[navid1996]

Hi. I am simulating a two-dimensional cross-flow fan in fluent. The fan is inside the case. The boundary condition of the input and output are both output pressures. The rotational speed of the fan is known. But the current is not established from input to output. Where is the problem? Thank you for your help

[EmmTheof84]

Originally Posted by navid1996

The boundary condition of the input and output are both output pressures.

When you say output pressures, you mean pressure-outlet or a set pressure? You can't have 2 pressure outlets, one of them must be inlet.

[navid1996]

Originally Posted by EmmTheof84

When you say output pressures, you mean pressure-outlet or a set pressure? You can't have 2 pressure outlets, one of them must be inlet.

Thanks for the answer, dear EmmTheof84. I analyzed both of these cases. Even with the boundary condition of inlet and outlet pressure, the flow was not established.

[EmmTheof84]

I assume you have set your rotating regions correctly (correct axis, correct rotation)?
Also, the Wall boundary condition that is your impeller needs to be set to "moving Wall", Rotation, Relative to adjacent cells (Which are the cells in your rotating region) and have a rotation of 0

[navid1996]

Originally Posted by EmmTheof84

I assume you have set your rotating regions correctly (correct axis, correct rotation)?
Also, the Wall boundary condition that is your impeller needs to be set to "moving Wall", Rotation, Relative to adjacent cells (Which are the cells in your rotating region) and have a rotation of 0

Everything you said has been entered correctly, but the flow is still not established. The flow entered is 0.004 kg / s, which is not logical and should be much higher.

[EmmTheof84]

Assuming you are running a transient simulation, have you defined your timesteps correctly?

If you are running steady state, try running first at 10% of your RPM, then double that and continue your solution. Repeat until you reach the 100% of your RPM

[navid1996]

Originally Posted by EmmTheof84

Assuming you are running a transient simulation, have you defined your timesteps correctly?

If you are running steady state, try running first at 10% of your RPM, then double that and continue your solution. Repeat until you reach the 100% of your RPM

I use transient simulation and set the timesteps according to the reference article.

[EmmTheof84]

Try running steady state until it converges and then use the converged steady state solution as a starting point for your transient analysis.
Also, what turbulence model do you use and have you made sure your y+ is suitable for your turbulence model?
Is your mesh resolution adequate?

If those fail, I am out of ideas

[navid1996]

Originally Posted by EmmTheof84

Try running steady state until it converges and then use the converged steady state solution as a starting point for your transient analysis.
Also, what turbulence model do you use and have you made sure your y+ is suitable for your turbulence model?
Is your mesh resolution adequate?

If those fail, I am out of ideas

Thank you again. I will do what you said and I hope the problem is solved. I use the K-Epsilon standard turbulence model. The mesh resolution was also checked. Unfortunately, my tutor could not solve the problem. Can you explain more about y+?

[EmmTheof84]

If you are using k-epsilon the your y+ should be between 30 and 300.
A more thorough explanation of y+ is found here:
https://www.youtube.com/watch?v=fJDY...idMechanics101
https://www.youtube.com/watch?v=nSdV...idMechanics101

You can plot your y+ value by going to results->graphics->contours. You will need to select all your walls, use turbulence as a value from the drop down menus and yplus from the drop down menu right below turbulence.
If your y+ is above 300 you will need to refine your mesh on the wall (inflation layers).
What version of k-epsilon are you using? If you search for a book called "Developments in turbomachinery flow. Forward curved centrifugal fans" by Montazerin, Akbari and Mahmoodi they recommend the k-e RNG model as it gives closer results to experimental. standard k-e and k-w tend to underpredict the flowrate and pressure.

[duri]

Is it possible to do cross flow fan simulations in 2D. I am assuming that the fan you mentioned is an axial fan. It is highly 3D problem. Are you modelling fan as geometry or source term? Could you share your flow domain.

[navid1996]

Originally Posted by EmmTheof84

If you are using k-epsilon the your y+ should be between 30 and 300.
A more thorough explanation of y+ is found here:
https://www.youtube.com/watch?v=fJDY...idMechanics101
https://www.youtube.com/watch?v=nSdV...idMechanics101

You can plot your y+ value by going to results->graphics->contours. You will need to select all your walls, use turbulence as a value from the drop down menus and yplus from the drop down menu right below turbulence.
If your y+ is above 300 you will need to refine your mesh on the wall (inflation layers).
What version of k-epsilon are you using? If you search for a book called "Developments in turbomachinery flow. Forward curved centrifugal fans" by Montazerin, Akbari and Mahmoodi they recommend the k-e RNG model as it gives closer results to experimental. standard k-e and k-w tend to underpredict the flowrate and pressure.

What does it mean if Y + is less than 30 and what is the problem?

[navid1996]

Originally Posted by duri

Is it possible to do cross flow fan simulations in 2D. I am assuming that the fan you mentioned is an axial fan. It is highly 3D problem. Are you modelling fan as geometry or source term? Could you share your flow domain.

Yes. Imagine cutting a 3D fan with 35 blades inside a case perpendicular to the axis of the cross flow fan.

[navid1996]

Originally Posted by duri

Is it possible to do cross flow fan simulations in 2D. I am assuming that the fan you mentioned is an axial fan. It is highly 3D problem. Are you modelling fan as geometry or source term? Could you share your flow domain.

https://forums.autodesk.com/t5/cfd-f...n/td-p/7783215
Similar to the link above

[duri]

The fan doesn't appear effective. Not sure how the flow enters the blade against centrifugal force from top. What is the actual problem what is the full 3D geometry.

[navid1996]

Originally Posted by duri

The fan doesn't appear effective. Not sure how the flow enters the blade against centrifugal force from top. What is the actual problem what is the full 3D geometry.

The real problem is that when the inlet and outlet pressure is the boundary condition at the inlet and outlet, the flow of 0.004 kg / s enters the inlet, which is not logical.But when the flow at the input is specified as a boundary condition, the flow is established correctly.
The full 3D geometry involves a cross-flow fan with 14 blocks inside a case. But by zeroing the thickness, I analyze the problem in two dimensions.

[duri]

It is not problem at all the, flow is driven by difference in total pressure at inlet + increase in total pressure and static pressure at exit. Here the total pressure at inlet and static pressure at exit are almost same. So total pressure increase in fan. Your right parameter is fan pressure ratio and flow rate. When you fix flow rate at inlet then boundary is driving the flow and not the fan.

[navid1996]

Originally Posted by duri

It is not problem at all the, flow is driven by difference in total pressure at inlet + increase in total pressure and static pressure at exit. Here the total pressure at inlet and static pressure at exit are almost same. So total pressure increase in fan. Your right parameter is fan pressure ratio and flow rate. When you fix flow rate at inlet then boundary is driving the flow and not the fan.

That's right. Thank you for your help.