code_saturne User's Forum

I have been trying to carryout a simulation of a flexible pipe type(blood vessel) simulation which I have mentioned before in another post.But the new problem is that my simulation is not running with the new setup where I have considered a rigid wall(fixed).I have attached the xml file below.
Notes:
1)I have used the properties in terms of "mm" as the geometry was done in unitless co-ordinates in salome.But it is being assumed as "m" depending on the co-ordintates in the solver.Hence the change.So it might look absurd but it is not.
2)I have tried PISO and SIMPLEC both fails with PISO failing earlier with "2" selected as the order.SIMPLEC fails too.The pseudo-steady works fine.
3)All three tubulence model was checked for k-w SST model(this cannot be changed and is ofcourse working model as listed in a lot of papers) -2 scale model (log law), 2 scale model(all y+),Scalable 2 scale model(log law).None works
4)Equation parameters for v-BiCGstab2,k-BiCGstab2,w-BiCGstab2 was selected and still no use.

Here is the setup log too.Also the link to mesh that I used is given below.
https://we.tl/t-nRTKT9hNJq

Hello,

Here are a few suggestions:

- rescale the mesh instead of changing units. It is much less risky.
- add en extruded section at the outlet (or use an imposed pressure outlet)
- use a more robust gradient option (least-squares with extended neighborhood ma be a little less precise, but smoother).

Regards,

Yvan

I have tried with all three of options of "the least squares related" calculation method.None works.
I am going to try the first two suggestions.But by extrusion do you mean a mesh extrusion?(imposed pressure outlet is not there,infact no option for the outlet at all after I turned the deformable mesh off).

Wanted to add something too.Is pseudosteady in any way applicable for transient flows in Code Saturne?Should I try that?

Hello,

Yes, I am referring to a mesh extrusion.

Regarding pseudosteady flow, this may be useful to initialize a transient flow: start with pseudosteady, then switch to transient in a computation restart. In the actual transient, since pseudosteady uses a local time step, results make no sense.

Best regards,

Yvan

Thank you Yvan,Scaling the model worked(also used least square method over extended cell neighborhood along with it) though I don't uderstand why as the code should take inputs and hence calculate rest.So conflict between mm and m should not be there right?Also sorry to say that the imposed presure outlet is not applicable in my case.As I don't know the outlet pressure before hand.The pressure to be input into it is the final outlet pressure right?
Laslty it still seems that convergence is barely there as I see on the convergence tool it reached only 10^-1 for velocity,pressure,k only omega reached 10^-3( my set precision in solver precision)How do I reduce that?[Mesh extrusion suggestion was not applied]I need it because my values are very small around 10^2 for pressure and 10 to 10^-1 scale for velocity.So having such small convergence will affect the results ,no?

Hello,

Regarding the outlet pressure, as the pressure used for incompressible flows does not need to be the "true" pressure, but can be shifted by any constant value, if you have a single outlet, you can choose any outlet pressure.

Regarding convergence plots, depending on the mesh quality, numerical settings, and flow characteristics, you might not always be able to reduce the residual much more. This is why designing an automatic stopping criteria is very difficult, and we prefer to recommend less automatic criteria to check for convergence.(see "Checking the convergence" here : https://www.code-saturne.org/documentat ... utput.html).

Best regards,

Yvan