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

Is Mean Free Path useful in determining mesh resolution?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 30, 2013, 19:46
Default Is Mean Free Path useful in determining mesh resolution?
  #1
New Member
 
Join Date: Jan 2013
Posts: 3
Rep Power: 4
pt39 is on a distinguished road
I've been trying to simulate an opening at a constant 20 psi that fills a closed space that is roughly 5''x3.33''x.214''.

I'm simulating this for 10 ms, at a timestep of 1e-5s. But my solution diverges.

I think this might be due to a poor spatial resolution in my mesh.

I read about something called the "mean free path", the average distance between collisions. Does this have any effect on what mesh resolution I need?

If so, I am simulating a blast wave, and according to wikipedia: "Shock waves are not conventional sound waves; a shock wave takes the form of a very sharp change in the gas properties on the order of a few mean free paths (roughly micro-meters at atmospheric conditions) in thickness. ".

Would my element size need to be on this 1e-6 order of magnitude to accurately simulate my model?

I am using SST for turbulence, Total Energy for thermal.
pt39 is offline   Reply With Quote

Old   January 31, 2013, 17:08
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX is a Navier Stokes solver. This has no relation to mean free path as the NS equations assume a continuum. So mean free path tells you nothing about what is requierd to get this model to converge.

Do a mesh sensitivity study to determine the mesh size you require. And to assist convergence you almost certainly need a smaller time step.
ghorrocks is offline   Reply With Quote

Old   February 1, 2013, 12:11
Default
  #3
New Member
 
Join Date: Jan 2013
Posts: 3
Rep Power: 4
pt39 is on a distinguished road
Hi Glenn,

I actually decreased my step yesterday to a 1e-6s adaptive timestep, and this also failed to converge at an adapted time step of 1e-7s about 1 ms into the simulation. This is also using the same mesh as before.

Would you happen to know what order should my time step be to accurately simulate a blast wave in such a small confined area? I'm using an RMS convergence criteria of 1e-4.

Here's a my model to illustrate:


The two Inlets have a static pressure of 80 psi, a total pressure of 160 psi, and a total temperature of 320K.

Last edited by pt39; February 1, 2013 at 12:30.
pt39 is offline   Reply With Quote

Old   February 2, 2013, 06:02
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What makes you think 1e-7s is small enough? One of the commonest beginner mistakes is to use a time step which on the human scale is really small and to therefore assume that this is adequate for the simulation.

If you want to estimate the time scale required for this simulation, work out the speed of sound and how long it takes to travel one mesh element. Then divide that by about 4. This gives you a CFL number of 0.25 which is a good place to start looking for a time step size suitable for your simulation. But it is only a starting point, your actual time step could be much bigger or smaller than that.

A better way which I recommend you use adaptive time stepping, but with a starting time step of 1e-12s and let it increase to the time step it needs from there. Once you know the time step it needs you can do future simulations using this time step as a starting point.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh around ship with appropriate free surface refinement Hannes_Kiel OpenFOAM Native Meshers: snappyHexMesh and Others 45 April 2, 2015 02:29
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
[ICEM] Free mesh control Rhyno466 ANSYS Meshing & Geometry 6 September 25, 2011 18:42
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 22:29.