[bietchetlien1995]

Hi everyone! Thank you so much for reading this post!
1. I put the velocity at 30m/s - constant (x-drect)
But when I run analysis (I use LES), in the contour of velocity, it showed some area near the bottom of INLET with velocity equal to zero (0).
So, any can help me to explain this and how can to fix this situation?
I will include the image in the comment!

[bietchetlien1995]

[QUOTE=bietchetlien1995;732371]Hi everyone! Thank you so much for reading this post!
1. I put the velocity at 30m/s - constant (x-drect)
But when I run analysis (I use LES), in the contour of velocity, it showed some area near the bottom of INLET with velocity equal to zero (0).
So, any can help me to explain this and how can to fix this situation?
here is the picture https://www.upsieutoc.com/image/xc4BNs

[LuckyTran]

1) You have the no-slip boundary condition on walls.
2) The figure is also rendered image and it's interpolating

[bietchetlien1995]

Hi Lucky! Thank you for answering.
I think the 1st reason is more suitable. But can You explain more for me. How slip or no slip effects to the constant velocity.
And the wall you mentioned, are they wall of building. ?

[LuckyTran]

The building has no slip walls obviously. But no I am talking about the boundary at the bottom upstream and downstram of the building. The 1000m before the building and 3000m or so after the building. There appears to be a wall there with the no-slip boundary condition

[bietchetlien1995]

https://www.upsieutoc.com/image/xLWgRN
Can you check here, I did it.
The bottom of the domain (we can say it's the ground).
I set it (this wall) with no slip condition!

[flotus1]

I won't click on any of these links, but here is my guess: You are displaying cell values.
These cell values are affected by the flow conditions inside the domain. E.g. by the no-slip boundary condition at the bottom. Boundary conditions are not prescribed at cell centers, but at cell faces.
Switching the displayer to node values instead should give you a constant velocity for your inlet face.

[bietchetlien1995]

Thank you so much! , you're right! when I unstick the "node value", the velocity in the inlet came to instant. it's FEM problem I've just remember.
One more question. which one is more accurate? node or surface value (maybe it's used gauss points)

[LuckyTran]

It's not a question of accuracy. You're just plotting things and not realizing what is being plotted and where.

Unchecking node values gives cell values which is opposite of what flotus said would happen. But nonetheless, I'm glad you're happy with your picture now.

[bietchetlien1995]

actually I didn't plot the value out.
But I've realized I did totally oppositely what Flotus1 said.
SO, am I right? when I uncheck it, the thing I received ARE THEY CELL VALUE?

Another question, I understood that velocity will come to the inlet (plane) as a point value at every node (follow the mesh created). Won't they?
Thank you so much LuckyTran!

[LuckyTran]

When you uncheck node values you see the values at either the cell centers of face centers depending on which surfaces you are making the plot based on.

In FVM, you are manipulating values of cells and faces and by convention we place these at the cell centers and face centers. The nodes (the corner thingies)... never come into play directly. That's why if you make a plot and check the node values, it can look wonky because there is an interpolation/extrapolation of the actual cell/face values onto the nodal points.

Originally Posted by bietchetlien1995

Another question, I understood that velocity will come to the inlet (plane) as a point value at every node (follow the mesh created). Won't they?
Thank you so much LuckyTran!

The velocity is applied to the faces not the points. The points don't really matter.... until you try to make a nodal plot.