[Bigfoot]

Hello,

I am an intermediate CFD user and a FloTHERM novice.

I have an enclosure with a board and several heat sources on it. These heat sources are cooled by 7 fans driving airflow out of the enclosure.

I have run this project with a few different meshes and I notice that the temperatures of the heat sources are fairly mesh independent (~3% variation) while the total flow rate through the box is highly mesh dependent (~100% variation).

Since the variation in flow rate does not cause a significant change in temperature of the heat sources, it leads me to believe that my model is capturing the physics near the heat sources on the board, but is not capturing the flow near the exit, i.e. near the fans correctly. I am also noticing something very curious - the operating points reported by FloTHERM for each fan are not on the fan curve! The static pressures being reported for the fans seem approximately right - but it makes no sense to me that FloTHERM is reporting incorrect flow rates for those fans given the static pressure it is computing. FYI - I am using an axial 3D 12 facet fan model to model the fans - not sure if that is the best choice for my situation.

I am wondering if any experts here can help me understand why this could be happening, and how to obtain confidence with the flow rate result.

Thanks,
Nikhil

[Gabriel_C]

Hello,

Hmmm... I always have problems with fans in simulations (and don't have so much experience with them) but the operating point was always on the PQ curve for me.
All the 7 fans are taking air out.... do you have some holes to let fresh air inside the enclosure?
Can you post a picture of the model with some construction details?

[Bigfoot]

Hi Gabriel,

Thanks for the reply. I don't think I am at liberty to post pictures of the model.

The enclosure does have sufficient venting in the front for the fans to draw air from.

I think the problem comes down to the fan solution not having converged sufficiently. What's weird is that out of the many simulations I ran for this model, the model with the coarsest mesh is the only model where the fan flow converged (and operating point is on the curve). For all the other models, I believe the temperature has converged sufficiently - evidenced by the residuals dropping below 10 and monitor points becoming steady, but the fan flow has not (after 500 iterations).

I dug deeper into this and found a note from FloTHERM that recommends setting 'fan relaxation' to 0.3 for faster fan flow convergence. I had it set 1 (default). I am currently trying this and will report if it helps.

Thanks,
Nikhil

Originally Posted by Gabriel_C

Hello,

Hmmm... I always have problems with fans in simulations (and don't have so much experience with them) but the operating point was always on the PQ curve for me.
All the 7 fans are taking air out.... do you have some holes to let fresh air inside the enclosure?
Can you post a picture of the model with some construction details?

[Gabriel_C]

Hello,

I understand, we all do simulations under strict disclosure agreements.
Let me give you a 1000 points hint for convergence problems:
- see who produces the highest residuals (temp, pressure, velocity...etc)
- under "Solver Control" tab check the "Error Field" and choose the corresponding "bad boy"
-run the sim for a few iterations (until high level stability is achieved)
- visualize in visual editor a plane with scalar "Error Field" and see where is the area that causes bad convergence

Maybe you knew this tip

Best regards, Gabriel

[Gabriel_C]

...one more thing.

if you have space and money for 7 fans maybe a couple of them (2-3) could be set to input fresh air from ambient and the rest to take the air out of the enclosure.

Just as a feeling (from past fan's simulations);
- fans extracting air from enclosure takes the air from "un-controlled" areas (maybe cold air also)
- fans inputing air in enclosure can be placed to guide the air flow directly into a heatsink fins

BR, Gabriel

[Pawel Zdunek]

Hello Sir,
maybe try to check in message window if you receive any communications about fans, overlapping elements etc, but I guess if this was a reason you wouldn't get best results in the coarsest mesh. There is also this thing about fan curves (I've read about it in user manual I guess) that user should avoid flow rate which coincide with pressure plateau (you know- don't operate the fan in range where P is constant) and the curve itself should be defined with "sufficient" datapoints.

[CFDfan]

Originally Posted by Pawel Zdunek

Hello Sir,
maybe try to check in message window if you receive any communications about fans, overlapping elements etc, but I guess if this was a reason you wouldn't get best results in the coarsest mesh. There is also this thing about fan curves (I've read about it in user manual I guess) that user should avoid flow rate which coincide with pressure plateau (you know- don't operate the fan in range where P is constant) and the curve itself should be defined with "sufficient" datapoints.

This is a bizarre thing to write in the manual. Mentor's people should know that in reality this plateau is usually the place where the fan operates at.

[Pawel Zdunek]

Originally Posted by CFDfan

This is a bizarre thing to write in the manual. Mentor's people should know that in reality this plateau is usually the place where the fan operates at.

I will check where I found it

[bighead]

pressure plateau is generally avoided as the "fan" will be "hunting" for the system operating point. This increases the computational time. A good check will be to see if you can generate system resistance curve for your model and mesh it well. This will help you to determine and check the corresponding operating point from FLOTHERM.

[Boris_M]

Hello,

the reason for this suggestion in the help of FloTHERM is that the plateau should generally be avoided with fans, rather work slightly the right of it as this link also shows:

http://www.esmagazine.com/ext/resour...ges/116338.gif

The plateau in the ideal case is not a plateau but a slight slope, not fully horizontal. However the fan development is not ideal :-)
You can also find fans with curves like in the link above and the issue here is the stall region. At the same pressure the fan basically can jump between the two or three points of flow rates and it becomes unstable and hard to converge for the solver. It is easier if the solution approaches from one side to that point but with a plateau there is suddenly only the horizontal section and which flow rate should the solver then apply.

In reality you cannot control that either and only the tiny imperfections of the airflow in reality will cause to jump between these points. Nature is more chaotic than the idealized world of CFD.
you have to consider that in CFD you try to estimate what nature does/what happens in reality but in reality it simply happens. If there is a fluctuation in pressure then there is one. That fluctuation can come from a butterfly flapping with his wings in the US or a bag of rice falling over in China. If you get what I want to say :-)

Hope this helps,
Boris