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

Increase in pressure drop when refine the mesh

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 5, 2018, 06:12
Question Increase in pressure drop when refine the mesh
  #1
New Member
 
Join Date: Jul 2018
Posts: 3
Rep Power: 7
Thromkar is on a distinguished road
Hello everyone,

I am Simulating a heattransfer problem with Ansys Fluent as seen on the attached picture.

Setup.jpg

I'm Using K-Omega-SST Turbulencemodel with "Coupled" Pressure-Velocity Coupling and the Pseudo-Transient formulation. Deactivating the Pseudo-Transient Solver leeds to the same results with slower convergence.

When performing a mesh independence study, i experienced a weird behaviour. As i increased my cell count, the pressure drop increased. The picture below shows the pressure drop over a mesh parameter. Doubling the mesh parameter will leed to 8 times more cells.

MeshRefinement.png

As we can see the pressure drop is increasing, but i never reach mesh independence. Refining the mesh even more is an option i want to avoid, since i allready got 6 million Elements in a 2x5x15 mm domain.

The Mesh is as good as it can get. Max. y+ Values are at 0,8 for most of the meshes. The y+ of the finest meshes are even lower.

I experienced the same behaviour with larger Setups, which contain more of the periodic geometries and using fixed velocity inlet and pressure outlet.

My question is, is there something wrong with my setup? Can i use symmetry boundary conditions (since the geometry is symmetrical I assume I can)?
Thromkar is offline   Reply With Quote

Old   December 5, 2018, 08:22
Default
  #2
Senior Member
 
acalado's Avatar
 
André
Join Date: Mar 2016
Posts: 133
Rep Power: 10
acalado is on a distinguished road
Are you using symmetry to essentially "double" your domain?

Which wall treatment functions are you using? I'm assuming near wall if your y+ is near 1.

And your results don't look too different. Between first and last mesh there is about 1% relative difference, which I would think is a good enough solution.

Cheers
__________________
Sapere aude!
acalado is offline   Reply With Quote

Old   December 5, 2018, 09:03
Default
  #3
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,668
Rep Power: 65
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Looks good. Forget the phrase mesh independence, it's mesh sensitivity.


However, I am skeptical your results for any given mesh are that accurate. For example you're saying that, for a fixed mesh, as you iterate your pressure drop stays exactly 622.5 +/- 0 and doesn't oscillate at all? Put numerical error bars on this plot. I wouldn't be surprised to see 622.5 +/- 5.
LuckyTran is offline   Reply With Quote

Old   December 5, 2018, 12:13
Default
  #4
New Member
 
Join Date: Jul 2018
Posts: 3
Rep Power: 7
Thromkar is on a distinguished road
Quote:
Are you using symmetry to essentially "double" your domain?

Which wall treatment functions are you using? I'm assuming near wall if your y+ is near 1.

And your results don't look too different. Between first and last mesh there is about 1% relative difference, which I would think is a good enough solution.

Cheers
I am using symmetry on both sides to essentially make a infinite domain.

When I understand it correctly, the SST model is switching automatically between Wall Functions and near wall treatment. Since i'm at y+<1 i assume, that im using near wall treatment. Am I wrong here?
Do i need to use the "Low-Re Correction" to enable near wall treatment?

Quote:
Looks good. Forget the phrase mesh independence, it's mesh sensitivity.


However, I am skeptical your results for any given mesh are that accurate. For example you're saying that, for a fixed mesh, as you iterate your pressure drop stays exactly 622.5 +/- 0 and doesn't oscillate at all? Put numerical error bars on this plot. I wouldn't be surprised to see 622.5 +/- 5.
Thanks you. In the future i will use the phrase "mesh sensitivity".

Sorry i didn't mention my convergence criterias. I defined my own convergence criteria by monitoring the "Periodic Pressure Gradient" and the "Bulk Temperature Ratio". My simulation is converged when both variables differ less than 1e-6 in the last 50 iterations. So the results aren't differ in 6th significant digits. I am very sure that my Results are not oscillating anymore. BTW all of my residuals are way below 1e-10.
Thromkar is offline   Reply With Quote

Old   December 5, 2018, 14:13
Default
  #5
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,668
Rep Power: 65
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Thromkar View Post
Sorry i didn't mention my convergence criterias. I defined my own convergence criteria by monitoring the "Periodic Pressure Gradient" and the "Bulk Temperature Ratio". My simulation is converged when both variables differ less than 1e-6 in the last 50 iterations. So the results aren't differ in 6th significant digits. I am very sure that my Results are not oscillating anymore. BTW all of my residuals are way below 1e-10.
In my experience if you run longer say over 100,000 iterations you'll find some slow gradual fluctuations in the periodic pressure gradient and bulk temperature ratio. And these can be quite significant.


But regardless, I think you've got some nice results.
LuckyTran is offline   Reply With Quote

Reply

Tags
independence, periodic, pressure, symmetry

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
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 07:38
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 11 August 6, 2021 06:40
Total pressure drop & static pressure drop Aarthar Main CFD Forum 3 April 11, 2018 03:32
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Repeated elements in a system – pressure drop llidito OpenFOAM 0 April 25, 2013 14:47


All times are GMT -4. The time now is 12:18.