Is Mean Free Path useful in determining mesh resolution?

pt39 · January 30, 2013, 18:46

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.

ghorrocks · January 31, 2013, 16:08

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.

pt39 · February 1, 2013, 11:11

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.

ghorrocks · February 2, 2013, 05:02

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.

January 30, 2013, 18:46	Is Mean Free Path useful in determining mesh resolution?	#1
pt39 New Member Join Date: Jan 2013 Posts: 3 Rep Power: 13	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.

February 1, 2013, 11:11		#3
pt39 New Member Join Date: Jan 2013 Posts: 3 Rep Power: 13	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 11:30.

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] Mesh around ship with appropriate free surface refinement	Hannes_Kiel	OpenFOAM Meshing & Mesh Conversion	46	October 4, 2019 07:28
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 08:52
[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

January 31, 2013, 16:08		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,699 Rep Power: 143	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.

February 2, 2013, 05:02		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,699 Rep Power: 143	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.