[dasdasdiedie]

I want to analyze flow around airfoil. But i couldn't be sure about how reference pressure must be defined. I define velocity inlet giving cartesian velocity and 0 gauge pressure. I set reference pressure 1 atm for this case. I think this means air around airfoil has 1 atm static pressure + dynamic pressure due to velocity. But in reality air is still and airfoil moves with velocity. Airfoil gains kinetic energy due to engine in aircraft. For slow velocity this counts for small change in refenence pressure. Static pressure change can be neglected maybe. But when flow is compressible dynamic pressure increases too much. Should i set reference pressure same as old case or should i find static pressure using compressible flow equations. For example if i set 0.7 mach velocity inlet for sea level simulation static pressure becomes 0.7 atm. One of the tutorial i saw, airfoil simulation was compared with wind tunnel data they used this 0.7 atm reference pressure for farfield pressure. Does simulating wind tunnel case and sea level real life situtiation case make difference ?

[LuckyTran]

The reference pressure can be set to almost anything. The reason for setting a reference pressure is strictly numerical precision. The best reference pressure (for numerical accuracy reasons) is to set it to whatever the most-probable pressure is, so that most of the gauge pressures in the domain end up being small. If your airfoil is small relative to the computational domain, you'll more often set the reference pressure to the ambient pressure because the pressure will be mostly ambient throughout the domain except around the airfoil. Even if it's a very high speed airfoil, if most of the flow domain is ambient, then it's better to set the reference pressure to the ambient pressure.


Either way, it's numerical precision. It doesn't affect the underlying physics.

[dasdasdiedie]

Thank you for explanation. But I am interested in underlying physics because i am trying to convience myself. Assuming if we had pressure inlet boundary condition wouldn't it effect solution. If i understood it right navier stroke equations are solved for pressure gradients not for pressure itself that's why reference pressure doesn't effect the solution. Within this way of thinking setting up pressurized inlet with respect to outlet creates pressure gradient and it drives flow. But if velocity inlet boundary condition for inlet and 0 gauge pressure for both inlet and outlet boundaries was setted there would be no pressure gradient based contribition to the flow. There will be only reference pressure added to whole domain.

Originally Posted by LuckyTran

The reference pressure can be set to almost anything. The reason for setting a reference pressure is strictly numerical precision. The best reference pressure (for numerical accuracy reasons) is to set it to whatever the most-probable pressure is, so that most of the gauge pressures in the domain end up being small. If your airfoil is small relative to the computational domain, you'll more often set the reference pressure to the ambient pressure because the pressure will be mostly ambient throughout the domain except around the airfoil. Even if it's a very high speed airfoil, if most of the flow domain is ambient, then it's better to set the reference pressure to the ambient pressure.


Either way, it's numerical precision. It doesn't affect the underlying physics.

[LuckyTran]

Originally Posted by dasdasdiedie

But if velocity inlet boundary condition for inlet and 0 gauge pressure for both inlet and outlet boundaries was setted there would be no pressure gradient based contribition to the flow. There will be only reference pressure added to whole domain.

A velocity inlet and outflow does not constrain the pressure gradient. The pressure field will be whatever it needs to be. And after you solve it, you will find that there is indeed a pressure field/gradient.

The reference pressure is purely a gauge. The reason it exists is when dealing with cases where there are small changes in pressure throughout the domain, because computers have limited machine precision. Using a good reference pressure enables the solver to solve for small changes more accurately. The reason for this is due to floating point representation of numbers, not Navier-Stokes or anything physical laws of the universe.

There is no need to debate. Solve your case using different settings of the reference pressure. Unless you did something very wrong, you'll end up with the same solution.