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

Weird velocity distributions on opening

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 25, 2019, 04:28
Default Weird velocity distributions on opening
  #1
New Member
 
Join Date: Nov 2019
Posts: 4
Rep Power: 4
Ordo is on a distinguished road
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.
Attached Images
File Type: jpg Post1.jpg (68.7 KB, 14 views)
File Type: jpg Post2.jpg (43.5 KB, 9 views)
Ordo is offline   Reply With Quote

Old   November 25, 2019, 05:34
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   November 25, 2019, 06:00
Default
  #3
New Member
 
Join Date: Nov 2019
Posts: 4
Rep Power: 4
Ordo is on a distinguished road
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).
Ordo is offline   Reply With Quote

Old   November 25, 2019, 06:15
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   November 25, 2019, 06:50
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,580
Rep Power: 24
Gert-Jan will become famous soon enough
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.
Gert-Jan is offline   Reply With Quote

Old   November 27, 2019, 01:15
Default
  #6
Senior Member
 
Join Date: Feb 2011
Posts: 495
Rep Power: 16
Antanas is on a distinguished road
Quote:
Originally Posted by Ordo View Post
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.
Antanas is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 18:47.