ICEM export mesh
I am currently using ICEM 12.1 in order to mesh a geographic bay in France. I have finished the mesh (using a blocking strategy with 19 blocks) and I would like to export it.
But when I export it, the nodes seems to be randomly written in my output file..
Is there a solution (an export format) to export block by block or to have an organized list of nodes ?
Thank you in advance
u are using which solver
i use Fluent and cfx so i will explane procedure for those
once you created blocking structure,press premesh i will show u how the final mesh
premesh is not actual mesh u have to load mesh from blocking
for that go to file-->mesh-->load from blocking
then icem will load actual mesh
for taking output go to O/P tab
1. select solver eg. Fluent_V6
2.give Boundary Conditions in next tab
3.then go to last tab
click it will ask whether to save project or not it is always better to save
then after saving it will prompt to open saved *.uns file select it and follow the pemaining steps
They are quite easy.
Thanks for your answer.
I am not using a traditional solver (I use a personal code).
I have made what you said and I reach a *.msh with a list of nodes coordinates (25 000 in my case).
But what is the order of these nodes ? It is not cut block by block ?
(Maybe, it is because I initialized with 1 block that I split after ?)
dhananjay1287 is using an unstructured solver, so he is happy with the unstructured mesh (no particular order with nodes just in xyz space), but it sounds like Youen has a structured solver and needs the mesh in structured multi-block format (ijk organized nodes)...
In the Blocking branch of the tree, right click on Premesh. You will see an option to "Convert to Multiblock mesh".
Then you can select your output format (assuming it is something like Plot3D, CGNS or some other format that supports MultiBlock) and output the multiblock mesh. What format are you using or do you still need to write a converter?
One side note, you can merge your output blocks and reduce the number of blocks if that helps in your code. I would be happy to help with that step also, but would need to see at least a screen shot (if not the actual files) in order to direct you.
Thank you PSYMN for this answer.
In fact, I need a mesh in a structured format (a 2D matrix xy).
Please find attached screenshots of my mesh, my blocking and this blocking when I unselect "Whole blocks" in the tree.
I have to write a converter to get my matrix of nodes coordinates (with empty areas) but I do not understand the output order of the nodes.
I have done a conversion to multiblock mesh and get a new output file. It seems to be better.. But can you explain me the order of this file ?
How to step by step
I would sugest you to do the next steps.
1.Save your project
2.At the File/Blocking/ press Save Multiblock mesh
3.At the Output Menu first select an output solver which supports multiblock (Multiblock-info or Plot3D etc) then press the "write input" button and save your file.
You can view your file with a simple text editor and check the format.
If you want to change the way the points are numbered you can do that by using the edit block menu
Hope this helps
I have understood !
Now I have just to connect my blocks together in a big matrix.
Yes, once you decide on a format (such as Plot3D or CGNS), you will find a lot of info on the web about the formats, etc.
You could also find ICEM CFD on the ANSYS website http://www.ansys.com/products/icemcfd.asp
Look at the output interfaces section and look under Technotes for our native file format information.
You could also search the built in help for "output blocks". Turning this on will let you merge your blocks to even fewer without losing the control (it only merges the output domains, but lets you keep your block splits).
But it looks good.
how to export mesh genereted by ICEM CFD in to CGNS format
i have created mesh for 2d & 3d objects in icem cfd . the problem is that my solver accepts grids only in cgns format so somehow i want to save them as file_name.cgns as my finally usable file.
The ICEM CFD creates so many files for each project, but i need only one file having information of geometry, blocks & mesh etc in cgns format.
please help me me short out this problem
Output to solver
You should probably try a few tutorials to get you past the basic steps (training would be a good idea too if you have access, but I know not everyone does).
Those files are native ICEM CFD files. The *.tin file is the geometry and mesh parameters, the *.uns file is an unstructured mesh file in native ICEM CFD format. The *.Blk is a blocking file. The *.fbc is a "family boundary conditions" file. The *.atr is an "attributes" file (needed by some solvers). The *.prj file is a "project" file that ties the rest of these together. None of these files are intended for the solver.
To output to solver, go to the "output" tab... Select your solver (set it to CGNS in your case). Then you can setup your boundary conditions (second icon), and finally, output to solver (4th Icon). Even if you don't want to set up bocos in ICEM (some users prefer to do that in the solver), you should still click on the bocos button and apply the empty bocos file.
Before outputting to the solver, it will ask you to save your project. Keep in mind that the output converters run off the saved files, so it is usually a good idea to save your project ;) but if you just saved after applying your bocos, you don't need to do it again.
During the output process, solver specific options will be available.
This "output" process will produce your *.cgns file. (or your fluent.msh file or what ever you asked for).
i suppose it will help me a lot.
thnx a ton Mr.Simon Pereira
I have to generate multi-block structured grids...i did the same as u told..
But Now i m facing a new prblm..whenever i use write input tab(under output) & then select doamin (as in my case there are 4 domains, due to splitting of the block to make it as a T shape, required for the topology) and click done, my system get kind of hang & that too for unlimited time... (the cursor works everywhere except the main window)
There comes a msg in feedback window(at bottom) as..
"Running ICEM CFD/CAE CGNS Interface Vers.4.3.1
child process exited abnormally"
some of my friends told me that its very difficult to export structured multiblock grids from ICEM CFD into CGNS format..!!
is this true..??
Can this problem occur due to improper installation of package..??
my system is well enough to handle large no. of simultaneous calculation, so i suppose this problem is not due to system configuration.
i tried the same project at other terminals, everywhere the response is same.
also the bocos tab is not doing any help..the new tab that opens after clicking on BC tab seems to be inactive...
u might be wondering for these many problems...but i will be greatful if u can help me to rectify them...
thnx in adance........................
if other members...know the solution to above problems..kindly help me..!!
Steps for 12.1
First, I see that you are using version 4.3.1, our current release is 12.1 and we are almost done with development of 13.0.
I haven't actually used 4.3.1 for a very long time. In addition to being old, we had a significant GUI change for the next release.
Perhaps your machine ran out of memory... How many elements were in those 4 blocks? If you coarsen it, will it export?
Here are the steps for output to CGNS with the new GUI... In this case, I am using 12.1, the current release.
1) block your model and run your checks, etc. to make sure the premesh is good.
2) right click on premesh (in the model tree) and select "Convert to Multiblock Mesh". This will convert to and load the 4 multiblock domains.
3) go to "Output (tab) => Select solver", set the "Output solver" to CGNS. Don't worry about setting the common structural solver unless you are doing FSI stuff.
4) Go to "Output (tab) => Boundary Conditions", set up your bocos. In this case, I set them up for inlet, outlet and walls (GEOM), but you could also just let the software create defaults.
5) Go to "Output (tab) => Write input". It will ask you to save the project, make sure you do.
6) Then it will ask you to select the mesh file. The 4 domains are in this folder (along with all the hundreds of other tetin, project, fbc, etc. that were ever created in this junk folder), but a selection filter reduces the display to just structured or unstructured mesh files that would be valid with CGNS. Since I just saved the project, it already knows the name of the muliblock file and selects it for me. I didn't even need to click on it, but I could select a different file if I wanted.
7) Next it asks me if I want to choose all domains or select domains. I just picked "all".
8) Then it wants me to select my "input type" parameters... It defaults to Structured based on the file I selected. You may want a different version of CGNS or perhaps HDF... You can also have it auto generate default bocos for each face.
9) I just hit done and it output the file. No problems...
Yourtechncs helpedme a lot...i could export mesh from icem to cgns format successfully.....
hope u will help me again...
Thanks a ton...
I am exporting mesh created for 3-D pipe from ICEM CFD in to Multiblock structured CGNS format. The problem is, there seems to be some connectivity problem between different blocks. The contour plots of the solution obtained from this mesh file indicates that information between different zones is not passing properly at the zone boundary.
Is there any feature IN ICEM CFD, so that i can have a better connectivity between different blocks, or will I have to follow certain procedure in exporting so that, this problem doesn't exist.
Connectivity is inherited
If the blocks are connected in ICEM CFD Hexa, they should be connected in the output...
I have imported a CGNS file into ICEM CFD 12.0 and I would like to just save a .msh file. I have done 'save mesh file as'. Is the .multiblock format the same as what used to be the .msh format ? ie, could I read that into Fluent as if I was using a .msh file ? This is actually for another program that can only read files in the .msh format....
Any thoughts ?
Thank you !!
|All times are GMT -4. The time now is 22:53.|