Weird velocity distributions on opening

Ordo · November 25, 2019, 04:28

Hi everyone

Inexperienced CFD user here. I'm trying to simulate the flow around a building in Ansys CFX, but I'm receiving some weird results, when I plot the velocities on my opening BC surfaces. The surface normal to Y axis and X axis are my inlets. There I've defined a logarithmic velocity profile. As I wanted to simulate different angles of attack of the wind, I've also split it into Y and X components. The other free surfaces (the ones displayed in the plot) I have defined as openings with reference pressure 0 Pa and Flow Direction normal to BC. The Walls of the building and the ground are defined as smooth walls.

Now, when I plot velocity on the opening BCs, I get these weird regions, where velocity is 0. These also move with my angle of attack, which is why I'm thinking it's not the mesh, that's causing problems, rather the BCs. I've also encountered this problem in another case, where the building geometry is slightly different, but all the BCs have been defined the same way.

Was also thinking about the height of the domain maybe not being large enough, currently the total height is 3 times the building height.

Any ideas, what this might be?
Would be grateful for any tips.

ghorrocks · November 25, 2019, 05:34

There are a few standard checks you need to do in any CFD analysis to show it is accurate:
1) Check the mesh is fine enough
2) Check it is converged tightly enough
3) Check the time step is small enough (if transient)
4) Check the boundary conditions are far enough away from the action

In your case looking at your images you have certainly problems with (4), and possibly with (2). Just about all beginners guess the mesh size required incorrectly, so you probably have a problem with (1).

So read this FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

And do sensitivity analysis on the boundary proximity, convergence tolerance and mesh size (and time step size if transient).

Ordo · November 25, 2019, 06:00

Thanks very much for the suggestions.

As for convergence, the solver managed to reach 1E-6 for RMS Residuals in just about 100 iterations, while the timestep was about 7 seconds. I set it up as a steady state analysis and initialized the domain with my logarithmic velocity BC.
I also checked convergence with some monitor points in the wake of the building and velocity wasn't changing anymore, as the solver approached the residual target.

The computational domain in total is 7 times the length of the building in the Y-direction and 4 times the length of the building in the X-direction. The mesh currently is just as fine as possible with my current license (512K cells).

ghorrocks · November 25, 2019, 06:15

That sounds likely that it is adequately converged. But you should do a run to 1E-7 and compare to check (this is a sensitivity analysis).

You certainly have a problem with the proximity of the boundary conditions to the object. So do a simulation with the domain 14x in Y and 8x in X and see if it makes a difference. I guarantee it does, so keep increasing the domain size until your results are not sensitive to the boundary location (ie a sensitivity analysis).

And don't forget you almost certainly have a problem with inadequate mesh resolution. You will quickly find that it is not possible to do much in the way of serious simulations with a 512k node limit. You will need to either get a full license or say the simulation is not possible with the available resources.

Gert-Jan · November 25, 2019, 06:50

You can appy symmetry on this simple geometry. So you can double the mesh resolution, or increase the size of your domain.
This is only valid for steady state situations. For transient analyses, you need 3D.

Antanas · November 27, 2019, 01:15

Quote:

Originally Posted by Ordo

Hi everyone

Inexperienced CFD user here. I'm trying to simulate the flow around a building in Ansys CFX, but I'm receiving some weird results, when I plot the velocities on my opening BC surfaces. The surface normal to Y axis and X axis are my inlets. There I've defined a logarithmic velocity profile. As I wanted to simulate different angles of attack of the wind, I've also split it into Y and X components. The other free surfaces (the ones displayed in the plot) I have defined as openings with reference pressure 0 Pa and Flow Direction normal to BC. The Walls of the building and the ground are defined as smooth walls.

Now, when I plot velocity on the opening BCs, I get these weird regions, where velocity is 0. These also move with my angle of attack, which is why I'm thinking it's not the mesh, that's causing problems, rather the BCs. I've also encountered this problem in another case, where the building geometry is slightly different, but all the BCs have been defined the same way.

Was also thinking about the height of the domain maybe not being large enough, currently the total height is 3 times the building height.

Any ideas, what this might be?
Would be grateful for any tips.

IMO your boundaries are too close to your object of interest. Here are the recommendations for external flows:

Quote:

A structure has height H & width W, the domain should be at least 5H high, 10W wide, with at least 2H upstream of the building & 10H downstream.
Verify that there are no significant pressure gradients normal to any of the boundaries of the domain. If there are, enlarge the size of domain.

November 25, 2019, 05:34		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	There are a few standard checks you need to do in any CFD analysis to show it is accurate: 1) Check the mesh is fine enough 2) Check it is converged tightly enough 3) Check the time step is small enough (if transient) 4) Check the boundary conditions are far enough away from the action In your case looking at your images you have certainly problems with (4), and possibly with (2). Just about all beginners guess the mesh size required incorrectly, so you probably have a problem with (1). So read this FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F And do sensitivity analysis on the boundary proximity, convergence tolerance and mesh size (and time step size if transient). __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

November 25, 2019, 06:15		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	That sounds likely that it is adequately converged. But you should do a run to 1E-7 and compare to check (this is a sensitivity analysis). You certainly have a problem with the proximity of the boundary conditions to the object. So do a simulation with the domain 14x in Y and 8x in X and see if it makes a difference. I guarantee it does, so keep increasing the domain size until your results are not sensitive to the boundary location (ie a sensitivity analysis). And don't forget you almost certainly have a problem with inadequate mesh resolution. You will quickly find that it is not possible to do much in the way of serious simulations with a 512k node limit. You will need to either get a full license or say the simulation is not possible with the available resources. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
kindly help me .. i have and error at line number 147..	m zubair	Fluent UDF and Scheme Programming	0	February 10, 2019 11:25
Problem with Velocity Poisson Equation and Vector Potential Poisson Equation	mykkujinu2201	Main CFD Forum	1	August 12, 2017 13:15
Velocity weird behaviour	cinclus	FLUENT	0	April 1, 2015 00:45
WSS and normal velocity gradient for the slanted pipe	wanna88	FLUENT	2	October 1, 2012 22:34
Velocity in Porous medium : HELP! HELP! HELP!	Kali Sanjay	Phoenics	0	November 6, 2006 06:10

November 25, 2019, 06:00		#3
Ordo New Member Join Date: Nov 2019 Posts: 4 Rep Power: 6	Thanks very much for the suggestions. As for convergence, the solver managed to reach 1E-6 for RMS Residuals in just about 100 iterations, while the timestep was about 7 seconds. I set it up as a steady state analysis and initialized the domain with my logarithmic velocity BC. I also checked convergence with some monitor points in the wake of the building and velocity wasn't changing anymore, as the solver approached the residual target. The computational domain in total is 7 times the length of the building in the Y-direction and 4 times the length of the building in the X-direction. The mesh currently is just as fine as possible with my current license (512K cells).

November 25, 2019, 06:50		#5
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	You can appy symmetry on this simple geometry. So you can double the mesh resolution, or increase the size of your domain. This is only valid for steady state situations. For transient analyses, you need 3D.