How to model a fan fixing the mass flow rate?
Hi everyone,
searching here and there, but i still miss something... maybe open a new thread will help me a bit. I would like to model a fan inside a closed loop circuit, fixing the mass flow and not the pressure jump. The reason is explained here. As an idea, I thought to use a flowRateInletVelocity coupled with a fluxCorrectedVelocity:
Are there any idea on how to model such kind of fan? Regards maddalena |
Hi,
Just to say I have solved this: Quote:
Regards maddalena |
Not sure why you are using fluxCorrectedVelocity at the outlet. zeroGradient should work fine. The mass flow specification at the inlet is already enough to guarantee the same at the outlet. However, your approach will not produce very good results, since the flow going out and the flow going in to the domain will not be well correlated as you would expect in the case of a real fan.
To fix it, you have 3 choices: 1. Modify the actuator disk code from windFoam to goal-seek your specified mass-flow rate. 2. Map the outlet velocity to the inlet using the mapping boundary functions like those used in the CHT boundaries. 3. Modify the fan internal boundary to support fixed mass flow (this is the hardest). |
Hi Eugene,
Quote:
Quote:
Quote:
you refers to the coupling condition on temperature, don't you? What I am wandering is: on the temperature coupling there is no external temperature fixed on one of the coupling side, while I should fix the mass flow rate on one of the fan side. How can I do that? As for the pressure, it should be defined automatically once the velocity is fixed. Am I right? Thanks for your suggestions and ideas, regards mad |
Hi maddelena
I got lost using the actuator disk. so i tried something else. here is what i did:
I added a constant source term to the Ueqn say M. i use setFieldsDict to initialize the source terms so that gets activated in the fan region. i run external scripts to automatically check if i have reached my target mass flow rate. (i use swak4Foam by bernard to calculate mass flow rate through internal face zone) if i have not reached my mass flow rate, the script changes the value of M using setFieldsDict and rerun until it reaches steady state and then check again if i have reached target mass flow rate. I know its not an elegant method to do that using external scripts when OpenFoam is such a great tool. but i am not so good at coding and have been losing so much time on this that i tried my method. atleast i am sort of getting wat i want. |
Hi Eugene,
I tried ur following suggestion: Quote:
Code:
volScalarField magUbar = mag(Ubar); but i am not getting what i want. i know i am doing some stupid mistake. but if i understand this properly, mayb i can do it elegantly. pls help!! |
Hi Robin,
Quote:
It would be great if the solver can check mass flow and adjust it in order to keep the prescribed value, during the same simulation. That is, what Eugene suggested yesterday with a solution similar to the CHT boundaries. Eugene, are you willing to help us?:rolleyes: mad |
Hi,
i just came around this post and like to make a suggestion. If I understood you well, you know about the mass flow and your simulation is incompressible. If so, you can use directMapped-BC for velocity at the inlet and map the velocity profile from the outlet to the inlet. You can use the setAverage option to make sure that your target mass flow is reached. Regards, Stefan |
Quote:
|
Quote:
Regards, Stefan |
Hi Stefan and thanks for joining this thread.
Quote:
Quote:
Quote:
mad |
Quote:
|
Quote:
Thus you suggest:
mad |
I'd would do it vice versa:
Quote:
Regards, Stefan |
that looks better. like maddelena asked, what abt k and epsilon?? and for my simulation i also have Temperature field. any suggestions on that??
|
Quote:
Code:
outletFan Quote:
Thanks for your time! mad |
guys one more thing.... isnt there a way to modify the channelFoam to get constant flow rate across the required domain? just a thought. i tried but dint work out. maybe if someone with a better understanding can give a hint?
|
One more question:
This is my 0/U: Code:
outletFan I do not like to fix my fan velocity, since it will affect the velocity field inside my domain as well, while it should be calculated by the solver! |
Quote:
|
Stefan, can you comment on this?
Quote:
Code:
--> FOAM FATAL ERROR: mad |
All times are GMT -4. The time now is 14:56. |