## Fluids

Topics relate to Fluent, CFX, Turbogrid and more

#### Direction vector is worng

• Agung Limowa
Subscriber

Heloo i really curious i have model but the direction vector of the outlet is wrong how i overcome this (The vector is moving back to the pipe instead of going out). I Imported my model to 3d in AutoCAD as slice material for the pipe the inlet is completely inside the tunnel (the case is the pipe has to suction the air from the tunnel and blowing out again) what should i do, the boundary condition is kinda confusing )

• Essence
Ansys Employee

Hello,

Remember that positive values for x, y, and z velocities indicate flow in the positive x, y, and z directions. If flow enters the domain in the negative x direction, for example, you will need to specify a negative value for the x velocity. The same holds true for the radial, tangential, and axial velocities. Positive radial velocities point radially out from the axis, positive axial velocities are in the direction of the axis vector, and positive tangential velocities are based on the right-hand rule using the positive axis.

• Rob
Ansys Employee

What boundary type did you pick? If it’s a velocity inlet (for an outlet) the image vector will still point into the domain. It’s to indicate the boundary rather than show the flow direction (inlets to tend to flow into the domain though). I'd check the mesh, with only one indicator arrow that could point to a very low cell resolution.

• Agung Limowa
Subscriber

Hello, thank you for your kind answer, I had moved to the older version where i can set my flow direction. And also the boundary type is outlet (for an outlet) but the vector stoll point into the domain ? is it will affect the calculation ?

• Rob
Ansys Employee

An outlet will point out of the domain, please post a screen shot of the boundary condition panel.

• Agung Limowa
Subscriber

Hi Here is my boundary condition every branch's name Otulet start from 4A, 4B (first image ) and so on, The second image is outlet 1,2,3

• Rob
Ansys Employee

You need to very carefully look at your boundary conditions. You cannot have an outlet (or inlet or any other external boundary type) inside the domain. The errors will prevent the model from running.

When you built the mesh you labelled some surfaces as "outlet" and that carries the type over to Fluent.

• Agung Limowa
Subscriber

oh i see now, that's why my fluent always floating point Exceeded and divergence, i will find a solution  to modify the boundary thankyou

• Rob
Ansys Employee

Assuming it's supposed to be interior either fix in Meshing (set the boundary type) or change into a wall (Fluent will create a wall & wall:shadow pair), then turn that wall into an interior.

• Agung Limowa
Subscriber

Thank you for the advice, i want to ask another question about using mass flow outlet as a condition, I try several times the mass flow outlet gives divergence and when i switch to pressure it can run okay so, how i overcome this?

• Rob
Ansys Employee

It depends on why it's diverging. What boundary type is at the other end?

• Agung Limowa
Subscriber

i have set it to mass flow outlet and interior tha common things make it is diverging because of the viscosity turbulent limited to xxxx

• Rob
Ansys Employee

Flow has to enter the system from somewhere, what is that bc type? Is it realistic to suck that much mass out from that boundary?

• Agung Limowa
Subscriber

Here is my condition of my vector, si the design is the air is flowing from the portal tunnel and it has to suction the air from blur vector to duct (as Inlet) and transfer it as air on outlet mentioned above. What boundary condition i should set

• Rob
Ansys Employee

Do you also want air flowing in the ducts? If so, you can't use a velocity or pressure boundary.

• Agung Limowa
Subscriber

Yes, I want it to flow in the ducts, but my question is

1. As mentioned above the inlet, outlet, etc cannot be placed inside the domain. if so, is it okay to place an inlet velocity inlet?
2. if I put velocity inlet, will the inlet suct existing air without creating new flow?
3. For a complete scenario should i make a new thread or continue here? because i really confused by boundary condition and how to set BC, ansys show error many times.
• Rob
Ansys Employee

OK, boundaries are covered in the tutorials (click on Help in Fluent) and on the Learning section here (CFD/Fluids courses). That should cover the basics.

In your case I assume your ducts have fans in them? Ie air is drawn into the duct and blown out of the other end. Do you need to model inside the duct? Or can you just set an inflow & outflow for the duct and ignore the middle bit? You images look a bit like tunnels, but at 0.5m across it's a lot smaller than I've modelled with ducts/jet fans present.

• Agung Limowa
Subscriber

yes it is a duct and tunnel case, and the duct have fans in it, so maybe to be clear here is my scenario

So, The air is flowing from the tunnel inlet (black arrow) all the way to the back of the arrow, and from the middle the air is suction to that back and have outlet there (tosca arrow) and all the air is inside the tunnel is suction from red arrow and finally ended at the portal (blue arrow)

Do you have an idea for the boundary condition i've set the tosca arrow as an outler, a green arrow as an inlet and the red arrow as interior and finnaly blue arrow as an outlet. Is this correct, bacuse i always have an error on my simulation either floating point, turbulence viscosity limited, Divergence in AMG Solver and so on.

• Rob
Ansys Employee

OK. For the external boundaries (tunnel ends) you need pressure or velocity, the choice will depend on what you know.

For the ducts it's a little more complicated. Do you need to model flow in the duct, or do you just need to understand the effect of the duct flow on the larger tunnel? Have a look at fan boundary conditions and FIX cell zone conditions, or neglect the inside of the ducts and use velocity boundaries with +/- components to suit.

• Agung Limowa
Subscriber

i need to model inside the duct can i have reference about to set the condition? ?

• Rob
Ansys Employee

https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v231/en/flu_ug/flu_ug_chp_bcs.html

• Agung Limowa
Subscriber

Hi, I'm sorry i can't open that, I'm using my school lab and there is no one in charge for the licencing option

• Rob
Ansys Employee

Click on Help in Fluent, then paste the link into the browser that opens. The solvers contain a token/cookie/biscuit that bypasses the log in requirements.

• Agung Limowa
Subscriber

• Agung Limowa
Subscriber

Hi, it's me again i have the question about the Inlet and outlet inside the domain, the problem is i want to set the parameter there what should i do the if in this case of problem ?

• Rob
Ansys Employee

You want to set the flow speed in the duct?

The inlet/outlet boundaries CANNOT have cells on both sides. So, the duct either needs a fan boundary, FIX/source cell zone conditions or to be a void. For the latter the ends are then, by definition, on the outside as there is a hole where the duct ought to be.

What purpose is served by modelling the flow inside the duct?

• Agung Limowa
Subscriber

I need to see how much the air quantity and to see if the quantity is sufficient on the outlet, if i set on boundary as interior cant control the flow there. So i need to set as a fan ?, If i set as a void i'm not sure the air will flow through the duct, and cdo you have reference about fix/source cell zone? im really sorry for too much asking, i'm really new and this boundary problem seems never ends

• Rob
Ansys Employee

No worries.

What quantity are you trying to find?

If the duct is a void in the model you're correct there is no flow, but, you remove some amount at one end and add the same amount at the other: you're controlling the flow without needing to worry about what happens in the middle.

• Agung Limowa
Subscriber

the airflow quantity, so what i want to sinulate is when i set certain amount of air in inlet will resulting how much air air at the outlet based on the air behaviour itself. so if like you said to set as an void andi'm controlling the air at the end ,  makes me can't see the air flow and how much the air flowing, so i'm guessing if i set as as a void it means i set the outlet and the inlet alone right, or can you elaborate more? the problem is i want to know how to know the outlet mass flow or velocity, thats why the air flowing through the duct i think is important because the duct has multiple outlet