Hi all

I have a diificulty to change a three dimensional model to two dimensional. i.e., I have a three dimensional geometric model and meshed in all three directions, when I run it for 3-D it works, but when I run for 2-D i get a message of conflicting symmetry and wall patch message. What should I do to make the flow two dimensional? The 3-d model is out of the capacity of the machine used, after few iterations.

Thank you very much

Susan

Hi Susan, firstly are you using CFX4 or CFX5 ? By the sounds of it you are using CFX4 ? Firstly have you managed to change the mesh so that it is only one cell deep in the third dimension which you are not going to be modelling ? My experience of CFX4 is limited and rusty, but I'm fairly sure that all you need to do is specify a model as being 1 cell deep and then in the comande file define it as being 2D. So if you had a model in which you were making it 2D ie x and y were modelled and Z was just 1 cell deep. Then there may be problems defining boundary conditions on the High Z and Low Z faces ?? May be someone else could confirm this ?

If you are using CFX551 then there are other issues. Previous versions of CFX5 could only undertake a pseudo 2D problem as a result of the unstructured nature of the mesher. However having just attended the Advanced mesher course, I have learnt that there is now a TRUE 2D approach that can be adopted in CFX551. Rather than a tet mesh being produced, a surface mesh is generated and then extruded to create what would be wedge like elements through out the geometry, so creating a constant thickness of elements. To achieve this you need to change the enviroment variables of your system before starting CFX551. The variable CFX5_2D_MESH needs to be set to TRUE. To return to a 3D mesh you need to remove the variable (not sure if setting this to false would work ???). Then when you are in Build you create a surface or Trimmed surface that represents the side of your geometry, create a solid by extruding this, ensuring constant cross section. Then create a periodic pair of boundary conditions on the surfaces that have constant cross section. All the other options are set as normal in Build.

Hope this helps

Bob

Thanks bob for your advise, I am using cfx4.3, what I did not understand from your comment is that I have 1.5m long in the z-direction, how can I make it a single cell? also the inlet and the outlet is in this direction do you mean not to mesh it at all on the Z direction?

thanks for your reply again

Don't get confused about the z direction it is just a standard assumption that the non flow direction is in the z direction. From your reply I assume that your flow is going in the z direction, so in the x or y direction you should in build put a mesh seed with 1 cell and change in the command file to two dimensional. Jan

Hi Jan

if I did not put any mesh seed in the x-direction, it will be one cell in that direction, but if I put even one mesh seed in any part of the x-axis, (except the corners), there will be two cells. what do you mean by puting a mesh seed?

tnx

This could be your problem, if you do not put a mesh seed then cells will be placed depending on you tolerance. Have you looked in your geometry file and checked the block size, all the block should have an extension of 1 in one of the three directions. Under mesh I think there is a menu with create mesh seed, select an curve/edge in the direction where there only should be 1 cell, and specify that.

Hi Susan, sorry for the confusion on the Z direction. As Jan said I just assumed that the Z direction was the dimension that you did not want to include. It is a strange concept to think that something is 2D and yet needs the third dimension to be included within the model, but I guess it all comes down to the fact that it is a finite volume method, and so needs 3 dimensions.

Also as Jan stated, it is often safer to include a mesh seed on the unwanted direction (value of 1 in the number of seeds) to force the code to put just the one cell in that direction. Bob