elements, nodes and faces
Hello everbody, I have a question concerning the terms "elements", "nodes" and "faces". I am generating meshes with ICEMCFD which shows me a certain number of elements at the end. When converting the mesh into CFX and starting the run, CFX will show me a slightly lower number of elements in the .outfile. I assume that this number is lower because the surface elements that were counted by ICEM are not counted by CFX, right?
In addition I also get values for "nodes" and "faces" that are far lower than my element amount. That makes no sense to me. Can anyone explain to me what these "nodes" and "faces" are supposed to be? My mesh stats in the .outfile are: Total Number of Nodes = 430941 Total Number of Elements = 2234526 Total Number of Tetrahedrons = 2150826 Total Number of Prisms = 83700 Total Number of Faces = 109804 Thanks Andy 
Re: elements, nodes and faces
Number of elements = number of tets + number of prisms in your .out file.
1 tet element has 4 nodes. When you have a number of tet elements in a mesh, each will share a large number of nodes. So typically in a tet mesh, your element count will be roughly 5 times larger than your number of nodes. In a hex mesh, it is closer to 1 node for each element. Faces in the .out file refers to boundary faces. 
Re: elements, nodes and faces
Thanks, I think I can imagine that and it sounds reasonable. However this raises another question for me. CFX uses a vertexcentered approach, right? That means when generating the mesh with ICEM CFX will build a new volume around each node of the ICEM mesh. When ICEM is showing me that it has generated let's say 2Mio elements this mesh will have about 400 000 nodes (following your argumentation). Summing up these two arguments (less nodes than elements and vertexcentered method) it follows that CFX will only create 400 000 elements, one around each vertex?! However the mesh stats in ICEM and CFX are showing that in both cases the number of elements is equal. How can that be? Even when considering possible effects at the boundaries (half element at the wall, etc.) this gap cannot be explained, I think.
Thank you for your efforts, Andy 
Re: elements, nodes and faces
CFX is a nodal based solver, but the statistics shown in the .out file are for the elements and nodes in the physical tet/hex/prism mesh, not the polyhedral mesh created by CFX.
The number of polyhedral elements built around the nodes would be equal to the number of nodes. 
Re: elements, nodes and faces
Hi Andy,
You are getting elements and control volumes confused. The number of elements is what is reported. CFX constructs control volumes around the nodes from element sectors, thus the number of control volumes is equal to the number of nodes, not elements. In a cell centered code, such as Fluent or StarCD, the elements are the same as the control volumes, so these are often used interchangably. This is obviously not the case with CFX. Robin 
Re: elements, nodes and faces
Thank you, that explains a lot!
Regards, Andy 
Re: elements, nodes and faces  another thought
Hello again, overnight another thought or question came to my mind concerning the elements and nodes.
You have said that CFX is using the nodes generated by ICEM as the centers of its control volumes that is in this case CFX will use about 400k CVs and ergo will store e.g. 400k pressures. Now my question is: When using ICEM to generate the mesh and afterwards a cellcentered solver instead of a nodecenered one, will there be 2Mio points in which the variables will be stored. In other words: Is ICEM that less efficient(or more accurate in terms of space resolution) when used with cellcentered solvers? Regards Andy 
Re: elements, nodes and faces  another thought
Hi Andy,
ICEM CFD has nothing to do with it; it just provides the mesh. Since CFX is element vertex centered, you will get fewer control volumes in an unstructured mesh than you would in a cell centered method. So yes, there will be fewer points where the the primitive variables (Pressure, Velocity uvw, Temperature, etc.) are stored. At first you might assume this means you have less accuracy, but you also have to consider how these values are obtained. CFX will have many more integration points and it uses linear elements (assumes a linear variation of the variable across the element), which increases the accuracy at each node. While the variables are stored at the nodes, the equations you are solving for are assembled for the flows through the faces at the integration points. In any Finite Volume method, the equations are essentially an application of Gauss' theorem, which converts a volume integral into a surface integral. When these are discretized, the integration is done over discrete faces. The accuracy of the integral equations will increase with the number of faces (i.e. the number of integration points) and the assumptions on how the values vary over the faces (constant or linear variation). In a tet mesh, a cell centered control volume has only 4 integration points whereas CFX has ~60 (it varies depending on the connectivity) so the integration accuracy that leads to the nodal value is much higher in CFX. It is for this reason that many cell centered codes are turning to "arbitrary polyhedral" control volumes; something CFX has been doing since it's inception (even TASCflow did this, although the initial mesh had to be structured). It has been demonstrated with other codes that a coarser polyhedral mesh can give a more accurate solution than a finer tetrahedral mesh; the same applies here. Another way to look at it is the number of integration points per element. Vertex centered (CFX) vs. cell centered (CC) value are: Element Type, Vertex Centered (CFX), Cell Centered tet, 6, 4 pyramid, 8, 5 prism, 9, 5 hex, 12, 6 Sorry for the long winded answer, but it is kindof a loaded question. Hope this helps. Regards, Robin 
hii
I want to know how to Calculate elements for model in FEA,and i need to
know how this elements is sufficient for that particular model...... 
If you are asking how to determine how many elements to use in a CFD analysis, try this: http://journaltool.asme.org/Template...umAccuracy.pdf
If you are asking about a FEA analysis (ie stress/strain modelling) then you are asking the wrong forum. Try a FEA forum. 
Thnxs ghorrocks
Thnxs for ur guide,its useful for me.....

All times are GMT 4. The time now is 07:16. 