# BC for compressible flows

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

 February 17, 2013, 09:17 BC for compressible flows #1 New Member   Lipo Wang Join Date: Dec 2012 Posts: 14 Rep Power: 6 Dear all, A basic problem, which I thought should be quite simple, puzzles me a long time... For compressible simulations (still subsonic, Mach is about 0.7) of flow passing a square block, the mesh is Cartesian and the scheme is MacCormack. I tried different boundary conditions of the pressure on the block surface, for instance: extrapolation from two internal points (as said in Anderson's book), zero gradient pressure (i.e. p_surface=p_1), or from the continuity eq. to update pressure etc. But none of them can work satisfactorily and finally the density runs to negative around the corner. Could anybody give me suggestions? Many thanks.

 February 18, 2013, 07:54 #2 Senior Member   duri Join Date: May 2010 Posts: 160 Rep Power: 9 Just hold the pressure and density from the nearest cell on the wall surface. Make sure velocity components are rotated properly to make zero normal component on the wall (for Euler solver).

 February 18, 2013, 08:03 #3 Senior Member   andy Join Date: May 2009 Posts: 129 Rep Power: 10 The exit boundary condition is usually tied to some extent to the inlet boundary condition. For example a "total pressure" condition at the inlet and a "static pressure" condition at the exit. What is your inlet condition? Zero gradient on pressure is usually fairly stable even though physically incorrect in most situations. Are you violating a stability limit during the initial bang?

February 18, 2013, 20:09
#4
New Member

Lipo Wang
Join Date: Dec 2012
Posts: 14
Rep Power: 6
Dear Andy,
Thanks. The outlet is given static pressure and the inlet is from extrapolation of two interior points' pressure, because I specify the inlet velocity (both direction and magnitude). From the visualization I found around the corner a lot of fluctuation. I think it is mainly from the corner and solid BC, but much less relevant to inlet and outlet, because the 'wrong' region is far from them. Am I right?

'Are you violating a stability limit during the initial bang ', I am not quite clear about this point. Do you mean that the initial value still need to be reasonable? I thought even an initial field is not 'good', it will evolve toward the final solution (the problem is time-dependent). Also no way to have a good initial field.

Quote:
 Originally Posted by andy_ The exit boundary condition is usually tied to some extent to the inlet boundary condition. For example a "total pressure" condition at the inlet and a "static pressure" condition at the exit. What is your inlet condition? Zero gradient on pressure is usually fairly stable even though physically incorrect in most situations. Are you violating a stability limit during the initial bang?

February 18, 2013, 20:15
#5
New Member

Lipo Wang
Join Date: Dec 2012
Posts: 14
Rep Power: 6
Dear Duri,
Thanks. I tried different BC, including yours (let pressure gradient =0 and the wall temperature is fixed.) But always failed. One observation may be helpful: I reduced the inlet velocity a bit, it can work. Do you have any idea about the problem?
If the mesh is very coarse, is it also OK? (I found from Anderson's book that the grid Re should be <30~50, but my case is much larger ~1000)

If you have a similar code to let me share? If yes, I will greatly appreciate!

Quote:
 Originally Posted by duri Just hold the pressure and density from the nearest cell on the wall surface. Make sure velocity components are rotated properly to make zero normal component on the wall (for Euler solver).

 February 19, 2013, 02:40 #6 Senior Member   duri Join Date: May 2010 Posts: 160 Rep Power: 9 Are you solving Euler equations or NS equations. Whether implicit or explicit. Time stepping etc. Give more details for better understanding of the issue. And also what kind of boundary condition at inlet and exit (characteristics or physical).

February 19, 2013, 03:40
#7
New Member

Lipo Wang
Join Date: Dec 2012
Posts: 14
Rep Power: 6
I am solving the NS equations, using the explicit MacCormack scheme. Time step is from the stability criterion and much smaller time step was also tried, but still diverge.
Because flow is subsonic, inlet BCs are: velocity (magnitude and direction) and temperature are given and the pressure is extrapolated; for outlet, the static pressure is given and u,v,w and T are extrapolated from two interior points along the flowing direction.
For the corner points in the channel, I tried many different possibilities for pressure: like average of two adjacent surface points', equal to the diagonal cell point's pressure etc. Results are always the same.

Quote:
 Originally Posted by duri Are you solving Euler equations or NS equations. Whether implicit or explicit. Time stepping etc. Give more details for better understanding of the issue. And also what kind of boundary condition at inlet and exit (characteristics or physical).

 February 21, 2013, 02:56 #8 Senior Member   duri Join Date: May 2010 Posts: 160 Rep Power: 9 BC's and time stepping are seems to be correct. It could be the problem with code also. Please do the following to ensure there is no bug in the code. 1. Simple rectangular duct with symmetry on top and bottom should work, it will give almost zero residual make sure it doesn't blows up later. 2. Full supersonic flow like flow over ramp. (if this fails problem is with time stepping and possibly scheme). if these two are working then problem is certainly with subsonic boundary conditions. Don't extrapolate from two interior points just use the value from the nearest cell. First order bc is sufficient enough to start with.

 February 21, 2013, 05:00 #9 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 3,681 Rep Power: 41 some time ago I worked on compressible flows using an unstructured-based code. I used to solve the continuity equation at wall on a non-symmetric FV, then the temperature and finally I computed the pressure at wall

 February 21, 2013, 11:53 #10 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 487 Rep Power: 12 The flow around a square block will probably be supersonic if the freestream Mach number is Mach 0.7. I'm not sure the MacCormack scheme is stable for the corners of your block. You may need to add artificial dissipation. The fact that it works if you lower the inlet velocity seems to indicate this. You've mentioned "square block" and "channel". If the square block is in a channel at Mach 0.7 then the flow may be choking. Lowering the inlet velocity would also help this.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Josh Main CFD Forum 5 June 15, 2013 07:13 luftraudi Main CFD Forum 0 July 17, 2012 06:35 Maarten de Jong Main CFD Forum 7 April 30, 2012 02:23 vishyaroon Main CFD Forum 0 April 15, 2010 14:24 Abhijeet Vaidya Main CFD Forum 10 November 18, 2002 09:21

All times are GMT -4. The time now is 05:07.