This should be a really simple one. Basically I am trying to analyse the effect on the output CFM of a system by placing different resistances in front of a fan with a fan curve based flow rate. So its a very simple little test chamber I set up.
However I get basically the same results regardless of the open area ratio I apply to the surface. I added a few vent holes in places too in case I was getting some strange results because the system was too well sealed but that didn't help.
The only other thing I can think of is that my fan curve isnt set up very well for this application. My hypothesis in this case was that as the resistance increased, the pressure behind the plate would increase, which would effect the performance of the fan and therefore affect the overall CFM out the end of the test chamber...
But maybe I am missing something, would really appreciate some input!
There are a few points to make here:
- Inlets and outlets should have a nice extension on them - 5x diameter is typical. You will need this on the cylindrical outlets
- Your resistance materials have a 0.2 FAR in one direction but are 100% open in the others. Set an FAR of 0 in the 2 normal directions within the material editor
- All fans/filters must have a good uniform mesh applied to them. We typically start with 4-5 elements through their thickness from inlet to outlet
- You cannot apply an rpm to a fan that is not cylindrical. Either model the fan according to it's real world shape or remove the rpm
- Using Advection Scheme 5 might help here too (Solve -> Solution Controls -> Advection)
Remember that you can press the blue '?' at any point to get help with that particular window. Hope that helps you move forwards.
Thanks for your reply.
I tried a few things, mainly concentrating on the meshing, I updated the resistance materials so that they had zero open area in the directions other than the flow, took off the RPM and played around with using adv 5. But I am still getting very similar results. I even tried using different fan properties.
This suprises me as I would expect the flow to vary with differeng resistances. I would only expect the flow to be so similar if a set CFM internal fan was used, not a fan based on fan curve data (as I have set up in my analysis).
Let me know if you have any further thoughts.
P.S. Here is a link to my share file - with mesh: https://mega.co.nz/#!5QBHibbS!LaPy9D2B6KNQR8UqnkdF
Thanks for sharing this model.
You do still need to make some changes here. Point 3 that I made (All fans/filters must have a good uniform mesh applied to them. We typically start with 4-5 elements through their thickness from inlet to outlet) needs to be applied. Can you give these parts a good uniform mesh - 4-5 elements through their thickness.
Are you sure that the fan working within it's range? Might be have a pressure that is above it's limit?
What was originally a very simple idea for an analysis has turned into a bit of a nightmare! I simply set up a uniform mesh, across the fan and the resistance material, and now I get a divergence issue. I even cloned the analysis and got rid of the fan in favor of a static cfm inlet, but its still divergent.
The simplest things often are, either because there is insufficient detail to raise the mesh count or we are not following the basic rules because it looks simple.
We need to ensure that we have nice amooth flow entering and exiting the model, something we do not have right now. I have it running OK with the end caps suppressed (they were causing poor mesh. Better solution is to extend them, those chambers should be about double the length and you need 5x diamter on the bottom outlet. Should run much better this way!
Ok so I extended the analysis, and now i am suppressing the end caps, and having the bc between the end caps and the air volume.
I set a more concentrated mesh on the resistance, removed the fan and added a bc of a set cfm on the inlet, but still getting divergence!
Here we just need a little more mesh (I refined it all by about 0.6 as you didn't have enough to capture the recirculation) and I also tend to use Advection Scheme 5 when we have fans and filters, anything with multiple pressure affecting devices.
You first model runs OK too, again it just needed more mesh - we also must extend the small outlet if you wish to have a P=0 present. This goes for both models and is probably a good reason that this is diverging. Anything where we have recirculation occurring over a Boudnary Condition can cause issues.
I have this working OK now. Try using a surface rather than a volumetric resistance. I am not sure why this is an issue, it should not be.
We were seeing high velocities around the edges of the resistance where it meets the solid, the boundary layer suggested a geometric issue, although I could not see one.
The odd little velocity blip is becuase we need more mesh refinement, I used a pretty coarse setup here.