CFD Online Logo CFD Online URL
Home > Forums > FLUENT

farfield Vs symmetry boundary condition

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

Like Tree1Likes
  • 1 Post By Jason

LinkBack Thread Tools Display Modes
Old   October 21, 2005, 12:39
Default farfield Vs symmetry boundary condition
Posts: n/a
Dear CFD enthusiasts,

i am trying to simulate flow around a car body. The car is placed in a box where flow is generated. If i use pressure farfield condition on the two side walls and cieling , the energy equation gets activated , since this being a compressible flow, and solution diverges saying "Divergence detected in AMG solver: Temperature".

The only option i think is to have a symmetry boundary condition. since that has zero slip condition. No fluxes in normal direction.

what do u guys think about this ? Does having a symmetry boundary condition simulate what is happening on the road around a car....or pressure farfield is more accurate???

Regards, Rajat
  Reply With Quote

Old   October 21, 2005, 13:53
Default Re: farfield Vs symmetry boundary condition
Posts: n/a
Pressure Far Field shouldn't ever touch a wall BC (your floor is presumably a wall). Also, what are you using for inlet/outlet BCs. When you use Pressure Far Field, typically you use it for all of your flow BCs (inlet, sides, and outlet), but you have to make sure that the BC is VERY far from any influencing bodies (probably 10 car lengths ahead, and 10 to 20 car lengths above and to the sides, and 20 car lengths downstream). You could use the symmetry BC, but again, since you're not really modeling a symmetry condition, you have to make sure your flow domain is much larger than your blockage so that you're not creating interference effects between "the cars" created by the symmetry BC.

I would recommend using a pressure inlet for the sides and cieling. You can avoid the "Reversed Flow in XXX cells" by having tapered walls with the domain expanding in the direction of the flow. Then your ceiling and side walls get a Pressure Inlet BC (but change the flow direction from "Normal to Boundary" to "Components", and assign the correct vector for the flow direction). That's assuming you're using the Pressure Inlet BC on your main inlet. If you're using a Velocity Inlet BC then you should apply that to the sides and ceiling instead of the pressure inlet. Your BCs are still going to have to be a decent distance from the vehicle, but a Pressure Inlet BC is much less sensitive to that than a Pressure Far-Field.

Since you're probably not simulating your car going 360+km/hr, then you don't need to incorporate the ideal gas law. If you're not looking at Heat Transfer, then you don't need the energy equation at all. Also, you're probably using the segregated solver. You should set your limits (Solve->Controls->Limits) so that you're not letting your pressure go out of whack. I use Pmax = Pstatic + 2*Pdynamic and Pmin = Pstatic - 3*Pdynamic. This gives the solver enough room to go a little out of the realistic range without going off into some rediculous pressures that just lead to divergence.

Hope this helps, and good luck, Jason
justsmile2007 likes this.
  Reply With Quote


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
inlet velocity boundary condition murali CFX 5 August 3, 2012 08:56
Mixed/Robin boundary condition aaev OpenFOAM Bugs 2 December 15, 2011 15:03
Slip boundary condition what is inside normunds OpenFOAM Running, Solving & CFD 2 June 4, 2007 06:45
Rotating interpolated boundary condition hani OpenFOAM Running, Solving & CFD 0 July 4, 2006 07:09
Regarding SYMMETRY boundary condition Praveen Athanki FLUENT 0 March 27, 2000 13:30

All times are GMT -4. The time now is 04:45.