[Jordan1997]

Hi there, my deadline for my senior project is fast approaching and any help would be extremely appreciated right now!

Using Star-CCM I'm modelling an external aerodynamics simulation of a fixed wing UAV (see attached photos). I have run preliminary simulations using the realizable k-epsilon turb model with a target Y+ of 30, all converged nicely.

I have separate surface controls for each of my surfaces, and upon running a drag report for each surface I'm getting some as positive and some as negative?? In this case my fan, hinge point and wing/fuselage joint are fine, but the fuselage, H-Tail, V-Tail and Wing all are producing negative results? I think the report is set up correctly.

To add to it, upon looking at the y+ in a scalar field I notice there are some missing sections of the geometry in the scene which have not appeared anywhere else. (See Photo)

Any ideas please, again any help would be much appreciated.

[ping]

the white patches in your scalar scenes are caused by your scalar setting of the clip values in the displayer and are not holes etc.
it is possible to have negative drag but not like you have on your major surfaces so you need to check the direction of the force report and even the flow with some section planes of velocity vectors although your pressure scalar looks reasonable. are you measuring force on the correct boundary surfaces.

[Jordan1997]

Thank you for your reply

My aircraft is aligned so that the z direction is downstream, the y direction is up and the x direction is spanwise i.e. My flow direction in my hemisphere region to achieve my small AoA is therefore (0.0, 0.02793, 1.0) and the velocity vector in my initial conditions is (0.0, 0.83758, 29.988)m/s.

In this way my flow direction in my drag report is also (0.0, 0.02793, 1.0). I've resolved the forces on each surface in each component and cant make any sense of it.

Velocity vectors look fine, certainly nothing that doesn't look streamwise?

If I select the boundary either under the parts-subtract-surface or under region-boundary-surface it returns the same force.

Feel like must be something in my report but not sure how?

[ping]

having commented that your pressure scene looks okay i now notice that the pressure field function is relative pressure and you have values of 10^5 and this is not good practice - relative pressure should be hovering around zero to ensure accuracy - i assumed you were displaying absolute pressure. so you need to run it again with the reference pressure set correctly - read about the numerical inaccuracies that you are causing at this help topic Simulating Physics > Flow and Energy > Pressure > Defining the Reference Pressure, and also ensure your reference location is in a nice place.
since force is a combination of pressure and the area it acts on this could be the cause of you problem.

[Jordan1997]

Lifesaver, my results make far more aerodynamic sense now and the relationships between surfaces seem reasonable too. Thanks for the reply and directing me to the appropriate page in the user guide