[alinik]

I follow all the Tutorial21 steps completely to simulate a FSI model of a water flow in a pipe with 0.02 mm thickness, but it CFX can not solve and shows this message: +--------------------------------------------------------------------+
| ERROR #002100061 has occurred in subroutine SERVE_CLIENTS. |
| Message: |
| The connection between this CFX process and an external process |
| has died unexpectedly. The following error was received: |
| External process : ANSYS |
| Error experienced : Read |
| |
| ** This error is fatal: Terminating ANSYS CFX Solver execution ** |
| Please review the output, error and log files from both the CFX |
| and external processes to determine the cause of the error. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created


can any body help me with this?

regards, alinik

[smn]

hi:
Explain about your initial and boundary coniditions....

[alinik]

boundary condition:

inlet: uniform normal pressure distribution over inlet area(varying with time)
outlet:fully developed velocity distribution(varying with time)
wall:no slip

thank , alinik

[smn]

hi:
the most important thing u should pay attention is your mesh quality...
after that,this error may be about your boundary condition.it seems that sudden inlet or outlet causes high mesh motion and distortion...try to ramp your boundary conditions.for example if the pressure outlet is 100 kpa try to ramp it from 0 to 100 in 1 second.this causes slow out going of fluid and prevents sudden distortion.

[alinik]

How can I improve my mesh in CFX both in solid and fluid domain?Is it possible to use an external mesh generator? my boundray conditions are the mathematical function whish were used by other researchers and solve this kind of problem.

thanks, alinik

[cfdman]

I think it is a two-way FSI and this is timestep error. You have to use same timestep on ANSYS and CFX and autotimestepping have to be off.
As i understand from your explanations, you have a model of water pipe so could you give some details about your model. For example what results do you want? maybe you can try one-way FSI. Because two-way is very computationally expensive.
If deformations are small, you should use one-way.

Regards

[alinik]

I use the same timesteps in CFX and ANSYS, I want to impose pressure at inlet and a fully develped velocity profile at outlet, which both of these boundaries are the function of time. I prefer to use two way, but how can I use 1 way could you tell me the steps? In addition, the geometry is so small(Radius=0.5 cm & thickness=0.07 cm ).

regards, alinik

[smn]

hi:
you can create mesh in gambit (.msh) and import it to cfx for your fluid domain.read help.

[ebpaul]

1) Ansys ICEM CFD is very good mesh generator you can try.
2) if i understand your problem correctly it is, water flowing in a pipe with some diameter. there is a pipe, inside the pipe water is flowing.

i dont know which software you have used to model the structural part, i.e the pipe.

if i see your BCs for fluid, one of the BC is wall with "No Slip" boundary details. what about "additional coupling sent data".
did you check properly for that.
probably you check this.

[stumpy]

The error message means that ANSYS failed. Look at the ANSYS.stdout file to see why - I assume the deformations were too large. Run a Static Structural analysis (not FSI) using the solid geometry and apply a typical fluid pressure. Does this work? How large are the deformations? Unless your initial fluid field produces deformations that are very close to zero, then you should solve a steady-state FSI case first, then restart this as a transient. The tutorials won't tell you how to do this; I would recommend getting some support/training from ANSYS.

[vic_09]

Hi,
I´m also doing a FSI with, thats what I think, the same problem: fluid flow through a pipe. But I´m doing it one way.

I´m working with Ansys Workbench 2.0 (Version 12.0.1).

I ´ve got two problems. Firstly the imported load (form the solution of the fluid) has only one value, although the simulation has 25 time steps. So in my opinion I should have 25 values which are given to solver of the structure.

Secondly the imported load has no influence of my structure. There are no deformations and so on. On the other hand a warning message is shown that large deformations influence the simulation. But I can´t see them and the simulation is not terminated...
So i guess I have to switch these large deformations on. But how?

The main problem is that I don´t know whether everything is ok what I´ve done. So if anyone has experience in this field and especially also worked with Ansys workbench, please help.

Regards,
Victor

[stumpy]

For transient 1-way FSI you should set it up as a 2-way FSI simulation, but then only send data in one direction. If you use your approach, it is possible to get 25 different loads, but it won't be a true transient, rather just 25 static results. The Large Deflection setting is under the Analysis Settings in Mechanical in WB.