Non overlap area fractions

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 10, 2011, 01:10 Non overlap area fractions #1 Senior Member   --------- Join Date: Oct 2010 Posts: 303 Rep Power: 17 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. __________________ Best regards, Santhosh. Last edited by saisanthoshm88; February 10, 2011 at 02:58.

 February 10, 2011, 04:18 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 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.

 February 10, 2011, 06:29 #3 Senior Member   --------- Join Date: Oct 2010 Posts: 303 Rep Power: 17 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. __________________ Best regards, Santhosh.

 February 10, 2011, 17:12 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 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.

 February 10, 2011, 23:17 #5 Senior Member   --------- Join Date: Oct 2010 Posts: 303 Rep Power: 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. __________________ Best regards, Santhosh.

 February 10, 2011, 23:30 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 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.

 February 11, 2011, 02:51 #7 Senior Member   --------- Join Date: Oct 2010 Posts: 303 Rep Power: 17 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! __________________ Best regards, Santhosh. Last edited by saisanthoshm88; February 11, 2011 at 04:20.

 February 11, 2011, 05:05 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 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?

 February 11, 2011, 08:05 #9 Senior Member   --------- Join Date: Oct 2010 Posts: 303 Rep Power: 17 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. __________________ Best regards, Santhosh. Last edited by saisanthoshm88; February 11, 2011 at 11:47.

 April 26, 2011, 13:05 #10 New Member   Sergio Croquer Join Date: Jan 2011 Posts: 15 Rep Power: 15 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.

 September 17, 2015, 13:44 #11 New Member   Hari Subramaniam Bhaskaran Join Date: Sep 2015 Posts: 7 Rep Power: 10 I am running a transient simulation with transient rotor stator interface. The overlap area is supposed to change as the rotor rotates over the stator. However, I notice that the overlap fraction does not change in every time step. CFX uses the initial overlap area and allows flow to occur only through the initial overlapped area.

 September 17, 2015, 18:42 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 No, TRS calculates the GGI overlap every time step. I have used this many times to model ports which slide open. If your model only uses the initial overlapped area then something is wrong with your simulation.