I pick this thread from one of my recent experiences. Typically, first order advection schemes (ADV1) and second order accurate advection schemes (ADV5) would produce different results because of artificial viscosity in ADV1. But would these results be very much affected ONLY while simulating distributed resistance, which models a negative pressure gradient zone? Or do these schemes always produce significantly different results for ALL types of physics, viz. incompressible turbulent flow, heat transfer, compressible flow etc.?
Regards
OJ
We would recommend switching away from ADV1 and to ADV5 for many purposes now. Standard incompressible flow should be OK but ADV5 will be better for compressible and pressure driven flows, those with resistances as you rightly say and also for many heat transfer calculations now too.
Some points to consider here:
Some points to consider here:
You are correct about the pressure drop issue.
Based on the dimensions you mentioned, the model should be amenable to analysis with Adv5
Hi:
These are good points.
One thing about incompressible flow (unless you are concerned or on the lookout for cavitation), is that the pressure is not a thermodynamic quantity and is purely mechanical in nature. So, when density is fixed (frequently a good idealization), the boundary condition for pressure is largely a relative value and the interesting result is the variation of pressure itself (such as a drop or a rise) within the model.
In the end, it depends on your judgement and the assumptions you want to make regarding the material properties when setting up the problem.
Let me try to be more clear.
I am not really interested in the head losses in the nozzle. I am more interested in the change in pressure as the water flows from a larger diameter area (green) to a smaller diameter area (red). This is water at 440 F and 1018 psi absolute. The system is a closed system (so the outlet does not dump to the atmosphere) so there is really no place that I can use a P=0 Boundary Condition.
Is the Boundary Layer meshing still a concern in this case?
As i mentioned previously, for constant density flow the P=0 boundary condition is purely a relative value- with constant density (which is an excellent assumption for a fluid like water) you will get the same velocity field with P=0 or with P=1000psi as a boundary condition while maintaining the same flow rate.
Moreover, with a constant density you should get the same pressure variation regardless of the pressure boundary condition value at the exit as long as you have the same flow rate at the inlet.
So, for example, suppose you put P=0 psi(gauge) at the exit and find that the pressure solution at the inlet is 17 psi (gauge). If then you assign P=1000 psi(gauge) at the exit and re-run the problem with the same flow rate as previously, you should get a pressure of 1017psi (gauge) at the inlet as part of the solution.
If, however, you are trying to model density changes due to pressure, you have to run compressible flow, which is entirely different from a constant density assumption. At this stage, you have to decide from apriori knowledge if the flow is sub-sonic or supersonic. Most water based analyses (except for water-hammer) assume that the density is only a function of temperature at best and that the flow is essentially incompressible., so this is likely not your concern, but i may stand corrected.
Finally, if you want to let density change with temperature as well because you are running heat transfer, then select as Variable for the water material and be sure to prescribe appropriate reference pressure and temperature for the environment settings.
The boundary layer mesh is still very important and critical to achieving a good pressure drop through pipes/valves, orifice plates, etc.
Like the earlier post said. Leverage the mesh adaptation and set your Y+ value to 30-50 for K-e. If you wanted to try using SST then I would change my strategy since the physics at the wall are modeled differently. Use 2015 since I am finding adaptation works really well in this version. Consider this rev3 of our mesh adaptation development.
If you toss your share file up here you might be surprised what sort of work people on this forum will do/show you with your model.
Cheers!
The Archive file can be downloaded from the link below. If anyone wants to take a stab at it, I would greatly appreciate it. Real world and hand calcs put the pressure difference between the green and red sections (screenshot in earlier post) at 16.7 psi, but I am getting 20 psi in the simulation.
Thanks!
https://www.dropbox.com/s/6fz2lyr46t9xuog/fluent-demo2_help.cfz
Can't find what you're looking for? Ask the community or share your knowledge.