CFD Online Logo CFD Online URL
Home > Forums > CFX

help needed in Cfx pre

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

LinkBack Thread Tools Display Modes
Old   February 1, 2012, 04:56
Default help needed in Cfx pre
Senior Member
Join Date: Nov 2011
Posts: 107
Rep Power: 8
shaswat is on a distinguished road
Please find the attached documents

I found that

A wall has been placed at portion(s) of an INLET |
| boundary condition (at 11.1% of the faces, 4.3% of the area) |
| to prevent fluid from flowing out of the domain. |
| The boundary condition name is: inlet. |
| The fluid name is: Fluid 1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead.

so I made a mistake in setting . kindly help me how to solve the problem smoothly

Thank you


Attached Images
File Type: jpg error.jpg (67.8 KB, 31 views)
Attached Files
File Type: txt outputnormal but wall blocking.txt (85.2 KB, 7 views)
shaswat is offline   Reply With Quote

Old   February 1, 2012, 06:08
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,202
Rep Power: 110
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your simulation has not converged very well, it might fix itself when you get it to converge. If it remains then you need to move the inlet boundary further upstream.
ghorrocks is offline   Reply With Quote

Old   February 3, 2012, 16:59
Default start steady-state and use smaller timesteps
New Member
Daniel Collins
Join Date: Jul 2011
Location: Michigan, USA
Posts: 5
Rep Power: 8
cfd_dansir is on a distinguished road
i imagine your pressure function is very dynamic. i am very familiar with this study of blood flowing in Artery.

1. it be wise to let your model "warmup" your pressure loss. start with a steady-state condition based on an average pressure loss to find a close convergence and to test the mesh and other conditions/boundaries/parameters, etc. Experiment and develop appropriate parameters.
1b. start also with more simplier fluid dynamics. e.g. use Newtownian fluid before a non-Newtowian value for viscosity. run the model without the porous media (the stent) before running with it.


2. decrease the size of your timestep. do some hand calculations of the Courant number, based on various points on your pressure curve. you may need to change the timestep accordingly. you can create functions in CEL with if statements, to create little pockets of different values of timesteps. or create table or other input.

3. since the pressure wave is very dynamic, expect to have smaller timesteps and need more inner-loops (coefficient loops) for the 2nd order inflections of the curve; namely the peaks and troughs. much like #2, you can create CEL function for this.

4. extend your mesh adequately length at either the inlet or outlet or both. this is what the previous post means by positioning your inlet.

5. try using smaller section of the pressure-curve to fine tune those aspects of the model. once you have the steadystate version (see #1), you can experiment and develop better parameters.

bottom-line, the blood flows in pulsations, using contractions from the muscles (and arterial walls). therefore, expect yourself to see negative pressure drops or backflow and backpressure and flow through the inlet--- this is expected! consider making it an Opening instead because of this fact.
cfd_dansir is offline   Reply With Quote


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
[ANSYS Meshing] remeshing in Ansys CFX - help or tutorials needed Doginal ANSYS Meshing & Geometry 6 September 24, 2014 09:43
Under Relaxation Factors in CFX Pre akj Main CFD Forum 0 December 15, 2011 02:50
Defining a domain in CFX Pre ashtonJ CFX 1 June 13, 2011 02:34
Heat transfer settings in ANSYS CFX Pre. saisanthoshm88 CFX 1 November 6, 2010 07:14
CFX Pre Hide symmetry symbols alvid CFX 2 August 15, 2007 11:34

All times are GMT -4. The time now is 16:08.