Hi everybody, I made a geometry which is not very complex,however meshing the geometry with structured grid does not seem to be very easy since the geometry has very small gaps and also its aspect ratio is high.so I meshed it using tgird,I solved the turbulent flow and heat transfer for it and it seems the results are fine!(I'm not sure).my questions are: 1.How can I make sure the grids are fine for my model? 2.Does taking the time to mesh it with structured grid seem reasonable? 3.if I use half structured(where flow is important) and half unstructured grid,is it gonna make the results better? 4.Can decomposing the volume be a method to mesh the geometry with structured grid? thanks

Hi John. Everytime you run any problem with CFD you MUST make sure the result is grid-independent. That is, you must run the problem twice with two different grids. If the results change significantly when you change the grid, then you know you have a problem. If the results are nearly identical then your results are correct (assuming your model correctly described reality).

John,

First and foremost your grid must resolve the geometry accurately. I assume you've done this.

Second look at your problem from a macro persepective and predict whether you will have areas of separated or recirculating flow. In these areas you may want to intensify your grid or even grow a hybrid boundary layer mesh using prisms. Of course this is all before you iterate. In a converged solution, try adapting the solution based on things like static pressure gradient.

Third, check your y+ levels - again through the adaption option. With the k-e turbulence model you're using the y+ maximum should be 150 or less. If it's not you need to adapt your grid.

Last, I have moved structured meshes into the obsolete technology column. Unstructured tri/tet meshes can be applied to any geometry and provide perfectly fine answers for real problems. Structured meshes are mostly for academia. If I had to Cooperize all my CFD models I would never get any work done.

John

Hi Scott, Thanks for your responds it was very helpful. Scott, I ran my simulation for two different grids and it seems the results are in good shape.but I have one question,when I compare the results do I have to compare all the variables like velocity, temperature, pressure, turbulant intenrsity.....or just velocity and temperature are fine? Thanks again John

Hi Scott, Thanks for your responds it was very helpful. Scott, I ran my simulation for two different grids and it seems the results are in good shape.but I have one question,when I compare the results do I have to compare all the variables like velocity, temperature, pressure, turbulant intenrsity.....or just velocity and temperature are fine? Thanks again John

HI John,Thanks for the good points you made.It was very helpful

Not so soon. Do not discard your old structured mesh technology yet. Try solving the following problem in stationary frame of reference in both fluent 4 and fluent 5 (structured and unstructured solvers respecively):

Geometric description: 3D annulus with inner radius of 4", outer radius 9.875", height 6"

Boundary conditions: Both inner and outer walls spin in the same direction at 100 rad/sec. Use quarter periodicity for the theta direction if this is not a pain to create.

In the axial direction, let one end cap be a wall and the other a symmetry type boundary.

The solution expected is a linear variation in velocity in the radial direction.

This problem may reveal some differences in the structured and the unstructured solvers of fluent that are worthy of further discussion.

That depends on your goal. Ex: if you want the temperature profile then differences in pressure, velocity, etc. may be unimportant to you. If you need every piece of data, then you must keep making your mesh smaller (larger numbers of cells) until everything is unchanged.