## Fluids

#### Air throw by fan

• sachin.kumar
Subscriber
Hello I am trying to simulate air throw by a fan inside a closed room. Its a 2 d simulation. I have develop two region in cad one for fan and one for room. I have used fan boundary condition where I have assigned pressure jump polynomial at a fixed rpm.
Can anyone tell me where I can assign this rpm value bcoz in fan boundary there is no such option.
Please guide me related to boundary condition.
• Rob
Ansys Employee

There isn't an rpm setting in Fluent: the polynomials give the pressure jump relationship with flow. What are you trying to model, and with which code? Images would be useful to help describe that.

• raul.raghav
Subscriber

As Rob mentioned, the polynomial you define is the pressure drop as a function of the normal velocity, and the polynomial is derived from the fan curve or PQ curve. You don't need to assign the rotational speed (rpm) since you define the polynomial at the specific rpm.

• sachin.kumar
Subscriber

Hello guys,

I am trying to simulate the fan and coil combination of a commercial cold room refrigeration evaporator. In this analysis, I have assumed the coil as porous medium. please refer the attached image.

In this analysis i do not have the fan geometry. I have only fan curve so my idea is to determine the velocity at the fan outlet by using the fan curve as a boundary condition. please check the procedure and correct me if i am wrong.

boundary condition: as shown in image the complete green color is provided the fan boundary condition. I have defined the pressure jump polynomial wrt. to velocity using fan curve. porous media is assigned as porous and resistance coefficients are defined accordingly.

3) at inlet: pressure outlet boundary condition is assigned.

Now my question is that i have a doubt in fan boundary condition.

is it right to use entire green color/venturi as a boundary condition

is it better to use exhaust fan at the fan outlet rather than assuming the entire venturi as a boundary condition

please suggest me the better procedure how to proceed

• Rob
Ansys Employee

The fan boundary is designed to work on the interior of the domain: setting the cell zone next to the boundary may cause problems: adding some duct to the upstream & downstream is recommended. You then need to decide whether you're using the 2d fan boundary (circular face only) or 3d fan zone (volume highlighted in green).

The "best" approach depends on what you're trying to model and why: given the fan curve, porous coefficients (will give dP v flow) and upstream pressure you could use a spreadsheet?

• sachin.kumar
Subscriber
Ok, I agree with you
You mean I have to place the duct at the inlet and outlet. So can you tell me the fan position
1. will be at the end of the duct?
2. In middle of the duct or it will be as it is?.
And one more thing at the inlet the shape is rectangular so the duct will be rectangular right now I have given a 100 mm rectangular duct as shown in previous image
At outlet the shape is circular it means the duct will be circular.
Please correct me if am wrong.
And what about the length of the ducts?
• sachin.kumar
Subscriber
In continuation with the previous post, one more thing if fan will be at it's actual position then what will be the extended duct outlet boundary condition. Becaouse at inlet already given pressure outlet. Kindly give your valuable suggestions
• Rob
Ansys Employee

Typically you want 5-7 diameters up & downstream of the area of interest to remove boundary effects from the bit you're trying to model.

Whether the duct and/or filters are square or circular is for you to decide: just make a sensible transition between the shapes rather than jumping straight from a circle to square as you may find you can't mesh it.

As an aside, we tend to use fan bc's inside the domain such that they don't block the entire system to aid in stability. In your case you may find the model isn't as stable as normal.

• sachin.kumar
Subscriber
In continuation with the previous post, one more thing if fan will be at it's actual position then what will be the extended duct outlet boundary condition. Becaouse at inlet already given pressure outlet. Kindly give your valuable suggestions
• Rob
Ansys Employee

We wouldn't usually have a fan body crossing the whole domain, they're usually to push air in a part of a domain. The typical use might be a jet fan in a tunnel where only some of the flow goes through the fan.

As I've not used one in quite this way I think the best bet is to set pressure in & pressure out as 0Pa & initialise the flow velocity at what you're expecting to get and see what happens. If that goes wrong we can review the results.

• sachin.kumar
Subscriber

Please see the modified image with upstream and downstream duct. but in this case the velocity vector are coming from both (inlet and outlet) the ends towards fan location instead of going from inlet to outlet because fan is sucking air from inlet. I am unable to understand why?

• Rob
Ansys Employee

Did you create a multibody part & therefore have flow through the whole domain?  Then initialise with a velocity in the desired direction. There are several possible causes: these will help narrow it down.

• sachin.kumar
Subscriber
Yes I have created multibody part and kept the gap (5mm) between fan and duct and also initialize the solution with right direction. But problem is that flow is coming from both the directions towards fan. I think the upstream duct should have large daimeter?

And do you know how to create 2d fan boundary in 3d model because I also want to try exhaust fan boundary condition of fluent?
• Rob
Ansys Employee

Yes, assuming you've got a labelled interior surface (bounding surface on one end of the fan) then you can use one of the interior boundaries (interior, internal, porous-jump, wall and more usefully, fan).

When you say there's a 5mm gap, is there mesh in that gap? Just want to clarify as I'm not sure what you meant.

• sachin.kumar
Subscriber
Yes there is mesh actually I took the fan radius less than the duct radius that's why there is a gap and then subtract the fan from duct with preseving the body of fan and then create the interface between fan and duct.
• Rob
Ansys Employee

Please can you post an image of the mesh, slice through centreline (ish) and show full elements (use the pale blue triangle option on cut plane). I think we're in danger of confusing each other.

• sachin.kumar
Subscriber

this time i have increased the upstream duct size. pl. see the image for fan position and mesh

In velocity vector image we can see the vectors are going top or bottom side and very few vectors are going towards outlet and if we see at the outlet the vectors are coming towards fan. kindly help me out I am in trouble.

• sachin.kumar
Subscriber

I have tried 2d of this model. here are the images of 2d fan and coil combination

In two dimensional the results seems to be same and I have observed one thing common in both 2d and 3d which porous media. I think porous media is creating a problem. what do you think about it. Let me do one thing I will simulate it by uncheck the porous media then get back to you

• sachin.kumar
Subscriber

Now it is confirmed, it is due to the porous media. here are the images without porous media

Now, can you give tips regarding porous media. I have determined inertial and viscous resistance coefficients and put them into fluent. please the attached images and tell me whether i am right or wrong

• Rob
Ansys Employee

The viscous coefficients look to be the defaults which are for "porous" rock: ie they pretty much block flow. Check how you derrived the coefficients, and (probably) set viscous resistance to zero.