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

opening sims as a wall.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 16, 2012, 15:45
Default opening sims as a wall.
  #1
New Member
 
Curran
Join Date: Mar 2012
Posts: 6
Rep Power: 5
Curran919 is on a distinguished road
I am modeling pulsatile (transient) flow over a backward facing step (Re~200). With my current mesh and configuration, steady state conditions put my opening far downstream of the area of interest.

Using an outlet, there is some backflow, so this obviously doesn't work as it walls off progressively more of the outlet at every iteration until its at 100%. Swtiching to an opening, there are no warnings in the output file about walling off the domain, but I still get strange results.

The inlet condition pulses between 0 (at t0)and 2mm/s. The expansion factor of the BFS is 2, so the mean flow in the downstream channel is 0.5 mm/s.

The results show my initialization values for the first time step, and each other time step with near zero values (max ~5.0E-3 mm/s). Streamlines show strong vertices at the corners between the inlet/opening and side walls. It looks as if there is no flux out the opening.

I've tried a wide range of different configurations for the opening with equally disappointing results, but I am thinking it must be how the opening is defined. How SHOULD the opening be defined for this?

Thanks for your help,
Curran
Curran919 is offline   Reply With Quote

Old   March 17, 2012, 06:20
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What does BFS mean? How fast is the pulsing? Is the fluid incompressible? Is the pulsing fast enough that compressibility effects are important? What experimental setup are you trying to reproduce?
ghorrocks is offline   Reply With Quote

Old   March 17, 2012, 14:26
Default
  #3
New Member
 
Curran
Join Date: Mar 2012
Posts: 6
Rep Power: 5
Curran919 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
What does BFS mean? How fast is the pulsing? Is the fluid incompressible? Is the pulsing fast enough that compressibility effects are important? What experimental setup are you trying to reproduce?
This is for a biological flow, so pulse is sinusoidal, 1hz. The fluid is incompressible (water). BFS is the backward facing step, similar to the steady state case seen here (http://tinyurl.com/6p2mole, flow in +x). The colleague I was taking this over from had achieved 2D results in fluent with the same parameters, so I imagine there is nothing over-complicated with the nature of the flow.
Curran919 is offline   Reply With Quote

Old   March 18, 2012, 06:05
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you post your CEL?
ghorrocks is offline   Reply With Quote

Old   March 19, 2012, 13:44
Default
  #5
New Member
 
Curran
Join Date: Mar 2012
Posts: 6
Rep Power: 5
Curran919 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Can you post your CEL?
From my newbie deductive skills, does the attached .ccl contain what you need?
Attached Files
File Type: txt BFS3.txt (20.3 KB, 4 views)
Curran919 is offline   Reply With Quote

Old   March 19, 2012, 19:47
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Yes, that is the CCL.

Some comments:
* You have fixed time steps of ~0.03s. Are you sure that time step size is OK? How did you check? You only have 30 time steps in the simulation which is very coarse.
* The Opening pressure and direction option for openings is usually a better choice. Why did you choose entrainment?
* Why did you choose "previous time step" for the time step initialisation option? Best leave this at automatic unless you have a good reason not too.
ghorrocks is offline   Reply With Quote

Old   March 19, 2012, 20:21
Default
  #7
New Member
 
Curran
Join Date: Mar 2012
Posts: 6
Rep Power: 5
Curran919 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Yes, that is the CCL.

Some comments:
* You have fixed time steps of ~0.03s. Are you sure that time step size is OK? How did you check? You only have 30 time steps in the simulation which is very coarse.
* The Opening pressure and direction option for openings is usually a better choice. Why did you choose entrainment?
* Why did you choose "previous time step" for the time step initialisation option? Best leave this at automatic unless you have a good reason not too.
Okay this, is very helpful!
*I didn't realise that was that coarse of a time step. I imagined you could get away with longer steps for such a low Re. That is what I had put my inlet velocity profile at, 32x32 points in 32 time steps for one oscillation. If I increase the number of steps in the simulation, should I increase the resolution of the inlet condition or will it interpolate enough?
*It hadn't worked when I originally defined the pressure, so I changed it to entrainment on the suggestion of an online resource. I imagine I should change it back.
*I was under the impression that is how the transient initialisation would work. I don't remember changing it from automatic, but I will change that back.


Also, I am expecting a series of shed vortices downstream of the recirculation zone, two for each period, possibly having up to 6 vertices before the outlet/opening. It seems obvious, but I should be simulating 3 periods to achieve all of this, correct? If this is the case, would it not be advantageous to run maybe 6 periods and take the final three if it is going to initialise the entire domain as stagnant? Or can I run the simulation once and use it as the IC for itself?
Curran919 is offline   Reply With Quote

Old   March 19, 2012, 20:55
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You should set time step size by a sensitivity analysis. It should interpolate your inlet condition.

I have had stability problems with entrainment. So unless you need it then revert to the normal pressure & direction option.

If you are trying to generate a time periodic flow then you need to run it long enough to establish it. It might take more than 3 cycles. It does not really matter whether you run it as one long simulation or multiple simulations with initial conditions, but restarting sometimes causes a small kink in the results so is best avoided if possible.
ghorrocks is offline   Reply With Quote

Old   March 19, 2012, 22:31
Default
  #9
New Member
 
Curran
Join Date: Mar 2012
Posts: 6
Rep Power: 5
Curran919 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You should set time step size by a sensitivity analysis. It should interpolate your inlet condition.

I have had stability problems with entrainment. So unless you need it then revert to the normal pressure & direction option.

If you are trying to generate a time periodic flow then you need to run it long enough to establish it. It might take more than 3 cycles. It does not really matter whether you run it as one long simulation or multiple simulations with initial conditions, but restarting sometimes causes a small kink in the results so is best avoided if possible.
Ah yes, I think it may be the CFL condition that I was ignoring. Lets hope this fixes it! Thanks a lot Glen.
Curran919 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
Very technical question about solving wall boundary layer ... jlb001 FLUENT 6 December 27, 2014 06:56
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
Changing BC from Opening to Wall during Solving Ahmad M. Kermani CFX 0 December 17, 2008 22:20
Wall functions? Pr Main CFD Forum 7 April 8, 2004 06:15
Quick Question - Wall Function D.Tandra Main CFD Forum 2 March 16, 2004 05:29


All times are GMT -4. The time now is 15:38.