CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

fsi model of water flow in a pipe

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2009, 14:22
Default fsi model of water flow in a pipe
  #1
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
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
alinik is offline   Reply With Quote

Old   October 13, 2009, 00:50
Default
  #2
smn
Member
 
Join Date: Jun 2009
Posts: 56
Rep Power: 8
smn is on a distinguished road
hi:
Explain about your initial and boundary coniditions....
smn is offline   Reply With Quote

Old   October 13, 2009, 23:39
Default
  #3
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
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
alinik is offline   Reply With Quote

Old   October 14, 2009, 09:14
Default
  #4
smn
Member
 
Join Date: Jun 2009
Posts: 56
Rep Power: 8
smn is on a distinguished road
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.
smn is offline   Reply With Quote

Old   October 15, 2009, 00:45
Default
  #5
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
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
alinik is offline   Reply With Quote

Old   October 15, 2009, 03:06
Default
  #6
New Member
 
Arda Ersan
Join Date: Aug 2009
Posts: 13
Rep Power: 8
cfdman is on a distinguished road
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
cfdman is offline   Reply With Quote

Old   October 15, 2009, 11:55
Default
  #7
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
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
alinik is offline   Reply With Quote

Old   October 25, 2009, 01:57
Default
  #8
smn
Member
 
Join Date: Jun 2009
Posts: 56
Rep Power: 8
smn is on a distinguished road
hi:
you can create mesh in gambit (.msh) and import it to cfx for your fluid domain.read help.
smn is offline   Reply With Quote

Old   October 26, 2009, 09:21
Default
  #9
New Member
 
Paul
Join Date: Mar 2009
Posts: 3
Rep Power: 8
ebpaul is on a distinguished road
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.
ebpaul is offline   Reply With Quote

Old   October 27, 2009, 15:00
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 517
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   November 5, 2009, 04:37
Default
  #11
New Member
 
Victor
Join Date: Oct 2009
Posts: 1
Rep Power: 0
vic_09 is on a distinguished road
Hi,
Im also doing a FSI with, thats what I think, the same problem: fluid flow through a pipe. But Im doing it one way.

Im 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 cant 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 dont know whether everything is ok what Ive done. So if anyone has experience in this field and especially also worked with Ansys workbench, please help.

Regards,
Victor
vic_09 is offline   Reply With Quote

Old   November 5, 2009, 12:29
Default
  #12
Senior Member
 
Join Date: Apr 2009
Posts: 517
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
FSI on a Rotating Structural Model drgolf CFX 9 August 30, 2007 12:08
Multiphase flow. Dispersed and free surface model Luis CFX 8 May 29, 2007 18:13
Flow laminar and stationary of water in a pipe manuel OpenFOAM Running, Solving & CFD 6 March 24, 2007 19:23
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
First steps - laminar flow in a pipe Maria Phoenics 8 November 27, 2001 12:26


All times are GMT -4. The time now is 00:08.