object moving upwards and flow from the left to right

Hej Guys,

I got a problem I cant solve in one step. I have let say one cube moving upwards with 40m/s and have a flow from the left to the right 10 m/s

I set up the simulation by having a thin brick and boolean differented out a box. So its a brick having a hole in it. Assign air to the whole volume. The brick wall left is an inlet the right wall is an outlet. The rest of the wall of the brick is not wall. The hole walls are walls. I set up these walls to have linear velocity upwards. I assign pressure to all faces. If I simulate I get obviously invalid result.
I need to see both movement's result, that the object is moving in a flowing "wind".

I wonder how to set up this simulation...

Thanks.

Bela

No votes yet

Reference frame for stationary object

Linear Velocity you assign to a wall has to be in the plane of the wall (e.g., "Flow Over a Rotating Wheel with Moving Ground"), so your current approach will not work.

You need to consider a reference frame where your object (cube) is stationary similar to "CFD Analysis of a Sail Yacht from SketchUp". In your case you need to:

  • Set your reference velocity to (40 10 0) or the equivalent for your axes
  • Assign all your outer boundaries to be Inlet-Outlets
  • Assign all your cube faces to be Walls, without Linear Velociity
  • Ensure your outer boundaries are well away (at least 6 object lengths in all directions) from the cube as in all the tutorials

still invalid

Something is wrong because its still giving me invalid result.

If I do it that way that I use only inlet and outlet on the opposite faces, then it is good but only one direction. Its like I need to run two simaltion and somehow combine the result because it wont work together. maybe its a bug?

The image represents the results from the method you describe.
http://s7.postimage.org/kx0s1acvf/simulation.jpg

Use Inlet-Outlets

I suggested in my previous comment that you make all your outer boundaries Inlet-Outlets and use a reference velocity of [40 10 0], did you try it?

Just to be clear Inlet-Outlet is a specific boundary condition type distinct from both an Inlet and an Outlet.

If you set a velocity parallel to an Inlet I wouldn't expect it to work - no flow will enter the domain - it's not a bug.

Looking at your geometry you also need to expand the thickness of your flow volume - unless you have a special 2D hexahdra topology as in the tutorial "Water Tank". You will also likely need Symmetry Local on your front and back faces.

of course I did... After

of course I did...
After restaring it several times it worked, but the results are still not valid, not that worse as above example though.

I think I need to give an example, like a wind generator blade. Lift based win blades takes the air from the front and despite the high pressure/drag because of the turn speed still have enough lift (pressure difference). This doesnt show up in the results. It shows otherwise actually. Very badly.
I dont think this method makes me closer to the result, simulating two different direction wind instead of object moving in a wind perpendicular to the flow direction wont solve it. Naturally it would be wrong, and how the hell you would solve it? One would have influence on the other. which is obviously seen on the result... THe arrow tells what happens to the wind... Its not usable this way.

Do you understand it?

Corrected Superposition Velocity

For the corrected superposition velocity try using the velocity calculation under the "Physics" section at "CFD Analysis of a Sail Yacht from SketchUp".

If this isn't what you are trying to achieve then, no I don't understand your requirements.

The velocity I used only to

The velocity I used only to see what happens with the wind... The angled arrows shoved that the flow is calculated in a way which is not good for me.
I needed pressure calculations. For the lift and cp ext caedium is good, but the to see the complex problem from different angles I am afraid it cant to for now.

so its like a flow along X 10 m/s and the object moves perpendicular to this flow 40 m/s.

I was wondering why did you stick to this system that the substance and objects 'have to be one'. It would give much greater possibilities if the substance and the objects could be separated which allow such simulation like a wind blades rotating, and calculating everything. Could make life significantly less headache. Maybe next major version?

Thanks for the support anyway.

Moving Reference Frame for rotating machinery

For a Caedium RANS Flow (and other field-based CFD) simulation you need a volume to construct a volume mesh, that is why the objects have to be subtracted from the flow volume.

You can still simulate rotating machinery using the Moving Reference Frame (multiple flow volumes) capability as shown in the tutorial "Rotating Paddle using Moving Reference Frame". For another example see "Caedium v4 Sneak Peek: Rotating Vertical Axis Wind Turbine CFD Simulation".

To move objects around within a flow volume in an arbitrary manner requires a moving mesh capability. It is a complex and often unreliable method. Moving mesh is not supported by Caedium.

Maybe I'm still misunderstanding your requirements, but you can create arbitrary new Results, based on existing Results. For example if you want to transform the velocity field to be relative to the global reference frame (object moving), then you would create a new result Ug = U - Ur, where Ur is a constant vector. For more on new result creation see the tutorial "Fluid Flow Around a Sphere: Theory Comparison".

Moving mesh> I agree that it

Moving mesh> I agree that it is unreliable, but very much needed in the industry. Somehow openfoam has to evolve as well ( maybe consider everything as a particle...even if it is slow it would work.). I take a look at the other option you presented after Christmas. Merry Christams to Symscape.

Trending Now