Sliding mesh with conjugate heat transfer

  • Topic Is Locked
  • 123 Views
  • Last Post 28 October 2019
  • Topic Is Solved
Ramy posted this 20 October 2019

Dear all, 

I am simulating a 2D first stage turbine as seen in Fig. 1. It is consisted of 4 domains; at the left, there is a fluid domain and a solid domain (stator vane) and at the right, there is also a fluid domain and a solid domain (rotor blade). The two domains at the right are moving down by using a sliding mesh technique. After initialization, once I start the iteration, I get a warning saying:

WARNING: The solid velocity has a significant normal component on 10708 faces of face zone 21.

The maximum angle between the velocity and face surface is 90.0 deg at ( 2.364e-02, 3.669e-02, 0.000e+00).

The solver may not achieve global energy conservation as a result.

The tolerance for this check (currently 20.0 deg) is controlled by the rpvar 'wall/vnormal-tolerance'.

Please check your setup. This warning will not be written again.

 

and then after couple of iteration, I get divergence because the temperature of moving solid gets unrealistically low (1 Kelvin). 

 

The boundary conditions are simple:

1- inlet (the left vertical edge at the left of the stationary domains): pressure inlet: 16 atm (Also, I tried mass flow inlet=15 kg/s and velocity inlet = 10 m/s as well).

2- outlet (the right vertical edge at the right of the moving domains): pressure outlet: 3.5 atm.

3- The upper and lower edges of the fluid domains are periodic boundary condition.

4- the interface (its length is 0.05 m) between the moving and stationary domains is "periodic repeat".

5- the two solids domain: constant heat flux (I also tried different values for it)

6- the moving domains moves down at a speed of 553 m/s.

7- time step size = 3.5 e-6 seconds.

8- I tried different schemes (coupled, simple, simplec, etc) but I got the same warning and divergence!!

 

I also tried a denser mesh for the moving solid body but didn't solve the issue.

 

Thank you. 

 

 

 

 

 

Order By: Standard | Newest | Votes
Ramy posted this 20 October 2019

more details: the two domains at the left have a conformal mesh and the two at the right have a conformal mesh as well. But between the two fluids domains they have a non conformal mesh and that is why the interface was created to enable the sliding mesh technique. 

abenhadj posted this 21 October 2019

So the wall rotor part is rotating at sane angular speed, right? Because the error warning message tells that there is a sort of normal motion which a MFR approach does not like. As you are running unsteady I recommend using interface for the rotating part at solid fluid contact sides.

Check the manual for the cases failing when solid motion and energy loads. The main restriction the body needs to be a surface of revolution.

Best regards, Amine

Ramy posted this 22 October 2019

Hi Amine, 

I tried the non-conformal mesh and created interface between the solid and fluid domains but unfortunately the same warning and divergence happened again! 

Do you have suggestions?

abenhadj posted this 22 October 2019

And both are rotating with same speed?

Best regards, Amine

Ramy posted this 22 October 2019

Yes. In the "cell zone conditions", I assigned a "moving mesh" to the fluid rotor domain  with a speed of -553 m/s (because it is moving in the -ve y direction) and for the solid rotor domain, I assigned a relative velocity of 0 (relative to the fluid rotor velocity). 

I also tried assigning an absolute velocity for the solid domain instead of a relative one but it gave the same error.

For the boundary conditions, I assigned a moving wall boundary condition to all the solid walls in the moving domain. 

abenhadj posted this 22 October 2019

Does the solid has a solid zone dedicated to him or not? It should be and you need to assign here in cell zone the same angular speed.

Why do you want to model the solid part? I would start with only walls.

Best regards, Amine

Ramy posted this 22 October 2019

Yes, The solid part has its own zone. I have four cell zones (two fluids and two solids). Actually, I want to model the solid part because my goal is to extrude this 2D case to a 3D case and I will add fluid domains inside the blades so the solid domain will have a fluid domain on his both sides (double sided wall with  conjugate heat transfer). 

abenhadj posted this 22 October 2019

If the whole rotor is rotating solid zones needs to be rotating too.

Best regards, Amine

Ramy posted this 22 October 2019

For this 2D case, they are sliding with the same speed (the solid and fluid). 

abenhadj posted this 22 October 2019

In 2d the rotational axis has to be the z axis.

Best regards, Amine

abenhadj posted this 22 October 2019

If axis symmetric then it is the x axis.

Best regards, Amine

Ramy posted this 22 October 2019

I am a little bit confused with the term "rotational axis" for a 2D case. So, I am attaching a picture showing three different axes. The black arrow represents the sliding direction. I am using number 2. 

Ramy posted this 22 October 2019

I figured out that this problem only arises when a solid domain is used (conjugate heat transfer). I did a case without solids and it worked well. So, I guess the axes are not the problem. 

 

rwoolhou posted this 22 October 2019

Have you checked the User's Guide in Heat Transfer to make sure you're not breaking one of the limitations? 

abenhadj posted this 22 October 2019

Again in planar 2D the rotation axis is the z axis.

Fluent does not like motion normal mesh as it thinks it should be some deforming mesh setting.

Unfortunately we are limited here by providing further suggestions without looking into the case.

Best regards, Amine

Ramy posted this 26 October 2019

Yes, It was the problem of the coordinates for the solid domain. Thank you.

Ramy posted this 26 October 2019

Thank you.

abenhadj posted this 28 October 2019

Thanks for the feedback.

Best regards, Amine

Topic Is Locked

Close