How does your mesh look around the tubes? It seems to me like you're starting out with too much detail. I would try to simulate just one of these bundles, maybe even just a 2D analysis and increase in complexity from there.
I would tend to agree with Amit - at least use symmetry along the central plane if not a 2D simulation to start. Then use the fact that you just cut your number of cells in half to make sure your cylinders are refined enough (using a local mesh).
With curved surfaces being approximated as rectangular cells your mesh resolution is going to make a lot more difference in drag than your surface roughness on those cylinders.
I created a local mesh to refine it around the cylinders a lot more, as well as testing using half-symmetry, and then quarter-symmetry (and reduced the inlet flow accordingly). I used a 3d comp. domain because the 2d was giving me some computing/memory issues for whatever reason. From these two tests, I get numbers that are way off from 6" of head loss again. However, there's an issue when I display the trajectories that could be related to this problem: the trajectories don't go all the way through the system, only up to a certain point. See below pics for the setup:
The local mesh around cylinders:
Trajectories that stop short:
Any idea of what's going on, or what my options are from here?
If you're looking to compare effects of roughness you need a LOT finer mesh. If you look at the mesh without the parts I couldn't even tell that those are round pins and not square/rectangular. Until your model looks just like reality the roughness is irrelevant. On flat surfaces it would be useful, but when your circle looks like a square the rectangular approximation makes your roughness equal to your mesh roughness.
In the Flow Trajectory tab what is the length limit of the paths shown? How big is this model actually? (.001" rods, 1" rods, ?)
When you setup symmetry did you use fully 1/2 or 1/4 of the model? The highlighted yellow region does not appear to be 1/2 of the thickness.
I'm not trying to compare the results of the different roughnesses, just a constant roughness of 5 microinches on the cylinders. How can I make the mesh recognize the curvature even more, because the mesh levels are already pretty high, and Solidworks can barely calculate the mesh/run the simulation as it is. The local mesh settings around the cylinders are currently:
- Small Solids Features Refinement Level: 5
- Curvature Refinement Level: 5
- Curvature refinement criteriod: 0.389 rad
- Tolerance Refinement Level: 5
- Tolerance refinement criterion: 5.85in
Just "Refine fluid cells" and "refine partial cells" are checked and are Level 5
How many cells are you generating currently?
I would likely alter your basic mesh settings so that the mesh around the rods has the same size in both directions (look like squares instead of long thin rectangles). You are creating a lot of cells in the bulk flow region that you may not need if the flow around the rods is your primary interest.
Unfortunately, it might also benefit to put reference planes in the center of your rods so that you know they are all resolved the same. It would be a royal pain to add them, but the more effort you put into setting up the initial mesh the easier it is for the software to get the answer you are looking for. Many of my models can take several full days to create all the BCs, ICs and local meshes but when it takes a day for each configuration and you're comparing a dozen changes it gets easier to justify the time up front.
Scott, your mesh looks very rough. Can you post a screenshot of a mesh only cut plane, and please be sure to toggle off "use cad geometry" in the cut plane definition. I think you may be surprised at what your solids actually look like.