sliding mesh problem in CFX

haribhaskaran · September 17, 2015, 11:41

I have attached the pdf with the cfx drawing. The overlap region is supposed to change with time. The pitch on both sides of the interface is the same (360 Deg). Therefore, I gave the pitch change option to be none. In that case, flow does not occur through the non overlap regions.

However, CFX does not update the overlap areas with time. Therefore, CFX calculates the flow with the original overlap areas and does not take into account the change in the overlap regions in subsequent time steps.

ghorrocks · September 17, 2015, 18:45

This is not correct. A TRS interface is recalculated every time step and I have used this many times. Something is wrong with your simulation if this is not happening.

Please post your CCL.

haribhaskaran · September 18, 2015, 09:38

I have attached the pdf with the CCL.

ghorrocks · September 19, 2015, 06:45

I see two main issues - you are fiddling with the GGI intersection parameters. Leave these at default; and you are using mesh motion but not defining any mesh motion. Your simulation is a rotating frame of reference simulation, so remove the mesh motion settings.

Some other points:

Why are you using a complex function to control time step size? It is much easier to use adaptive time stepping homing in on 3-5 coeff loops per iteration and it looks after itself. Your complex function is going to be a lot of work to do sensitivity analysis on (and if you have not done a sensitivity analysis it is bound to be wrong).

You appear to have mesh motion and rotation on the air top domains, and mesh motion on the stationary domain. Is this what you intended?

You appear to have defined a gravity direction. Why have you done this? Is gravity important in this simulation (it does not appear to be)?

You appear to be using zero reference pressure. You should put a pressure equal to the typical pressure in the simulation, or something close to it. I realise your pressures are low in this simulation so you should use that as a reference pressure, not zero.

You appear to be using the high speed turb wall functions model. Why is that?

You appear to be using the viscous work model. Why have you done this? Is it significant? It would not appear to be.

You appear to be adjusting a lot of GGI intersection control parameters. Why are you doing that? I have never had to adjust these ever. Just leave them at defaults.

You are also setting a lot of advanced solver settings: Compressibility control, interpolation scheme, intersection control. Why are you doing this? You should be leaving these as defaults unless you have a very good reason to change them.

haribhaskaran · September 22, 2015, 08:57

Thanks a lot for all the feedback Glenn

I had another question regarding the flow through a boundary. If I want to find the total flow through the boundary until a particular time-step and use it to define the boundary condition, is there a way to do it ?

Antanas · September 22, 2015, 10:53

Quote:

Originally Posted by haribhaskaran

Thanks a lot for all the feedback Glenn

I had another question regarding the flow through a boundary. If I want to find the total flow through the boundary until a particular time-step and use it to define the boundary condition, is there a way to do it ?

Hmm... Maybe... create massflow monitor and then export curve data to csv and integrate it for ex. in matlab. If timestep is constant then you may try to use monitor statistics to get time integral of monitor.

Mazze[ITA] · September 11, 2021, 07:38

The problem is clearly the non-overlapped region. The non-overlapped region of the upstream interface should communicate with the non-overlapped region of the downstream region.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
3D Hybrid Mesh Errors	DarrenC	ANSYS Meshing & Geometry	11	August 5, 2013 06:42
Convergence moving mesh	lr103476	OpenFOAM Running, Solving & CFD	30	November 19, 2007 14:09
How to control Minximum mesh space?	hung	FLUENT	7	April 18, 2005 09:38
sliding mesh problem	annie	FLUENT	0	November 5, 2004 07:47
CFX Mesh problem	Atit Koonsrisuk	CFX	4	October 5, 2004 08:14

September 17, 2015, 18:45		#42
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,718 Rep Power: 143	This is not correct. A TRS interface is recalculated every time step and I have used this many times. Something is wrong with your simulation if this is not happening. Please post your CCL.

September 19, 2015, 06:45		#44
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,718 Rep Power: 143	I see two main issues - you are fiddling with the GGI intersection parameters. Leave these at default; and you are using mesh motion but not defining any mesh motion. Your simulation is a rotating frame of reference simulation, so remove the mesh motion settings. Some other points: Why are you using a complex function to control time step size? It is much easier to use adaptive time stepping homing in on 3-5 coeff loops per iteration and it looks after itself. Your complex function is going to be a lot of work to do sensitivity analysis on (and if you have not done a sensitivity analysis it is bound to be wrong). You appear to have mesh motion and rotation on the air top domains, and mesh motion on the stationary domain. Is this what you intended? You appear to have defined a gravity direction. Why have you done this? Is gravity important in this simulation (it does not appear to be)? You appear to be using zero reference pressure. You should put a pressure equal to the typical pressure in the simulation, or something close to it. I realise your pressures are low in this simulation so you should use that as a reference pressure, not zero. You appear to be using the high speed turb wall functions model. Why is that? You appear to be using the viscous work model. Why have you done this? Is it significant? It would not appear to be. You appear to be adjusting a lot of GGI intersection control parameters. Why are you doing that? I have never had to adjust these ever. Just leave them at defaults. You are also setting a lot of advanced solver settings: Compressibility control, interpolation scheme, intersection control. Why are you doing this? You should be leaving these as defaults unless you have a very good reason to change them.

September 22, 2015, 08:57		#45
haribhaskaran New Member Hari Subramaniam Bhaskaran Join Date: Sep 2015 Posts: 7 Rep Power: 10	Thanks a lot for all the feedback Glenn I had another question regarding the flow through a boundary. If I want to find the total flow through the boundary until a particular time-step and use it to define the boundary condition, is there a way to do it ?

September 11, 2021, 07:38		#47
Mazze[ITA] Member Lorenzo Mazzei Join Date: Dec 2010 Posts: 60 Rep Power: 15	The problem is clearly the non-overlapped region. The non-overlapped region of the upstream interface should communicate with the non-overlapped region of the downstream region.