Dear SolidWorks Forum Community,

I have to ask you once again for your opinion. I will have to perform an external flow analysis and I thought that the best thing is to start with a very simple and basic study. If the results are satisfying and correlate with theory results then later on I can move on to more complex study situations. So, I want to perform an external flow analysis with the wind blowing perpendicular to a flat plat (e.g. advertisement panel). For this problem I also have a problem statement from a CFD book which is as follows:

The solution to the problem is theoretically very easy. One has to consider the drag coefficient of the body/shape (here we have a flat plate) and use the formula for the drag force to perform the calculation. The solution is as follows (just for the force acting on the front face of the panel):

You can see that we just have to use the formula and put in the values, e.g. 2 for the drag coefficient of a flat plate, 1.3 for the density of air and so on. Basically, the drag coefficient of a flat plate does not change with the Reynolds number and is approximately 2.0 for most problems as you can see from the following screenshot taken from a CFD book:

The resultant drag force calculated according to the above formula is **18kN! **The next thing to do is to set up a Flow Simulation study and check the results with those from theory. So, I would expect to end up with about 18kN of force on the front face. If you want you can download the complete model (without the study files) and have a look, but here I want to share some screenshots with you. **The problem is that the result from the study shows a normal force (x-direction) of 7.5kN only which is 2.5 times smaller value than the theoretical one! **The following screenshots show the settings of the study:

**So, the initial mesh refinement level is set to 7 with a minimum wall thickness of 25 mm (because the plate is 50 mm thick). The minimum refinement number is 2, the refinement level is set to 3 and the refinement strategy is set to Tabular Refinement. With these setting I want to make sure that the mesh is going to be good enough, but the model is really simple, so it should work. I set a surface goal for the Normal Force in X-Direction. Then I ran the study and got the result of 7.5kN on the front face. The following screenshots show the results:**

Now, the very first question that comes to my mind is: **why do I get a force of 7.5kN with Flow Simulation and 18kN with the theoretical formula? **Am I doing something wrong? Are the settings that I am using suitable for this very simple part? It took really long for the solver to finish, why is it doing so many iterations? Could you quickly perform a study with your own settings and share the results with me? Do I have to change some settings? Or if not, which result should I trust? Later on it would be important because if the force is bigger than I would have to use more material (e.g. thicker plate).

I hope you can help me with this simple problem so that I have the feeling that I am well equiped to start a more complex problem.

Thank you in advance for your hints!

Message was edited by: Teodor Penchev (link to the solution added)

Hi Teodor, I had some time to play around with your model this afternoon. The biggest change I made:

1. switched it to a 2D analysis with a 4mm slice.

2. increased the initial mesh significantly

3. made the compdomain significantly larger, 30m to the back, 10m to the top and bottom and 20 in front.

4. change the goal to be all the faces instead of just the front face

What i'm getting is 17.6N/4mm. About 17.6kN. Note, you need to adjust your equation for the density of air which is 1.2 in your model.

I haven't spent a lot of time on this to look at the goal convergence but wanted to give you some suggestions on next steps.