Learning Forum

[viv_vid]

Hello Everyone,

I am working on a project wherein I am studying the flow from a nozzle and analyzing the velocity distribution. The following figures show the inlet and outlet boundaries which I set initially

[aitor.amatriain]

Could you please show us some pictures of the mesh? Have you tried first to solve the same case but with single flow?

[Rob]

Did you do share topology in SpaceClaim? If yes, do you have any wall and wall:shadow pairs in the model? If no, did you do anything with the mesh interface set up in Fluent?

[viv_vid]

Dear Aitor these are the mesh pictures and yes I initialy tried with only water(without air) for the first case where the inlet was different. For the second case I have not yet tried that.
I also noticed that in fluent the inlet direction seems to be reversed somehow.


To answer you Rob yes I did share the topology. I do not have any wall shadow pair in the model and no I did not mess with the mesh interface. My archive file size is greater than 50mb therefore I am not able to attach it here. but I can provide you with the pictures if they are needed.
Thankyou

[Rob]

Ah, did you label the face that's between the nozzle and airbox?

[viv_vid]

Yes I labeled that face( which connects the nozzle and the airbox) as inlet. As shown below

[Rob]

OK, there are some hard coded labels that set stuff in Fluent. Inlet, outlet, wall etc. That surface is an "interior" type, but has been forced to be an inlet. If you're lucky it's fixable in Fluent. Change the boundary type to "wall". This should give a wall & wall:shadow. Then turn the wall to interior.

[viv_vid]

Thankyou for suggesting me this Rob. I did that and changed the wall to interior. Should I then change the zone name now to Inlet?
For now there is no inlet...so only wall and outlet..Where should I give the inlet conditions then in fluent?

[viv_vid]

These are the boundary conditions I see now

[Rob]

Are the wall and outlet adjacent to each other? This also means you don't have a flow boundary for the faces at the extreme +/- x direction. I think you'd better revert to Meshing and fix it there. It's doable in Fluent, but needs some knowledge of the mesh manipulation tools: I don't advise going that route at this point in your CFD career.

[viv_vid]

Yes the walls and outlet are adjacent to each other as shown

I did not understand the part where you mentioned about flow boundary at the extreme face. Could you explain me how to do it in the Meshing?

[Rob]

Use Named Selections. The face that's common to the two volumes should be interior. In the above the outlet is the face coloured in red.

[viv_vid]

So you mean I shoud put inlet at the starting point of the nozzle and outlet same as above at the extreme end of the box and in between where the two volumes share the face, put that as interior right?

[Rob]

Correct. There are two types of surface boundary in Fluent, internal and external. Internal have cells on both sides, and a limited set of options: that doesn't include inlets & outlets. External bc's are just that, and have inlets, outlet, symmetry etc available.