CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Non overlap area fractions (http://www.cfd-online.com/Forums/cfx/84850-non-overlap-area-fractions.html)

saisanthoshm88 February 10, 2011 01:10

Non overlap area fractions
 
I'm simulating a problem that involved a number of mesh interfaces the problem is that my solution doesn't converge. My suspicion to this is that there may be a refinement problem at the interface regions.
The following are the non over lap area fractions for the interfaces in my domain:


I have a rotary domain in the set up.So Interface7 is a Frozen rotor interface.

And actually the surfaces for side1 and then of side2 of any interface exactly match with each other however there is a difference in the mesh resolution which indeed results in the so called non overlapping area fractions.

Discretization type = GGI

Intersection type = Bitmap
Domain Interface Name: Interface1
Non-overlap area fraction on side 1 = 1.25E-07
Non-overlap area fraction on side 2 = 2.28E-07
Domain Interface Name: Interface2
Non-overlap area fraction on side 1 = 4.02E-04
Non-overlap area fraction on side 2 = 5.28E-03
Domain Interface Name : Interface3
Non-overlap area fraction on side 1 = 1.12E-07
Non-overlap area fraction on side 2 = 5.60E-08
Domain Interface Name : Interface4
Non-overlap area fraction on side 1 = 3.97E-08
Non-overlap area fraction on side 2 = 1.57E-04
Domain Interface Name : Interface5
Non-overlap area fraction on side 1 = 8.62E-04
Non-overlap area fraction on side 2 = 1.17E-04
Domain Interface Name : Interface6
Non-overlap area fraction on side 1 = 3.57E-03
Non-overlap area fraction on side 2 = 7.94E-08
Domain Interface Name : Interface7
Non-overlap area fraction on side 1 = 1.23E-06
Non-overlap area fraction on side 2 = 6.40E-05

Can some one please look at these values and suggest the interface regions which need more refinement.

Thanks in advance.



ghorrocks February 10, 2011 04:18

You cannot tell much from the numbers alone. You will have to post an image of the geometry and an image of the interface meshes.

saisanthoshm88 February 10, 2011 06:29

Well, Glenn please find a ppt that contains the images of my mesh on the link: http://www.2shared.com/document/UxwL...sh_images.html

I couldn't show the geometry as it's quite big but any way my application is to analyze the hot air flow in a oven.

ghorrocks February 10, 2011 17:12

You may have a problem with the coarse mesh on the curved intersections.

But how significant are the non-overlap areas reported? If they are a fraction of a percent then ignore them, they are just discretisation error. If they are signficant you have a problem.

saisanthoshm88 February 10, 2011 23:17

Yep as you see them in my first post, the non overlap areas are only a fraction of a percent but can there be a problem if the volume mesh is coarse in some region and can you please tell me of some way to check these extent of non overlaps in CFX-pre itself instead of proceeding all the way to the solver.

ghorrocks February 10, 2011 23:30

Non-overlaps caused by surfaces not in contact can be seen in CFX-Pre or the solid modelling package or mesher. The interface is intersected in the solver so there is no other way that I am aware of.

saisanthoshm88 February 11, 2011 02:51

Thanks Glenn, well I just saw the Mesh visualization advice in the CFX documentation.For a better convergence do I really need to maintain all the criteria as recommended (or) will it be fine if I maintain only the element volume ratios as suggested and Ignore the rest of the criterion like: Max. face angle, Min.face angle, Edge length ratio, connectivity number.

And moreover can you please suggest me of some way to know the number of elements in the mesh volume that seem to violate the recommendation for a particular criterion , as of now I'm just able to view such elements by creating some Isovolumes in CFX-post, is there a better way of doing this.

As of now, i've acheived a convergence till the residual target of 1.E-03 but i'm trying to have it till 1.E-04.So I'm just trying out different approaches,i'm also considering upon setting a physical Time step so :

1. Can you please tell me how to calculate the physical time step, my problem is to analyze the hot air flow in a heating oven. The domain doesn't have a inlet and outlet it's like there is a rotating fan with a heating element around it. So it sends in hot air into the oven and the air flows over the trays.

2. Can you please suggest me some generic monitor points for such case.

Thanks in advance!

ghorrocks February 11, 2011 05:05

How important each mesh quality parameter is will depend on the simulation you are doing. But in general the comments in the documentation are correct, you want your mesh to achieve all the quality requirements for the best chance of success.

The number violating is not really of interest, merely the fact that some do violate. So I would not bother trying to count them, just fix up your mesh and eliminate them.

Your convergence problems may well be caused by your mesh quality problems. Time improving mesh quality is always worth while.

Is your simulation steady state or transient?

saisanthoshm88 February 11, 2011 08:05

Glenn, it's a steady state simulation but I was just considering the approach of choosing a physical time scale instead of the Auto time scale to check if that helps convergence but I didn't know how to calculate the physical time scale.

sercro April 26, 2011 13:05

There is some guidelines on how CFX calculates the timescale when the "Autotimescale" function is on. It can be found in the ANSYS CFX-Pre guide or the ANSYS-Modeling guide (most likely the latter, I'm not sure). In these references you can also find a way to estimate a physical timescale.

Usually is a factor that considers the dimensions of the domain and the flow speed (so it involves the residence time inside the domain). There are some rules of thumb, i.e., for turbomachinery it is common to use a physical timescale = 1/n (n: rotational speed in rad/s). Maybe you can find something similar for your problem.


All times are GMT -4. The time now is 07:08.