CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   opening sims as a wall. (http://www.cfd-online.com/Forums/cfx/98708-opening-sims-wall.html)

Curran919 March 16, 2012 15:45

opening sims as a wall.
 
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

ghorrocks March 17, 2012 06:20

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?

Curran919 March 17, 2012 14:26

Quote:

Originally Posted by ghorrocks (Post 349962)
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.

ghorrocks March 18, 2012 06:05

Can you post your CEL?

Curran919 March 19, 2012 13:44

1 Attachment(s)
Quote:

Originally Posted by ghorrocks (Post 350051)
Can you post your CEL?

From my newbie deductive skills, does the attached .ccl contain what you need?

ghorrocks March 19, 2012 19:47

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.

Curran919 March 19, 2012 20:21

Quote:

Originally Posted by ghorrocks (Post 350321)
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?

ghorrocks March 19, 2012 20:55

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.

Curran919 March 19, 2012 22:31

Quote:

Originally Posted by ghorrocks (Post 350326)
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.


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