Angle of attack of far field inlet not constant throughout the domain

SBH_ · November 26, 2018, 08:29

Hello, I am trying to simulate the intake performance in a turbofan at climb conditions, where I have an AoA of 22 degrees. My domain is a box, where one face is set as inlet and the others as openings. At the inlet I specify my angle of attack by decomposing the velocity in Cartesian components, however as seen from the picture attached the direction of the flow comes back to axial direction downstream in the domain.

I have tried to rotate my mesh and kept constant the axial velocity, and also set more faces as inlets but nothing. Any suggestions??

ghorrocks · November 26, 2018, 17:02

You need your top and bottom domain faces as inlet as well.

SBH_ · November 27, 2018, 08:38

The issue was that the inlet domain was initialized with axial velocity. Now the problem I am having is with convergence. The strategy I have been following for the case with no angle of attack has been as follows, with no problems:

Turbulence scheme: 1st order
Advection scheme: Upwind
Auto Timescale factor 1 for 200 iterations

Turbulence scheme: 2nd order
Advection scheme: 2nd order
Auto Timescale factor 1 for 200 iterations
Auto Timescale factor 2 for 200 iterations
Auto Timescale factor 5 for 200 iterations
Auto Timescale factor 10 for 200 iterations

However now, with an angle of attack, at Auto Timescale factor 1 it crashes, so I am trying with local time scale instead:

Turbulence scheme: 1st order
Advection scheme: Upwind
Local Timescale factor 2 for 200 iterations

Turbulence scheme: 2nd order
Advection scheme: 2nd order
Local Timescale factor 2 for 200 iterations
Auto Timescale factor 1 for 200 iterations
Auto Timescale factor 2 for 200 iterations
Auto Timescale factor 5 for 200 iterations
Auto Timescale factor 10 for 200 iterations

Does it make sense to you? Any other idea for the convergence strategy?

Thanks in advance.

ghorrocks · November 27, 2018, 18:26

Hard coding a time step is not much good in a steady state simulation. A much better way of doing it is to start with a small time step and adjust it as you go using "Edit run in progress". If the simulation is monotonically converging then increase the time step, if it is starting to diverge then decrease the time step.

Also read this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria (including the bit about local time scale factor)

SBH_ · November 28, 2018, 09:48

It actually did converge with this strategy so problem solved. Thanks a lot for your help!

November 26, 2018, 17:02		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,917 Rep Power: 145	You need your top and bottom domain faces as inlet as well. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

November 27, 2018, 18:26		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,917 Rep Power: 145	Hard coding a time step is not much good in a steady state simulation. A much better way of doing it is to start with a small time step and adjust it as you go using "Edit run in progress". If the simulation is monotonically converging then increase the time step, if it is starting to diverge then decrease the time step. Also read this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria (including the bit about local time scale factor) __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
decomposePar problem: Cell 0contains face labels out of range	vaina74	OpenFOAM Pre-Processing	37	July 20, 2020 06:38
Periodic Pressure drop	cfd_begin	CFX	10	May 25, 2017 08:09
Out File does not show Imbalance in %	Mmaragann	CFX	5	January 20, 2017 11:20
Pressure distribution on a wall	darazsbence	CFX	17	October 6, 2015 11:38
angle of attack	kiran	FLUENT	0	September 10, 2004 09:18

November 27, 2018, 08:38		#3
SBH_ New Member salva Join Date: Jul 2018 Posts: 3 Rep Power: 8	The issue was that the inlet domain was initialized with axial velocity. Now the problem I am having is with convergence. The strategy I have been following for the case with no angle of attack has been as follows, with no problems: Turbulence scheme: 1st order Advection scheme: Upwind Auto Timescale factor 1 for 200 iterations Turbulence scheme: 2nd order Advection scheme: 2nd order Auto Timescale factor 1 for 200 iterations Auto Timescale factor 2 for 200 iterations Auto Timescale factor 5 for 200 iterations Auto Timescale factor 10 for 200 iterations However now, with an angle of attack, at Auto Timescale factor 1 it crashes, so I am trying with local time scale instead: Turbulence scheme: 1st order Advection scheme: Upwind Local Timescale factor 2 for 200 iterations Turbulence scheme: 2nd order Advection scheme: 2nd order Local Timescale factor 2 for 200 iterations Auto Timescale factor 1 for 200 iterations Auto Timescale factor 2 for 200 iterations Auto Timescale factor 5 for 200 iterations Auto Timescale factor 10 for 200 iterations Does it make sense to you? Any other idea for the convergence strategy? Thanks in advance.

November 28, 2018, 09:48		#5
SBH_ New Member salva Join Date: Jul 2018 Posts: 3 Rep Power: 8	It actually did converge with this strategy so problem solved. Thanks a lot for your help!