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

Vortex Tube Fluid Flow Simulation

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

Like Tree3Likes
  • 2 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 4, 2021, 10:43
Default Vortex Tube Fluid Flow Simulation
  #1
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 287
Rep Power: 12
sasanghomi is on a distinguished road
Hi

I am trying to model the fluid flow inside a vortex tube.

I applied
Total Pressure @ Inlet
Static Pressure @ Cold Outlet
Static Pressure @ Hot Outlet

You can see the geometry in the attached pic.
My problem is that it is too sensitive to the mesh.
I started with 2 million grid cells and now 8 million mesh (for the attached sector). The cold temperature does not stop changing.

Does anybody have the same experience?
Regarding the turbulence model, I am using K-epsilon RNG. if you have any suggestions about turbulence options, please let me know.
Attached Images
File Type: jpg VT.JPG (42.6 KB, 11 views)
__________________
Best Regards
Sasan Ghomi
sasanghomi is offline   Reply With Quote

Old   June 4, 2021, 23:19
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,140
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
A separate point:
You will not be able to get any k-eps family turbulence model to work on this. You have a slight chance that SST with the curvature correction model will work, but you more likely will need RSM or an LES model for this.

Your question:
If the value does not stop changing then you do not have an accurate solution to it yet. You might need to refine the mesh further, but you also might need to do other things (eg tighter convergence tolerance, switch to transient simulation, different turbulence model etc). You need to look at the results and work out whether it is mesh resolution or something else causing the problem.

Finally:
A CFD with 8 million elements is not a very big mesh. It is common to require meshes of this size or larger for mesh independence. Sometimes much larger
sasanghomi and aero_head like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 5, 2021, 12:57
Default
  #3
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 287
Rep Power: 12
sasanghomi is on a distinguished road
Thanks Glenn for your response.
I would be thankful if you could let me ask you another question.
Do you have any ideas about the Mesh? I can see most articles have used hexahedral grids. I suppose in this case the flow direction is not necessarily perpendicular to hexahedral mesh. So, do you think that tetrahedral cells reduce the accuracy in this case?
__________________
Best Regards
Sasan Ghomi
sasanghomi is offline   Reply With Quote

Old   June 6, 2021, 07:04
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,140
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Dissipation is lower for a flow which is aligned to the grid compared to one flowing at an angle to the grid. So if the flow is aligned with the grid with a hex mesh then you will get a bit lower dissipation. If the flow is not aligned to the grid you will get about the same dissipation between hex and tet meshes.

Also, hex meshes form polygons around the nodes with less faces than tets. This leads to reduced memory consumption. It is quite a big difference, about a factor of 2 or 3. But if you have heaps of memory this is not important. But if you are running out of memory you will run a bigger simulation with a hex mesh than a tet mesh.

But at the end of the day these are just general guidelines. Try a hex and tet mesh in your case and see if it makes any difference for you.
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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
cfd simulation of fluid flow in a radiator ztdep Main CFD Forum 0 April 23, 2017 05:01
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
Ansys Fluid flow simulation for a cooling system help!!! pradon16 ANSYS 0 July 24, 2012 10:15
why is solid temperature same as fluid temperature on flow simulation ? qihongming FloEFD, FloWorks & FloTHERM 0 May 26, 2009 08:57
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 20:28


All times are GMT -4. The time now is 04:32.