I would like to know how in fluent axisymmetric flows are calculated does the compuatatinal domain is 2d or it is wedge (a sector of the cylsinder). Also for a 2d reactangular case does fluent solves the equation in 3d or not if yes I think they use one grid in z direction.How do they calcuate size of thes grid . Please help Z

In axisymmetric flow it's based on a 2d computational domain (assuming you selected the 2D axisymmetric solver) where the axis of rotation is coincident with the x-axis. Then, fluent solves the flow in cylindrical coordinates (r=y, theta=all angles, z=x). Instead, you can use the 3D solver, and set periodic boundary conditions on a wedge. One example of this would be a missile with 4 wings... create a 90degree wedge, and then use the periodic boundary condition (just one example).

For a 2d rectangular case, fluent solves it in a 2D domain, but uses the depth you define in the reference values to give it the third dimension for calculating forces, mass flows, etc.

Hope this helps, and goodluck, Jason

Thanks for your answer. I have been doing a calculation of flow behind bluff body in a 2d case. Actually I noticed a strange thing in fluent is that the size of the cell in z direction is almost equal to the width of domain. It seems that they have long cells in z direction. Actually as far as I know that we can not set the size of the cells in third direction.

What is the physical basis behind using uch an option in fluent.

When you say z-direction, I'm assuming you mean into and out of the screen (since x is horizontal and y is vertical in the 2D solver). The default value for the depth in Fluent is 1m. You set the depth as one of your reference values (report->reference values). It doesn't do any caculations in the third dimension when you are using either of the 2D solvers. The only time the third dimension comes into play is when you are getting results out of Fluent, it integrates them over the depth defined in the reference values.

Hope this helps, and goodluck, Jason

Thanks again for answering.Let us say I have 2d grid in the left i have velocity_input zone. Now I am reporting the surface area of this zone. Can you tell me how this surface area calculated. I guess using the default value of 1 m is it correct. so one must take great care when imposing the mass flow rate boundary condition in 2d cases Y

The area of this boundary codition is height*depth... height is what's actually modeled (in the y-direction) and depth is what's defined in the reference values. You can do one of two things... keep the default depth value of 1m, and just remember that everything you calculate is per meter of depth (if you're working in inches, then set the depth to 1inch and remember that everything is per inch of depth... remember that if you aren't working in meters that you HAVE to set this even if you change the units... Fluent will keep the depth at 1m, or 39.something inches unless you change it). The other option is to put in whatever depth you actually have... lets say you're modeling a 2D duct that is 8m in the z-direction, then set your depth to 8m! If you set the depth to whatever depth you actually have, then you can set your mass flow rate to whatever mass flow rate you actually have. IF you leave the depth at 1m, then you should divide your mass flow rate by whatever depth you have (assuming you're working in meters) to get a mass flow / meter of depth, then use this value as your boundary condition.

Hope this helps, and goodluck, Jason