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

Ansys Fluent - Turbulence model problem and meshing

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

Like Tree4Likes
  • 1 Post By vinerm
  • 1 Post By vinerm
  • 1 Post By vinerm
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 16, 2020, 16:39
Default Ansys Fluent - Turbulence model problem and meshing
  #1
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
Hi

I am currently working on a project that involves CFD simulation on ANSYS and i need some help as it has got me stuck. I am designing a faucet atomizer and it's functioning is similar to a nozzle.

I have designed it on CATIA and am trying to analyse it on ANSYS Fluent.

I am using the following conditions:

-Pressure based solver, absolute velocity, steady flow

-Flow characteristics: Laminar at inlet, turbulent at outlet

-Boundary conditions: inlet velocity: 0.041 m/s, inlet pressure: 300000 Pa,outlet pressure: 0 Pa

-Fluid: water(liquid)

I have the following doubts:

1.)I read that turbulent models give accurate results even if flow is laminar but not vice versa so i chose turbulent but which turbulent model should i apply?

2.)My geometry has swirl, complex curves and rotational flow and i read that k-epsilon, k-omega models do not handle such flows and curves well so which model should i adopt(my geometry is very small in dimensions so swirl may not matter?).

3.)How should i do the meshing of my model? I did it multiple times according to my understanding but due to some reason the solution didn't converge and diverged a couple of times as well. My system also does not have a lot of computational power hence less elements and nodes in mesh.

I have attached the link for the images of extracted volume, my mesh and the part.
I will be able to share the geometry file with you if you require.

I will be very grateful if you can help me out.

Thanks
https://drive.google.com/open?id=1Tk...bbRwx0Z7kTBhV_
Swish31 is offline   Reply With Quote

Old   April 16, 2020, 16:56
Default Domain of Interest
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
It all depends on whether you are analyzing the inside of the atomizer or the outside, i.e., the surroundings where outlet of faucet is considered as inlet. Or it may have both; the faucet as well as the surroundings.
Swish31 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 16, 2020, 17:08
Default
  #3
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
Sir i want to analyze the inside.
Swish31 is offline   Reply With Quote

Old   April 16, 2020, 17:17
Default Setup Suggestions
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
Since the flow is wall bounded, prefer SST k-\omega model. Eddy viscosity models, such as, k-\varepsilon and k-\omega do not handle anisotropy in turbulence well, however, this needs to be tested for your case; the turbulence in your case may or may not be isotropic. However, k-\omega would work to a good extent. The most important part in your case is the pressure. You have mentioned a pressure of 3 bar. Is it gauge or absolute? If you consider fluid to be incompressible, then the pressure won't have any effect. So, you have to consider it compressible. With compressible fluid, you should not use velocity inlet; use either pressure inlet or mass flow inlet. I'd suggest you to start with incompressible fluid and velocity inlet. Once that case works fine, then you should start working with compressible fluid.

As far as mesh is concerned, if you cannot generate hex mesh, generate a fine tet mesh, close to 1.5 - 2 million cells. Then, in Fluent, convert it into polyhedral. This will reduce the count below half a million and may also improve the quality. However, the conversion requires good amount of RAM. For 1.5 mn cells, you will need at least 8 GB. If you can't do that, then try to put good quality tet mesh with at least 4 layers of boundary layer mesh, called inflation in Ansys Meshing. This is required for using SST k-\omega.
Swish31 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 16, 2020, 17:22
Default
  #5
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
Sir the 3bar pressure is gauge pressure as the water that generally flows in our pipes is 3 bar. The fluid is water so how to go about the compressible fluid part since it is incompressible.

If using the k-Omega model will generating a good quality tetrahedral mesh with inflation layers work or do i have to give some other features as well?
Swish31 is offline   Reply With Quote

Old   April 16, 2020, 17:26
Default Compressibility
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
3 bar at inlet and 0 bar at outlet imply a drop of 3 bar across the nozzle, which is significant. If that is required for the mass corresponding to 0.041 m/s velocity at the inlet to go through, then you won't have to use compressible fluid. That you can check by running a case with constant density. Fluent will predict the pressure at the inlet for the required mass to go through. If it is closer to 3 bar, then it is good. If it is way too less than that, which I expect, then you will have to use compressible fluid. That option is available under material properties as compressible liquid. The coefficients given are as per water so you don't have to change those.
Swish31 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 16, 2020, 18:07
Default
  #7
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
So ill use the pressure based solver with k-omega velocity inlet only.
Swish31 is offline   Reply With Quote

Old   April 30, 2020, 17:30
Default
  #8
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
Dear sir,
I solved the problem using velocity inlet and pressure outlet and the inlet pressure i got was 2.2 bar as opposed to the expected 3 bar.
Why is this difference there? Is there any error? The fluid is water hence incompressible.
Swish31 is offline   Reply With Quote

Old   May 1, 2020, 16:21
Default Pressure Drop
  #9
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
Any particular reason that you want it to be 3 bar? Is it a value reported from some test? If that is the case, then you will have to look at other aspects, such as, roughness of the impeller blades and casing, length and roughness of the inlet and outlet ducts. As per the setup, assuming mesh is fine enough to resolve the shear stresses at the blades and the casing of the pump, results would be within 10% error. So, if for a certain flow rate, 2.2 bar is the pressure drop, then that's it. Do note that you have to compare total pressure drop and not static pressure drop.

Every fluid is compressible, even lava and molten steel. All that matters is Mach number. Any flow above Mach number 0.25-0.3 is considered compressible, provided it is in continuum.
Swish31 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 6, 2020, 16:39
Default
  #10
Member
 
Siddharth Vohra
Join Date: Apr 2020
Posts: 42
Rep Power: 2
Swish31 is on a distinguished road
Thank you ! I was able to get it done. Now onto the spray pattern.
Swish31 is offline   Reply With Quote

Reply

Tags
ansys, cfd, fluent, mesh, turbulence analysis

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
Hydrodynamic analysis of submarine model with ANSYS FLUENT? Sovereignty ANSYS 0 January 20, 2019 19:36
[ANSYS Meshing] Ansys Fluent Meshing Problem: Conflicting zone names SimonWjp ANSYS Meshing & Geometry 1 November 14, 2016 02:59
Ansys Fluent Meshing Problem: Conflicting zone names SimonWjp FLUENT 0 November 8, 2016 11:38
[ANSYS Meshing] ANSYS Meshing Problem Saikat_FM ANSYS Meshing & Geometry 1 September 15, 2016 03:25
[ANSYS Meshing] Dynamic Meshing of a Valve in ANSYS FLuent 15.0 A.Jalal ANSYS Meshing & Geometry 0 March 23, 2015 19:37


All times are GMT -4. The time now is 15:01.