[papis]

Hi to all

I am using ICEM CFD as a mesher as well as "mesh parser"(importing grids from various formats and then exporting the grid in the format that I want).What I have noticed is that the output (in my case either fluent v6 or CFX) is always single precision.
(By output I mean the node coordinates since connectivity etc is only integers.)

Even if I import a plot3d mesh (in double precision) or a fluent.msh( also double precision from other software) when i export the mesh the output is in single precision.

an example of the first node of the grid

double precision msh file :
-1.9021172349563999e+00 1.0981879031046000e+00 1.9021172349563999e+00
output of icem msh file:
-1.902117235 1.098187903 1.90211723

This causes me problems because in my mesh there are elements which by the single precision transformation produce negative volumes.

I also checked the CFX solver output.It has an option to decide whether single or double precision is needed.I checked double precision but the output was still single.
(I am using ascii files)

I am sure there is a solution to this problem but I can't fint it so any help would be greatly appreciated.

Thanks

[mjgraf]

this is a good one for Ansys support.
I would be curious for their reply. I never needed to mesh something that fine.

[papis]

Yes indeed the resolution seems to be very fine.However we must have in mind that at high reynolds numbers (for example~12-20 million) the boundary layer should be 1d-06 or less which is already close to the single precision margin so smaller values than this could be critical.Also when the aspect ratio of the cells varies very much single precision isn't enough.

Let's say we have a Wind turbine blade which runs at a high reynolds number.

Then we will need a very small boundary layer ~1d-06 but at the farfield we will have cells with size edge 100 or more.In case we had 6 digits in the output(less than single precision) the small cells would be alright but 100,123456 would transform to 100,1234 which could cause problems later on. Imagine if you start with a boundary layer cell and end in a cell of size 100000(ok this is not realistic!!) then all the cell sizes after this margin could cause problems since 100000,1 or 100000,9 would be the same and thus the cells formed from these nodes would have a random orientation.

[mjgraf]

looked at some .cfx5 mesh files created in icem.

it seems dynamic

grab from file

-0.760037899 0.6098202467 -2.788345814
-0.1590990275 0.1590990275 -2.605000019
0.5338656306 0.5338656306 -3.730600119
4.144724432e-31 -1.49849999 -3.730600119
5.493000031 -1.49849999 -3.190599918
-0.7781959772 1.905998964e-16 -8.06760025
-2.003626526e-16 -1.409999967 -8.06760025
1.524000049 1.49849999 -3.730600119
2.752790639e-16 1.49849999 -3.730600119
5.505399696e-16 1.49849999 -6.543600082
10.99300003 1.49849999 -6.543600082
5.493000031 1.49849999 -6.543600082

still say ask ICEM via ansys support.

[papis]

I asked ansys support and here is the answer:

Technical Details: Activity Description: a defect Activity Detail: It looks as though the choice between double or single precision does not work when the output file is written in ASCII. When it is written in binary then the double-precision file is larger than that obtained with single precision. I will submit a defect about this but it looks as though one workaround for you would be to use the binary format. There are some other options too: ANSYS Fluent can import Plot3d meshes directly. So if you are using Fluent there should be no need to go via ICEM. CFX-Pre can import meshes as Fluent .cas or .msh files. So you could use Fluent to do the conversion. If from Plot3d, you can write to CGNS (.cgns,.cgn) or PATRAN neutral (.out,.neu) formats, then you could import that file into CFX-Pre. Thanks for pointing out the problem. Regards

Hmm....Really disapointed about that.It seems that there isn't an option four double precision in ascii format....There isn't even a option to control the decimal places of fluent output....

Activity Description: Can't seen an option for dp for Fluent output Activity Detail: There doesn't seem to be an option to choose whether the export to Fluent V6 is double or single precision, or rather to control the number of decimal places. I don't know to how many decimal places Fluent meshes are imported into ICEM. It is possible to display the coordinates of vertices and using Settings > Display > Float Display Precision you can set the number of decimal places. So that might help you to judge. However, if you are planning then to export to the CFX binary format, I am not sure how you will be able to obtain the information necessary to import the mesh for use with your own solver. Regards

If anyone has a guide of how the CFX mesh file is constructed it would be very helpful.It seems we must drop msh file support for our in house solver.