlet pressures but they are not behaving as expected. Does anybody have any idea what I am doing wrong and why my static pressures at the outlets do not equal the values set in my expressions?

Many thanks

Trev0r

[Trev0r]

I've actually solved this now, I needed to integrate the global velocity components v over outlet1 and u over outlet2 instead of w. I thought using the local coordinate system with z normal to the outlets changed the definition of the velocity componets but global velocity components, not local ones must be used.

[PranjalNewton]

Hi there, Did you try the transient formulation? I've been trying to apply pressure as function of previous pressure and flow rate. I've been trying to do this through UDFs in fluent but after a long time, I finally came to know CFX can also do FSI simulation. Can you please suggest a way to get values of a variable at previous time step? I know that CFX only keeps current value so there has to be a file i/o method.

Please help. Thanks.

[stumpy]

Why do you need the pressure at the previous timestep? Are you calculating dP/dt? If so, just ask for Pressure.Time Derivative in your CFX expressions.
If you really do need to old pressure, there's a hack you can use. Search this forum for "Update Loop = TRANS_LOOP".

[PranjalNewton]

I tried that but I'm getting errors. SO, instead of solving for the differential equation, I did backward discretization so that I just need these values. I did that by UPDATE_LOOP command through same process you discribed. The Multifield solver just doesn't run giving an error code zero. (Note that I've gone through the CFX-ANSYS Training. I've taken all the necessary considerations I could.)

A major question that I have, which experienced person like yourself might answer is: Is it possible that some approximation like newtonian fluid or medium mesh may result in solver not even solving? As far as I know, you just obtain an unrealistic result.

[stumpy]

Error code zero doesn't mean too much. What's in the CFX and MAPDL log files before that error?

[PranjalNewton]

I got it! I was getting a back flow at outlet. I modeled it as 'outlet' rather than 'Opening'. After all the studies into solver stability and Theory Guides, It finally came down to such a simple mistake

Thank you for helping. (I looked into the log files and found that outlet was being closed!).

[ftab]

I have a question regarding setting Windkessel model in steady solution and appreciate if Andrew or Pranjal answer it.
When you are setting the boundary you have two options:Opening or Pressure outlet.
If you set it as opening with ~6000 Pa pressure, there will definitely be a back flow (according to your own pressure contour in Post 1) and there will be negative pressure as the boundary.
Setting as pressure outlet is even worse as 100% of the outlet will be changed to wall.
How did you both manage to converge to correct solution?

[shiju7279]

Can you please share the udf file for it?

Originally Posted by Trev0r

I've actually solved this now, I needed to integrate the global velocity components v over outlet1 and u over outlet2 instead of w. I thought using the local coordinate system with z normal to the outlets changed the definition of the velocity componets but global velocity components, not local ones must be used.

[zh&c]

Hello,I want to calculate dQ/dt? Could you tell me how to get previous time step flow rate?Thank you!

[ghorrocks]

The supported way of doing it is using a user fortran routine - and note you will have to store the variable yourself, it is not kept in CFX.

stumpy's post covers other options:

Are you calculating dP/dt? If so, just ask for Pressure.Time Derivative in your CFX expressions.
If you really do need to old pressure, there's a hack you can use. Search this forum for "Update Loop = TRANS_LOOP".

Note the TRANS_LOOP approach is unreliable and unsupported. It might not work for you.