First I would like to say I am very new to CFD simulations, but do have experience with FEA. I have worked through a few tutorials and I am left with a few issues in a simulation I am trying to run.
I am simulating a air curtain out of a open face refrigerator (see example picture of what I am trying to do). Some issues I am running into is that the velocity seems to drop off to quickly even with high arbitrary numbers. The air flow doesn't seem to want to flow into the open environment that I created and I am not sure what boundary conditions I am missing. I am having trouble modeling the temperatures as well. If anyone could help me out I would greatly appreciate it.
There are quite a few important points to make here, I apologise for the long list - make a cup of tea
- You cannot apply internal surface Boundary Conditions (BC) - all of these need to be removed (the only internal BC's you can apply are to volumes where you have a heat loss/gain
- You do not actually have any internal air - there is no metal part separating the internal and external so you really just have one air volume with a few shelves floating within it
- To move the air - why not match reality more closely and model internal fans? You could make them cuboid to cover an array if necessary (just be sure to give them a 0 rpm if they are not cylindrical). They would also need a good uniform mesh - 5 elements from inlet to outlet
- Really the only BC's you need are the slip/symm on the sides and a p=0 perhaps somewhere on the external domain - the front?
- Do you need to consider temperatures? You have one set so it looks like it - so this means you need an ambient temp where you have the P=0 - then you could assign a +ve or -ve heat generation internally to a volumetric resistance (which would essentially be the cooling coil) to cool the air, which would be more representative of reality
- The automatic mesh will be insufficient here, but let's start with getting the rest of the setup right and then look at how we can refine it
- Under Physics (Solve -> Physics) you only have flow on and not heat transfer
- Run for 500-1000 iterations, 100 will not be sufficient
- Finally - you could probably run this happily in 2D, this is almost always how I run these models, far simpler and faster to sove
I suggest you make thesee changes and re-post your model and then we can discuss further.
Thanks Jon for taking the time to explain the issues I am having it helps me immensely.
I will probably try to do a 2D model when making the discussed changes. If I run into anymore problems I will let you know.