Missed "Part" when exporting 2D model from ICEM

nasa55 · April 9, 2014, 09:32

Hi guys
I have a 2D model (a 3D model with 3 degree thickness). It is simply like a slice of a cylinder (annulus). I generated my grids in ICEM and defined surfaces as different parts of my object. In addition, I have to define a symmetry which is a line in my case (the center-line). When I export the grid, the symmetry line is not exported to my CFX-pre. Why?

If I DON'T define the symmetry and run the model without it, Ansys suggests me to use 1:1 connectivity for periodic surfaces or make a model with 2-cell thickness. The first suggestion doesn't work and when I made my domain with 2-cell thickness, it works. But obviously, the results are not correct.

Why my symmetry line is not exported to CFX, although I defined it a separate part in ICEM.

Any help is appreciated.

brunoc · April 9, 2014, 10:16

I'm guessing you're talking about the axis. If that's so, then no, CFX won't import it because CFX doesn't use 1D regions (the axis line, in your case).

But you won't need it anyway. Just define a rotational periodicity using the low and high theta surfaces from your model and you're good to go.

nasa55 · April 9, 2014, 11:18

Quote:

Originally Posted by brunoc

I'm guessing you're talking about the axis. If that's so, then no, CFX won't import it because CFX doesn't use 1D regions (the axis line, in your case).

But you won't need it anyway. Just define a rotational periodicity using the low and high theta surfaces from your model and you're good to go.

Thanks for the reply. Yes, I mean axis. But actually I couldn't understand what do you mean by "low and high theta surfaces". I have defined "Rotational Periodicity" for both side surfaces by interface option. The connectivity type is automatic.

When I run it with one cell thickness, it crashes and says that all vertices for a fluid domain lie on boundaries and I have to use 1:1 mesh connection or domain thickness with at least two cells. There is another suggestion by the solver which says using an advanced parameter in G:G connection. What's wrong in my model?

brunoc · April 9, 2014, 12:51

By "low and high theta" I meant both surfaces on your periodic interface.

Now, before anything else, keep in mind that CFX solves its equations for the mesh nodes (which represent control volumes).

About the interfaces, a '1:1' interface means that both surfaces used in the interface have identical meshes, so no interpolation is needed between the data from each side of the interface. A 'GGI' (General Grid Interface) interface, on the other hand, means the meshes are different, and therefore an interpolation is needed.

A GGI interface behaves numerically just like any other boundary condition: it sort of imposes values on the control volume, but these values must be related to their counterpart on the other side of the interface.

But in a 1:1 interface, since the mesh is equal on both sides, what CFX does is it actually merges the control volumes from each side of the interface (that is for each node pair from the interface). So those two nodes now represent only 1 control volume, instead of two, and they behave kind of like an internal control volume. No actual value needs to be imposed.

When you have a mesh with only 1 element in its thickness and you use a GGI interface, the solver has nothing to solve for since all values lie on a boundary. But when you use a 1:1 interface, then those nodes from the interface behave like internal control volumes, so that the solver has something to solve for.

April 9, 2014, 09:32	Missed "Part" when exporting 2D model from ICEM	#1
nasa55 New Member Join Date: Jul 2011 Posts: 14 Rep Power: 14	Hi guys I have a 2D model (a 3D model with 3 degree thickness). It is simply like a slice of a cylinder (annulus). I generated my grids in ICEM and defined surfaces as different parts of my object. In addition, I have to define a symmetry which is a line in my case (the center-line). When I export the grid, the symmetry line is not exported to my CFX-pre. Why? If I DON'T define the symmetry and run the model without it, Ansys suggests me to use 1:1 connectivity for periodic surfaces or make a model with 2-cell thickness. The first suggestion doesn't work and when I made my domain with 2-cell thickness, it works. But obviously, the results are not correct. Why my symmetry line is not exported to CFX, although I defined it a separate part in ICEM. Any help is appreciated.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
manualInjection model in sprayFoam	Mentalo	OpenFOAM Running, Solving & CFD	1	April 2, 2014 09:29
about Subgrid-scale model	impecca	OpenFOAM Running, Solving & CFD	4	December 20, 2013 10:36
2D Model of Three-Bladed VAWT using ICEM CFD	mikebausas	ANSYS Meshing & Geometry	3	June 29, 2013 04:06
[ICEM] Spatial oscillation in results of a model with ICEM mesh	highhopes	ANSYS Meshing & Geometry	16	June 25, 2013 08:44
[ICEM] Exporting Cartesian coordinates from ICEM to Matlab?	user_of_cfx	ANSYS Meshing & Geometry	0	October 17, 2011 10:17

April 9, 2014, 10:16		#2
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	I'm guessing you're talking about the axis. If that's so, then no, CFX won't import it because CFX doesn't use 1D regions (the axis line, in your case). But you won't need it anyway. Just define a rotational periodicity using the low and high theta surfaces from your model and you're good to go.

April 9, 2014, 12:51		#4
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	By "low and high theta" I meant both surfaces on your periodic interface. Now, before anything else, keep in mind that CFX solves its equations for the mesh nodes (which represent control volumes). About the interfaces, a '1:1' interface means that both surfaces used in the interface have identical meshes, so no interpolation is needed between the data from each side of the interface. A 'GGI' (General Grid Interface) interface, on the other hand, means the meshes are different, and therefore an interpolation is needed. A GGI interface behaves numerically just like any other boundary condition: it sort of imposes values on the control volume, but these values must be related to their counterpart on the other side of the interface. But in a 1:1 interface, since the mesh is equal on both sides, what CFX does is it actually merges the control volumes from each side of the interface (that is for each node pair from the interface). So those two nodes now represent only 1 control volume, instead of two, and they behave kind of like an internal control volume. No actual value needs to be imposed. When you have a mesh with only 1 element in its thickness and you use a GGI interface, the solver has nothing to solve for since all values lie on a boundary. But when you use a 1:1 interface, then those nodes from the interface behave like internal control volumes, so that the solver has something to solve for.