You appear to have two completely different physical problems set up - one (the lower picture) has a single inlet, a plugged branch (no flow), and an outlet; the second (upper picture) has two inlet flow branches and an outlet. Why would you not expect completely different flow fields from completely different boundary conditions?

"Both have the same geometry, input pressure, and outlet flow rate."

So what? You have one case with one inlet, and the other with two. Surely, the case with two inlets will have a lower velocity than the case with only a single inlet. I see no mystery here. Mass flow = velocity*cross-sectional area*density, cut the area in half, the velocity needs to double.

TTFN
FAQ731-376: Eng-Tips.com Forum Policies

Need help writing a question or understanding a reply? forum1529: Translation Assistance for Engineers

And two inlets = mixing flow vs. no mixing for a single inlet...

I would appear I didn't explain the setup quite clearly enough. For the top case I have two inlet boundary conditions (one condition for each face with an arrow pointing in) set up at 20 psi each, and a mass flow rate of 83.4 lbm/s. The lower case has one inlet boundary condition (one condition that includes both faces with arrows pointing in selected) which has 20 psi going into both inlets, and the same mass flow rate.

Essentially in both cases there are two faces with 20 psi and one outlet with 83.4 lbm/s. My confusion is why the simulation would be different if I used two different setups to simulate exactly the same physical condition. I uploaded the picture again, hopefully the situation is a little more clear.

• http://files.engineering.com/getfile.aspx?folder=6ddd649f-e4ae-421b-8391-0b

Again, it's not the same condition. I'm struggling to understand why you can't see that. In one case you have 83.4 lbm/s going into a single inlet, while in the other case, the same mass flow is going into two inlets. How is that the same condition?

TTFN
FAQ731-376: Eng-Tips.com Forum Policies

Need help writing a question or understanding a reply? forum1529: Translation Assistance for Engineers

"in both cases there are two faces with 20 psi and one outlet with 83.4 lbm/s."

I don't think the second face is getting the boundary condition you think it's getting. There is either a software or input file glitch. Are you sure the vector sign is correct on both faces?

Based on these setup pictures it would seem to me that the vectors are pointing in the right direction.

IRstuff - the reason that this should be the same condition is because Ansys allows you to select multiple faces for one inlet boundary condition. So instead of creating a second boundary condition I included both inlet faces on the same condition. It's clear that Ansys does not treat multiple face input the same as the two individual single face boundary conditions, but what I am trying to understand is why.

I have a feeling that Ansys is written in such a way that it chooses only one face of the two selected and just ignores the other one. I would like to be able to combine both inlet faces into one so that I ensure they both have the same conditions all the time since I will be iterating through different inlet conditions.

• http://files.engineering.com/getfile.aspx?folder=35af7ed3-1faf-4227-8909-aa

Could it be due to the different turbulence boundary conditions you're using in the first example (with the two inlet boundary conditions)? Inlet Two you're basically fixing the eddy viscosity and intensity to a certain percentage of the flow rate (I forget exactly how CFX works that out), and (again from memory) the Zero Gradient boundary kind of settles itself out based on the rest of the flow field - so you could find that where you expect the flow conditions to be 'exactly the same', the different turbulence conditions are having a big influence on the flow. Not sure whether the effect should be of that magnitude, but try running it with the same turbulence boundary conditions and see what you get?

Also, I know it's not always easy to do, but having the inlets so close to an area of quite large flow gradients certainly isn't recommended - the courses I did for CFX all had the recommendation for the inlet to be maybe 10-20 diameters away from areas of large flow gradients. This helps minimise the effects of the boundary conditions on the interesting area of the flow - the turbulence equations have time to settle themselves out if they aren't very accurately set. I remember seeing examples with quite large differences in results, simply based on where the inlet was located.