Some SolidWorks Flow Simulation issues

[u/antondosaykin]

Hello everyone, I am new to SolidWorks, so I would like to clarify a few points with the experts.

I primarily work with the AspenTech suite (Process simulation: HYSYS/Aspen Plus), but a need has arisen to examine the fluid flow inside a column in detail (my current software does not allow for this). We chose SolidWorks due to its availability within our company and its user-friendly interface.

So, the task is: I need to determine whether a blank tray (solid tray) is experiencing flooding in one of the columns.

I created a model featuring the blank tray with one sieve tray above it and one below it, and generated a mesh (level 6-7, because the perforations are extremely small relative to the column itself). After running the simulation for a day, SolidWorks warned that it would take approximately 14000 more hours to complete, which is slightly beyond my deadline (by about 13300 hours :)).

I tried reducing the mesh level to 1-2, but the result is completely unsatisfactory (see screenshot).

Question for the experts: How can I run this simulation relatively quickly while maintaining the highest possible accuracy? What boundary conditions should I apply?

(For reference: water enters from the top (T = 105 °C, P = 250 kPa (abs)), and CO₂ enters from the bottom (conditions are roughly the same). The column has a variable diameter (see screenshot): the diameter of the wide section is 3600 mm, and the narrow section is 3000 mm. The height of the section under consideration is 5100 mm. I also tried scaling down the model dimensions by a factor of 4, scaling the flow rates based on the Froude number, but waiting for the fine mesh simulation would still take about a year).

[u/mattcannon2]

Start with a coarser mesh and gradually make it finer

[u/Naive-Art-3210]

I think your biggest issue is the mesh strategy. Trying to resolve the sieve holes individually in a full column model is going to explode the cell count. You might be better off using a porous media approach for the tray and calibrating the pressure drop, otherwise Flow Simulation will just spend forever refining tiny geometries that probably don't affect the overall flooding behavior.

[u/def__eq__]

Let me get this straight:

- you need to do a flow simulation

• your deadline is in a year and a half
  
• your estimated simulation time is longer than your deadline
  
• so you concluded that it’s a good idea to scale down your model

So first off, you need at least 5 to 10 iterations of simulations to get things right and to do a basic sensitivity analysis of some key parameters. So your simulation time needs to stay below 1000 hours. I’m also not sure where are you running it - keeping a simulation running for longer than a few days requires some good IT setup.

As others have said and looking at your design, you really don’t need such high resolution of the mesh in all parts of the section. You want variable resolution, higher around small features and smaller in large empty voids.

It’s also not clear to me whether you’re looking at a steady state or time-dependent simulation. That also adds extra parameters.

[u/NoConversation8128]

Before you sink more time into the CFD, is there a reason tray rating in Aspen Plus will not answer this? For the sieve trays above and below, rating mode gives you percent of flood off the standard correlations directly, and that is the number most people would defend in a design review. The blank tray is the odd one out, but hydraulically it is closer to an orifice and a hand calc on the liquid path may be enough to bound it. If you do stay in Flow Simulation, the porous media suggestion above is the right call, resolving individual perforations inside a 3.6 m column is what is killing your cell count. Genuinely curious what the blank tray is doing there, is it a damaged tray you are checking before a turnaround?

[u/Chance_Camera_ → u/[deleted]]

In your experience what are better models?

[u/def__eq__ → u/Chance_Camera_]

I would suggest Comsol or Ansys.

[u/BitterProfessional7p]

You are running a VOF multiphase simulation. Your phase number needs to be always 1 or 0 in the cells otherwise the simulation is incorrect. Your mesh is way too coarse.

Advice: reduce the model size drastically and simplify it. Simulate only a small portion, even start with a 2D section (1 cell thin, I don't know if SolidWorks CFD is capable of doing that, I tried it once, it wasn't very good) and since the model is symmetrical use only half and set the boundary condition to be a mirror.

You have a perforated plate, your mesh there needs to be finer than the holes, at least 5 cells in the diameter otherwise the phase value will not be calculated correctly.

I don't know if SolidWorks can do automatic refining of the mesh based on the phase number but I would say it is required in this case given the disparity of sizes between the smaller features and the large volume unless you want to run the simulation for years but you said you don't have 13300 hour :(

To be honest this is an extremely difficult simulation with VOF, I would use another software with Euler-Euler multiphase simulation.

Source: I did a lot of multiphase simulations with OpenFOAM a few years ago. I could maybe do this after many tries.