CFX Post- Force function problems?

watttt · November 12, 2012, 05:47

Hi there,

I am currently trying to simulate a simple prolate ellipsoid (http://en.wikipedia.org/wiki/Ellipsoid) in a fluid flow. But I am currently having problems showing that the simulation is independent of the position of the outlet. I have set the outlet as an average static pressure of 0 and can see form a pressure plot on the sym plane that the pressure has stabilised behind the object. But whenever I lengthen/shorten the outlet the drag force (calculated using the force function) changes! To make matters worse it doesn’t even change in a pattern, the force just randomly jumps about by 10% both up and down. Has anyone ever seen this before? The mesh I am using is consistent between all runs and looks pretty reasonable. This makes me think its a problem with the force function? I could be wrong through. Its driving me nuts!

Thanks

murx · November 12, 2012, 09:57

Hi,

unfortunately I do not have a solution for your problem. But have you tried to calculate the forces manually by integrating the inertial and viscous forces around the elipsoid?
e.g. areaInt_x(Pressure)@elipsoid + areaInt(Wall Shear X)@elipsoid
Does the resulting value show the same behaviour as the force functions?

Maybe this can give you a hint where your problem originates from.
I have some similiar problem where the manual integration always differs from the force functions.

ghorrocks · November 12, 2012, 17:35

Can you post an image of your body and the outlet position? Also include some mesh details.

watttt · November 14, 2012, 09:01

Quote:

Originally Posted by murx

Hi,

unfortunately I do not have a solution for your problem. But have you tried to calculate the forces manually by integrating the inertial and viscous forces around the elipsoid?
e.g. areaInt_x(Pressure)@elipsoid + areaInt(Wall Shear X)@elipsoid
Does the resulting value show the same behaviour as the force functions?

Maybe this can give you a hint where your problem originates from.
I have some similiar problem where the manual integration always differs from the force functions.

Interestingly this manual calculation does differ to that force function, but it still shows the same problems I was having before.

Quote:

Originally Posted by ghorrocks

Can you post an image of your body and the outlet position? Also include some mesh details.

I have attached some pictures of the mesh

Defauly body spacing=0.7m
default face=0.035-0.7
face on body=0.03-0.031 with 50deg angular resolution
infaltion= 5 layers max height 0.01m
Max yplus=17

Inlet: 3m/s Medium Turbulence
Outlet: Average Static Pressure over whole outlet 0 Pa Relative

Looking at the forces given in the .out file it also varies between outlet lengths. So maybe it is something to do with my mesh.

ghorrocks · November 14, 2012, 17:45

Your mesh does not have inflation layers. Alternately the inflation layers are so small that the transition from the inflation layers is terrible. Yes, the problem is your mesh.

You need to use inflation layers for any flow which generates a significant boundary layer, and the transition from the inflation layers to the bulk mesh need to have roughly the same volume elements on both sides. You might also need to refine the wake area a bit.

November 12, 2012, 05:47	CFX Post- Force function problems?	#1
watttt New Member Join Date: Feb 2012 Posts: 3 Rep Power: 14	Hi there, I am currently trying to simulate a simple prolate ellipsoid (http://en.wikipedia.org/wiki/Ellipsoid) in a fluid flow. But I am currently having problems showing that the simulation is independent of the position of the outlet. I have set the outlet as an average static pressure of 0 and can see form a pressure plot on the sym plane that the pressure has stabilised behind the object. But whenever I lengthen/shorten the outlet the drag force (calculated using the force function) changes! To make matters worse it doesn’t even change in a pattern, the force just randomly jumps about by 10% both up and down. Has anyone ever seen this before? The mesh I am using is consistent between all runs and looks pretty reasonable. This makes me think its a problem with the force function? I could be wrong through. Its driving me nuts! Thanks

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
[Other] mesh airfoil NACA0012	anand_30	OpenFOAM Meshing & Mesh Conversion	13	March 7, 2022 18:22
[blockMesh] error message with modeling a cube with a hold at the center	hsingtzu	OpenFOAM Meshing & Mesh Conversion	2	March 14, 2012 10:56
Force can not converge	colopolo	CFX	13	October 4, 2011 23:03
Force Report help~ or maybe Custom Field Function	sailor	FLUENT	0	April 13, 2011 04:45
viewing cfx post while working on cfx solver manager	HMR	CFX	5	March 9, 2011 23:33

November 12, 2012, 09:57		#2
murx Member Max Join Date: May 2011 Location: old europe Posts: 88 Rep Power: 15	Hi, unfortunately I do not have a solution for your problem. But have you tried to calculate the forces manually by integrating the inertial and viscous forces around the elipsoid? e.g. areaInt_x(Pressure)@elipsoid + areaInt(Wall Shear X)@elipsoid Does the resulting value show the same behaviour as the force functions? Maybe this can give you a hint where your problem originates from. I have some similiar problem where the manual integration always differs from the force functions.

November 12, 2012, 17:35		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,862 Rep Power: 144	Can you post an image of your body and the outlet position? Also include some mesh details.

November 14, 2012, 17:45		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,862 Rep Power: 144	Your mesh does not have inflation layers. Alternately the inflation layers are so small that the transition from the inflation layers is terrible. Yes, the problem is your mesh. You need to use inflation layers for any flow which generates a significant boundary layer, and the transition from the inflation layers to the bulk mesh need to have roughly the same volume elements on both sides. You might also need to refine the wake area a bit.