[JulienV]

Dear Ansys Cfx users,

I am currently running cfx simulations and I need to reach the pressure loss values generated in the whole geometry. (Please find the attached file representing the geometry).

I tried two different ways to get the values.

1st Method:
I am reading the value in cfx-post calculated as : areaAve(Total Pressure)@outlet - areaAve(Total Pressure)@inlet. Because the pressure losses are the sum of the static and the dynamic pressures as well as the "Total Pressure" is in cfx post, I thought this was the right method. However, this way of calculating the head losses is not satisfying because I get very high values.

2nd Method
I found to reach other values of the pressure losses by calculating 1/2*rho(V_outlet²-V_inlet²)+rho*g*deltaz+(P_statique_outlet-P_static_inlet) with:
V_outlet=areaAve(Velocity)@outlet
V_inlet=areaAve(Velocity)@inlet
P_static_outlet=areaAve(Pressure)@outlet
P_static_inlet=areaAve(Pressure)@inlet

I am confident in the way I mesh my geometry so I do not think the mesh is the problem.

My questions are:
- What exactly gives the "total pressure" value in cfx post ? On what it physically depends?
- What do you think about the two different methods ? What else do you propose?

Thank you for your help.

Julien

[ghorrocks]

Total pressure is p+0.5*density*velocity^2, which is the standard definition of total pressure.

You say the values are high - why do you know they are high? Are you comparing to experimental results? Or is the total pressure at the outlet greater than the inlet? Or something else? I can't comment on the validity of your methods until I understand what you are comparing to.

I am confident in the way I mesh my geometry so I do not think the mesh is the problem.

I cannot count the number of times I have heard statements like that. Likewise, I cannot count the number of times I have replied with "unless you have done a mesh sensitivity analysis to check your mesh you are just guessing. It is the cause of accuracy problems in the majority of simulations done by people inexperienced in CFD".

[JulienV]

Dear Glenn,

Thank you for your answer.

1) I say the values given by the 1st method are too high because there are around 1000 Pa where the 2nd method gives around 500 Pa and the ie idel'cik theory gives around 500 pa too. How could you explain the difference?

2) In this expression : p+0.5*density*velocity^2, what is p? This is the static pressure but how it is determined? on what it depends?

3) What do you think about the 2nd method?

4) I have already done a mesh sensitivity for this case

5) What would you do in order to reach the pressure loss values?

Thank you.

Julien

[ghorrocks]

1) Is the simulation constant viscosity? Density? Is gravity activated? Is it just a straight forward incompressible simulation with no unusual physics?

2) p is static pressure. It is a solution variable, so is one of the variables CFX is solving.

3) See answer for Q1.

4) Please mention important things like that.

5) I do not understand this question.

I have two general comments:
1) Your outlet is quite close to the bend in the duct and therefore is likely to have a recirculation present a the outlet. This complicates things significantly, including the calculation of pressure drops. You might want to move the outlet boundary further downstream to get it away from these effects.
2) Some experimental pressure drops over features place pressure tappings at a specific location, such as for oriface plates. If you are comparing to experimental values you should use pressure values taken from these points, not area averages.

[JulienV]

Dear Glenn,

In my problem, I have constant viscosity and density and this is an usual physics simulation.

I will try to displace the outlet and see.

Thank you

[ghorrocks]

I assume you have not activated gravity and so the hydrostatic component is not relevant.

The key difference boils down to average(V^2) does NOT equal (average(V))^2. Your approach 1 uses average(V^2) in the form of total pressure, but approach 2 uses (average(V))^2.