[Sergi_cfd]

Hi all!

I'm running out of ideas and I would like to share my case with you to see if you can find what I'm doing wrong.

I'm adding a radiator to a race car and I'm adding an additional porous region to represent the radiator. I've created the interfaces, but I'm hitting trouble to correctly set up the physics of the radiator region.

• First of all, the image that I link here is making reference to my global coordinate system and the local coordinate system that I created for the radiator, which is angled.
  Look at Coordinate systems image
  
  
• Then, moving on to the physics settings, for the axis, I assume that I have to specify here my global coordinate system and the flow axis which is at the x-axis.
  Look at Physics settings_1 image
  
  
• For the orientation manager, I’ve selected the local coordinate system that I generated for the radiator and for the Principal Axis 1, which I think that it makes reference to displacement radiator axis of the x-axis relative to the Laboratory Coordinate System.
  Look at Physics settings_2 image
  
  
• Similary, for the Principal Axis 2, I assume that it makes reference to the y-axis, and I put the following values.
  Look at Physics settings_3 image
  
  
• Finally, for the porous inertial and viscous resistance, I’ve set up low values for the ZZ component of the tensor because it’s the direction of the airflow in my radiator coordinate system. And for the XX and YY components, I’ve put big values to prevent flow moving in these directions.
  Look at Physics settings_4 image

So, this is my case and I hope that you can give me any ideas in order to work out that I’m missing or what I’m doing wrong.

Thanks in advance to all of you!

[cwl]

Good man yourself - you've done a great job! Also a good description of the settings

The only question is .. what is your question or the problem you've faced?

[Sergi_cfd]

Originally Posted by cwl

Good man yourself - you've done a great job! Also a good description of the settings

The only question is .. what is your question or the problem you've faced?

Hi @cwl!

So my problem is that I've set up everything as I detailed in my post and when I run the solver, after 30 iterations or so, all the residuals diverge. Then, I look at a vector plane that I generated to see the airflow across the radiator, it doesn't go in the direction of the flow direction, it makes strange things.
EDIT: I added 2 images to show all the mess of airflow that I get in the radiator.

That's why I assume that I might have done something wrong in the 2nd and 3rd steps that I described in my first post and that's why I was seeking for advice.

[dmirel]

Hello Sergi,

Not 100% sure but from what I see you have interfaces between the sides of the radiator and the fluid domain so the air could exit through these areas which are supposed to be walls. In case you have these interfaces, delete them and try to run the case again.

Demirel

[Sergi_cfd]

Originally Posted by dmirel

Hello Sergi,

Not 100% sure but from what I see you have interfaces between the sides of the radiator and the fluid domain so the air could exit through these areas which are supposed to be walls. In case you have these interfaces, delete them and try to run the case again.

Demirel

Hi Demirel,

Thanks for your reply! Yes, you're right, I have 2 in-place interfaces. One for the inlet face of the radiator and another one for the exit face of the radiator.

All the lateral walls of the radiator are considered as normal walls and no interfaces were created in these walls.

So, correct me if I'm wrong, but if I undestood it well, you mean to remove these 2 interfaces that I created?

I was under the impression that these interfaces were necessary because what I did is a subtract region of the wind tunnel area, car and radiator. And then a 2nd region with the radiator which I selected as the porous media region. As a result, what I got is two radiator inlet regions, and two radiator outlet regions and that's why I created the interfaces between these.

I hope that I made myself clear. BTW, later in the day I can upload more images to try to clarify all this.

[dmirel]

Originally Posted by Sergi_cfd

All the lateral walls of the radiator are considered as normal walls and no interfaces were created in these walls.

Hi Serge,

After looking at your first velocity vector plot I thought you have these walls defined as interfaces but maybe is just because of the section plane.
If looking at the vectors in this scene one could understand that there is flow in -Y through the porous region walls.

You are right, you need just two interfaces, inlet-radiator and outlet-radiator.

[Sergi_cfd]

Originally Posted by dmirel

Hi Serge,

If looking at the vectors in this scene one could understand that there is flow in -Y through the porous region walls.

Hi Demirel,

So I think that my mistake could be related to the axis coordinate system that I set up in my case.

If we look back to my initial post at the second bullet point, what I don't really know if I have to select for the Axis the global coordinate system or the local coordinate system that I created for the radiator.

And then, there's obviously something wrong as well in the orientation manager for the local coordinate system of the radiator because as you very well pointed out, there's flow in -Y in the radiator and what I need is flow in -X (global coordinate system) or Z (local coordinate system).

I don't know if this clarify something or makes everything even more complicated.

[dmirel]

Hello Serge,

It might be because of the axis.
You have to use a local coordinate system for the radiator related to the global one.

Demirel

[bluebase]

Hi Sergi,

is it correct that the second principal axis is set to [0,0,0]?
The same question goes for the first one, it's set to [1,1,0].

Assuming you want to specify the inertial resistance ZZ in respect to you local coordinate system, then the set principal axes make no sense to me.
Despite the documentation saying a zero-length principal axis results into a fall-back to the original principal axis, [1,1,0] and [0,1,0] seems wierd.

It seems to me, [1,0,0], and [0,1,0] would be a reasonable choice (in the local coordinate system).

Anyhow, i don't know whether there are other reasons for your problem.

Best, Sebastian

[Sergi_cfd]

Originally Posted by bluebase

Hi Sergi,

It seems to me, [1,0,0], and [0,1,0] would be a reasonable choice (in the local coordinate system).

Anyhow, i don't know whether there are other reasons for your problem.

Best, Sebastian

Hi Sebastian!

I haven't seen your replay till now, but yesterday I arrived to the same conclusion and there you go, it seems that I got it right!

I'm attaching you a vector scene with what I think that now is the right airflow across the radiator!

Thanks to you all, I really appreciate your comments.

This forum is just the best in this field!

[bluebase]

Hi Sergi,

i am glad we could help.

One question though, are you sure the flow through the radiator is now correct? It flows in the (likely) global z direction. Though i would presume the flow should either be parallel to the ground or in the local z direction (from the very first picture in your initial post). However, i do not have any knowledge about race cars, let alone f1 vehicle.

Best,
Sebastian

[Sergi_cfd]

Hi Sebastian,

It seems that it's not over yet my case! The airflow is clearly is flowing in the radiator in the global Z direction, and I have to tweak this to achieve that the flow will go in the local Z direction.

But I have a new doubt. In my local coordinate system orientation, do I have to reference it to the global coordinate system?

To put it simply, when you wrote " It seems to me, [1,0,0], and [0,1,0] would be a reasonable choice (in the local coordinate system)", this orientation that you suggested it's with respect to the global coordinate system?

Cheers,
Sergi

[bluebase]

this orientation that you suggested it's with respect to the global coordinate system?

No, my suggestion was not in respect to the global cs (coordinate system). Instead, as i was indicating with the info in the parenthesis, my proposed vectors were assumed to be in the local coordinates.


So you either enter the local cs vectors x and y in global coordinates into the principal axis 1 and 2, or you switch the cs of the tensor to the local cs.


Best,
Sebastian

[Sergi_cfd]

Hi Sebastian,

Finally, I used the local coordinate system to set the principal axis 1 & 2 orientations as you suggested and that's what I got in the attached file. The airflow seems to be now fine!