I'm running a transient simulation in a closed system (no inlets or outlets).
I've noticed that if my fluid is modeled as an ideal gas, the initial condition that I use for pressure is applied. I verify this by checking the pressure in the backup file at 0 iterations.
If the fluid is incompressible, however, I notice that the initial condition I set for pressure is not applied. If I set a constant initial condition, that condition is replaced by a zero field for initial pressure. If I set a variable initial condition for pressure, my initial guess is shifted by some amount.
What's going on?
Here's a summary of the behavior you should expect:
1. If the density depends on pressure (say for an ideal gas) and you set an initial condition for pressure for a transient run, then you should see exactly that pressure in the backup file at zero iterations.
2. If you run the problem with incompressible fluid(s), then there isn't a transient term for density to tie the initial pressure level to the subsequent behavior. Therefore, CFX-5 will enforce the reference pressure level at the default location. You can control the location of the pressure reference point and the reference pressure level by setting the expert parameters `pressure reference node` and/or `pressure reference value`.
If you set a constant non-zero initial condition for pressure, you would still see a uniform initial pressure of 0 [Pa] for an incompressible case, since that would be consistent with the pressure at the reference node.
If you want the initial pressure level you set to be enforced for an incompressible fluid, you could either set the `pressure reference value` to the desired value as an expert parameter or you could just specify the reference pressure in the domain definition to be the desired value.
For a variable initial condition, the pressure field will be shifted by a constant amount so that the pressureat the reference node will equal the pressure reference value.
If you want a variable initial pressure field to be enforced, you have two options:
(a) Run the problem with the fluid specified as an ideal gas
(b) Set the problem up with incompressible fluid(s) and check the spatial coordinate for the node selected as the reference node for the pressure level (this will be echoed in the output file). Calculate the pressure at that location from your initial pressure expression, and set the pressure reference level to that value using the expert parameter `pressure reference value`.