[rizwan4081]

Greetings.
I am new to Ansys Fluent. I am doing an analysis where I am analyzing the flow over a car in a tunnel. I have the Student version of the software with a limitation on the number of mesh elements of a max being 512000 cells. I would like to know how to calculate the minimum element size of the mesh?
The tunnel is 500 meters and by default the mesh element size is 25 meters, But I want to know if there is a way to calculate a minimum size so as to guarantee the convergence of solution?

[vinerm]

If it is a single car in a tunnel, then you do not need 500 m of tunnel. At most, the car is 4.5 m long. That means that you require about 10-12 m upstream of the car and about 40 m downstream. In total, 50 m should do.

As far as grid convergence study is concerned, that you have to do with at least three levels of meshes. Considering that you have limitation due to academic license, I'd recommend to use fine mesh close to the car and then grow it fast enough so that by end of tunnel the mesh cell is big enough to diffuse reflections. If diameter of tunnel is around 10-12 m, then the mesh cell near the outlet can be as large as 0.5 to 1 m. But with 50 m tunnel, half a million cells would not be bad; you would manage to get good resolution.

[rizwan4081]

Thank you for your reply.
I totally understand about the difference in the size of the carbody and tunnel.
I would like to know if there is anyway to find a minimum element size for meshing that depends on the length of the tunnel so that I could modify the tunnel. The reason for selecting the 500m tunnel is due to the presence of JEt fans inside.

[vinerm]

The size of the smallest cell is not defined by the size of tunnel but by Re number of the flow. If the objective is to study the flow around the vehicle, then it is the region around the vehicle that needs to be resolved. If the objective is to study the flow field in a tunnel due to presence of car(s) and ventilation fans, then car is not the most important part, nor is the jet. You can have more or less uniform mesh. If objective is to study the drag on the car, then you can almost totally neglect the tunnel size as well the ventilation fan, until and unless the fan is in the proximity of the car and car is very close to either the entry or the exit of the tunnel. In this case, mesh at the car surface has to be fine enough so that you get of the order of 1.

[vinerm]

The very first thing to decide about cell size is the objective. Assuming that the objective is to determine the drag on the vehicle, assume that the vehicle is made up of flat plates. Now, based on the Re number (Re number has to be based on the length along the car, starting from its front and not based on the diameter of the tunnel), you can get a drag coefficient from graphs, such as, Fig.1.8 from

https://www.researchgate.net/publica...S/figures?lo=1

Based on this, you can determine wall shear stress, since it is related to drag coefficient. is a function of this wall shear stress. Assuming that you need a around 10, you can determine what should be the value of y, i.e., half the height of the first cell adjacent to the wall. Every other cell in the domain can be larger than this cell.

[rizwan4081]

Let me explain my problem.
The analysis I am doing consists of long tunnel in which there is a vehicle carrying hazardous goods. One of the vehicle is fire and as a result there is production of smoke and other gases. Now I need to check if the ventilation is sufficient enough to push this smoke out overcoming any baclayering phenomenon. To do so I simplified the tunnel length considering the most critical section alone. Unfortunately I have only the student version of the software ansys fluent, thus I am confused with what mesh size I could take and find a relation relating mesh size and length of tunnel, so that i could perform my analysis on the software with good convergence of results.

[vinerm]

If the objective is analyzing the flow of the smoke, then the capability you have is more than enough. You can use more or less uniform mesh. Even if you keep length of each cell to be around 0.25 m along the length, you can still use enough cell across the area of the tunnel. I don't know the area of the tunnel. Assuming it has 6 m diameter, you have option to put 250 cells across the area, i.e., 250 faces covering an area of around 28 sq.m. That would be more than enough for smoke flow.

[rizwan4081]

Ah ok. But how did you determine the length of each cell to be 0.25m? The tunnel Length geometry is this:
Tunnel Length 500m Height 7.8m
Vehicle inside the tunnel: length 75 meters

[vinerm]

This is not based on any formula, just experience or gut feeling. You need at least 80-100 faces to cover the area of the tunnel cross-section. With 0.25 m, you get 250. That's more than enough. You can reduce it to 125 and reduce cell size in length direction to 0.125 m. But gradient would be low along the length. Hence, you can use bigger cell dimension along the length but it has to be smaller in other two directions to resolve the gradients.

[rizwan4081]

Earlier you had explained about the Flow depending upon the reynold number. Reynolds number is a function of Characteristic Length, Is this length the minimum size of mesh?
IF not what is used it for and how can one determine it?

[vinerm]

Reynold number is based on length and velocity scale but these scales could come from anywhere. For flow over boundaries, this has to be length of the wall in the direction of the flow. For flow through ducts, this is usually hydraulic diameter of duct. For the analysis of smoke flow, you can use the latter, i.e., based on hydraulic diameter of the tunnel. If the tunnel cross-section is reduced or increased in size, keeping the flow through it same, then Re will increase or reduce, resp.

For a higher Re, smaller mesh cell would be needed because Re is calculated using inertial and viscous strengths but it signifies the ratio of integral to viscous length scale.

[rizwan4081]

Thank you for clearing my doubts instantly. Is there any way theoretically we could simplify the geometry or even scale it accordingly in relation to the minimum characteristic length. The only issue of what I have is further reducing the length of the tunnel so as to obtain less than 512000 cells.

[vinerm]

The size of the tunnel should not be scaled on the basis of characteristic length scale, rather on the basis of diffusion or uniformity of smoke. E.g., if smoke distribution across the cross-section of the tunnel does not become uniform for 200 m, then 200 m is the minimum distance required to be modeled from the source of smoke. A quantitative value of this can be determined using similarity laws but if you have never studied those, then it would be too much effort for one case, until this is your Masters or Ph.D. work. I'd suggest you use 500 m, coarse mesh of 150000 - 200000 cells and then see if the smoke distribution becomes uniform by a certain distance. If it does, then you can shorten the domain length and remesh with a finer cell size for the final simulation.

[rizwan4081]

Greetings.
Do you have any references for performing the Grid Convergence test?

[vinerm]

There are a lot of references available on-line but you don't need any. Since you are limited by the license, you should try with 200000, 350000, and 500000, and then observe a few particular field values, such as, area averaged mass fraction of smoke at outlet to determine the sensitivity. You just need to find out how much the solution varies across various meshes. If the variation is within acceptable limits, then you can go ahead with the coarsest mesh that gives acceptable results. Usually, the acceptable limit of variation is 1%, however, that is only a number. Even if the results vary by 2-3% from 350000 to 500000, then you can use 350000.

[rizwan4081]

Greetings.

Thanks for your advice I got good results with the mesh strategy you advised.

I have a few doubts in the Solution part of the Software. I am performing a transient analysis for visualizing the fire. I need to obtain a simulation for atleast 10 minutes How do I determine the Time step, Number of Iterations. Also how does changing Time step affect the result?