Hi all, I have modeled an air duct with Y â€"connection with one inlet and two outlets. I wanted to find out the pressure loss coefficient for the Y-fittings. The inlet flow velocity is defined. My questions are :

Is it possible to force any condition at the outlet so that the flow is equal in both the branches (though it is not practical)?what type of boundary condition should be applied??

Is the pressure value in the inlet will be atmospheric or we have to define that??

Any suggestions are highly appreciated.

Thanks!!

For the outlets, use the outlet BC with split ratio of 0.5 for both the outlets. Essentially when you have multiple outlets, this is the procedure...just make sure that the split ratio adds upto one. Pressue loss coefficient is a function of the pressure drop and the volumetric flow rate. Hope this helps !!

what mike saied could be right

It is right !!

Thanks Mike,i really appreciate it. I did what you suggested but the solution is not converging.The residual tolerance was set to 0.0001 but when it reaches 0.001 the solution is getting oscillated.i did chek for errors in mesh quality and stuff but evrything is fine.The inlet velocity was defined as 4 m/s.Its a steadystate,high Re.No K-E model with incompressible flow. could you tell me what kind of changes should i do to satisfy the convergence criteria(i know its hard to give any suggestion without knowing much details.pls let me know wot kind of details to be specified??)

Anybody's input is highly appreciated.

thanks.

i am also getting the following warning :

*** WARNING #001 *** FLUID INFLOW DETECTED AT SOME OUTFLOW BOUNDARIES WHERE MASS FLUXES ARE FORCED TO ZERO.

IF THIS CONDITION PERSISTS, YOUR RESULTS MIGHT BE WRONG

THE OUTFLOW BOUNDARY MIGHT NOT BE WELL SPECIFIED OR THE GRID MIGHT BE TOO COARSE NEAR THE OUTFLOW BOUNDARY

but the grids seem to be fine?how to get rid of this problem?

thanks!!

Almost certainly you have a recirculation zone that is extending to the boundary.

In some cases you end up with recirculations that stretch out further than you would physically expect. One solution (if the geometry and overall problem specification allow) is to put a contraction in to close them off.

Other solutions include extending the model sufficiently to allow them naturally to close.

Note that putting a 50/50 flow split on a two manifold problem is in effect defining the answer. If the resistance is different to the two outlets the flow split would, in reality, be different.

Defining BCs for a manifold splitting is always problematic as you often have to 'know' more than you really do and therefore your BCs are in danger of defining the answer rather than letting the code work it out for you.

In a case where the flow rejoin (i.e. a car HVAC system) modelling to the point where the flows rejoin may be possible.

In other cases you may need to look at the solution and assess whether the BCs you are placing on the model are correct and whether the model domain is sufficient to allow the code to really have a chance of making the correct calculation.

If you run a single iteration with

RESDATA 0 1

turned on it will write out a file of the cell residuals that you can TRLOAD.

This allows direct display of where the errors are. However it is rarely more use than simply looking at the flow field itself as it is usually obvious from the flow structures where the code is having problems.

James, Thanks for ur input.