Absolute/relative pressure offset - CFD
Hello everyone,
I am writing on the forum because I have some doubts about the absolute/relative pressure setting in the CFD analysis of a duct. Specifically, I need to evaluate the pressure drop in a duct where I impose the inflow, using the appropriate condition with velocity profile, and the outflow has zero pressure.
If you set the pressure offset to either 101325 Pa or 0 Pa, you will always get the same result. I would like to note that the fluid conditions are at atmospheric pressure, and the outlet condition is at 0 Pa. Therefore, I ask if I need to set other conditions to obtain the pressure drop in this circuit, or if the way I am setting it up is correct in my case (i.e., with a 101325 Pa, or 0 pressure offset), or if other settings are necessary because is not clear if the zero pressure at the outlet take into account the absolute pressure or not.
I'm doing all of this simulation into SimLab 2022.3 and I'm using the solver setting with absolute pressure offset. The fluid is water.
Tanks to all
Find more posts tagged with
The point is that if I set or not the absolute-pressure-offset, the inlet pressure is the same in both case (abs pressure = 0 Pa and p_out=0 or abs pressure = 101325 Pa and p_out=0). Last check that I can do is to set 101325Pa at the outlet with 0 as offset.
Altair EmployeeThe point is that if I set or not the absolute-pressure-offset, the inlet pressure is the same in both case (abs pressure = 0 Pa and p_out=0 or abs pressure = 101325 Pa and p_out=0). Last check that I can do is to set 101325Pa at the outlet with 0 as offset.
I believe the results are also consistent with the input file values for the boundary conditions.
For example:
absolute-pressure-offset = 101325, outflow pressure = 0, resultant pressure difference = 300
>> Internally the solver sees outflow pressure = 101325, solver sees inlet pressure is 300 + 101325 = 101625
>> Results will represent the inlet pressure as 300 and outlet pressure as 0
The absolute pressure offset is only seen internally by the solver
(This is what I meant in the earlier comment, using absolute pressure offset = 0 is easier for me - to avoid the confusion between what the solver sees and what the user sees.)
Altair EmployeeHi,
“Absolute pressure offset” is used to convert to absolute pressure units. By default, this value is set to zero and the pressure values in the simulation is gauge pressure. By using Absolute Pressure offset value of 101325 Pa, the values are converted to Absolute. This is used for ideal gas and isentropic density types.
For pressure drop analysis in a duct, you will not see any effect of this parameter.
The value for the absolute-pressure-offset is added to whatever pressure values are specified within the input file. For example, if you specify absolute-pressure-offset = 500, and you specify pressure = 125 at the outflow, the solver actually uses 125 + 500 = 625 at the outflow.
In general, the pressure difference is calculated - the reason you see the same difference whether you use 0 or non-zero for the absolute pressure offset. That is when you are using constant material properties - where the density for example does not depend on pressure. You would specify the material properties consistent with whatever is your basic operating pressure.
If the density, for example, does depend on absolute pressure - when you're using isentropic density or ideal-gas density, then we need to make sure the solver is seeing the absolute pressure values. If the outflow is truly standard atmospheric pressure, then we need to use pressure = 0 with absolute-pressure-offset =101325, or pressure = 101325 with absolute-pressure-offset = 0. I prefer the latter so as to avoid confusion in setup and results. (I suppose one could use some other combination of outflow pressure and absolute-pressure-offset such that the solver sees the desired absolute pressure value, but that to me would only create more confusion.)