Assuming I'm modelling the flow through a nozzle. For the boundaries I defined one velocity inlet and one pressure outlet. The pressure drop through the nozzle is quite large (about 1000E05 Pa). Since I have nothing to compare my results, I generated first different grids (structured, unstructured, finer and coarser resolution, but all adapted), which I was secondly testing with different models (in my case laminar investigation, RNG k-e + differential equation for tubul. viscosity and Spalart Allmaras -> it is likely that in my problem the low Re number effects are pervasive beside adverse pressure gradients in the boundary layer, whereby the high Re effects may also be not negligible). Well, looking on the main results, it can be summarised that: - the upper range of the static pressure at the inlet is for the unstructured mesh about 10% higher than for the structured case (both with RNG and comparable number of elements) - coarse and fine (structured) grids lead to similar results (both with RNG) - looking just the structured, fine grid: RNG and laminar leads to similar results, Sp-Al model differs just in the calculated upper range of the static pressure at the inlet (10% higher than with other models) (you can assume that all models reached a sufficently converged solution)

my questions: - is it possible to say if the difference in the upper range of the static pressure (10%) between sturctured and unstructured is normal (quality of structured mesh is better, also are the gradients from cell to cell a bit smaller)? - and in the same way: is it possible that there is such a big difference (10%) for the static pressure value at the inlet when using different turbul. models? I mean, even a model (Sp-Al) is not best suited for a problem, are there such differences likely or must there be a mistake somewhere in the setup (what I do not belive) ? - total different question: beside comparing the results with experiment or publications, can anyone give me an advice based on his experience, how he would start in order to get a feeling in which way the "journey" goes? (let's say that at this stage very few details are known of the problem)

(1). Nozzle is a standard device. (2). It can be a subsonic nozzle for metering purpose, or it can be a supersonic nozzle. (3). The nozzle flow has been studied for a long time, and you can use 1-D analysis, 2-D inviscid analysis, and 2-D (or 3-D) viscous analysis. (4). In the nozzle analysis, you need to know the pressure ratio (inlet total to exit static), and also the Reynolds number. (5). If you are getting 10% variation in static pressure , then I think, it is well above the acceptable engineering range of 5%. And I am sure that the skin friction coefficient will be totally off the scale. Check the skin friction first for each cases. (6). It is a good exercise. But if you are the chief scientist of a company, then I guess you will have to work harder. What do you think? (you didn't say what codes you are using in the calculation )

.. thank's John for your reply. 1 to 3) To be honest I have to say that I haven't described all the details about the nozzle. But you can believe me that this "nozzle" flow I'm investigating is not a "standart" design (e.g. I have to make 3d analysis because of the special features). 4) pressure ratio inlet to outlet is about 10:1, Re number varies between 660 and 6000 (Ok, 6000 sounds not so extrem high) 5) ...thanks for the hint about skin friction. I compared the models and grids on their skin friction coefficient. Surprisingly (?!) they are all in the same range (max value between 10 and 16... so all are equally bad or good (I don't know if these values are in general too high)) -> by the way, I used for the turbulence models the two-layer zone model; for all models I could accordingly generate a mesh (structured or unstructured) which is sufficently resolved near the walls (y+ <= 4; definition for y+ like in Fluent) 6) The code I'm using right now is Fluent. ... well, I'm not chief scientist of a company. Actually I would describe myself as a beginner in CFD with basic background in flow physics... but anyway I will work harder!

But thanks a lot (once more) for your comments!

With choked nozzle flows what is important are the inlet boundary conditions. You can impose massflow (adapts your inlet total conditions), or you can impose total conditions (adapts mass flow). If you impose massflow then a change in effective geometry (due to boundary layers) will increase your inlet total pressure. This all holds if you have a subsonic to supersonic flow in your nozzle (Mach=1 in the effective nozzle throat). Normally when you compare CFD with experiments you impose total conditions as you measure these (normally). Maybe this helps.

(1). Regardless of how you calculate it, you can take a look at the flow behavior in the inlet wall region up to the nozzle. (2). You should be able to see the difference between two calculations in terms of the velocity field, and the pressure field. (3). I mean, you nozzle inlet wall in principle should act like the leading edge of a wall,with zero boundary layer thickness there. (4). So, in the axial direction, in the inlet region, increase the mesh density there, as if you are computing the flow development at the entrance of a duct. This is important because Re is relatively low. What I am saying is: try to simulate the nozzle inlet as the duct entrance condition with zero boundary layer thickness. (5). If you have a duct ahead of the nozzle, you could try to simulate the boundary layer profile at the nozzle inlet. (6). The other way to test the setup and the code is to increase the Reynolds number so that you have relatively thin boundary layer on the wall. And you should see the better agreement between various cases. If you don't, then the code is not reliable. (7). So, you should see better agreement for high Reynolds number cases.