well, the your friend's suggestion will work, but is a hard work. You can generate a plane with a rectangular grid. You can choose the size and the grid spacing in the options of the Plane menu. After this, you can to export the X,Y,Z and u,v,w data.

The operation can be repeated for other planes, or simply moving the plane in the normal direction according to your grid spacing.

Other is to use Tecplot. Load you result into tecplot. Generate a cubic zone with the grid spacing you want. Interpolate the data into this new zone. So, "write data" in the file menu. Choose ASCII ( binary format is default) and the variables. it's done.

I hope help you

Hi Jonathan,

It is just an idea with not yet any warranty that this will finally work, but if it could work, than it would save you a lot of time.... So it could be worthwhile to try it out.

I was thinking about making use of the ANSYS CFX built-in interpolator in the solver itself, i.e. not necessarily using CFD-Post for this purpose.

So you could generate easily (e.g. by using ICEM-CFD Hexa) a regularly spaced mesh, which is matching your intentions about the grid (spacing) on which you like to capture/export the flow information. With this mesh you create a similar CFX setup as in your original case. Once you have done this, you could start an ANSYS CFX simulation on this regularly spaced mesh and use your original flow result as a CFD simulation which you like to use as initialization of your "flow simulation" on the regular mesh (-ini option to the CFX solver or Initialization settings in the CFX Solver Manager GUI). What CFX will do? It will read in your original flow result and will try to interpolate it to the nodes of the regularly spaced mesh as initialization values for the new run. All used independent variables will be interpolated at once and as they are available from the original simulation result file, but for this it is important, that the setup of the new CFX run on the regular mesh is as close to your original run as possible (from a physics perspective), so that CFX has two simulations with matching physics definition.

If you now save a zero-iterations results/backup file in ANSYS CFX, than this RES/BAK file will contain the result of this initialization process, i.e. the result of the CFX interpolator from the original flow simulation (and grid) to the regularly spaced mesh, without any additional iteration operations on this interpolation result. The simulation on the regular grid can be stopped after 1 iteration/timestep, since the intended work is already done by the CFX interpolator at simulation startup. The resulting zero-iteration RES/BAK file than could be examined in CFX-Post or even exported in CSV format.

Could that potentially fit your needs? Would be interested to hear, whether that will work for you.

Best regards,

Thomas Frank.

Have you tried using a point cloud?

Thank you everyone who responded to help me. I've been trying to make use of your advice without asking for more help too quickly.

I like the idea of trying to use TecPlot, but I have not been able to figure out how to load my solution file into it. I think I need to export my data (and I found the "Export" command, and practiced using it with planes), but I don't know how to export the entire CFX solution so that I can load it into TecPlot. How do I get my data loaded? Was there a file somewhere I could copy out of my ANSYS files?

I'm still working on the rest; it seems like a point cloud would let me go beyond the normal limits of the plane sampling. I wasn't able to set up a point cloud of regularly spaced points for any of the volumes I had set up; it only wanted to take points at random for volumes. I could set up something regularly spaced for planes, though.

Jonathan,

Tecplot 360 is able to read the CFX *.res files - including transient cases there are some years. But if you have a old version of Tecplot ( not 360 version), you can use the Export option in the SOLVER. Choose the CGNS format. It is a general purpose CFD format . There are some options available that I do not remember now, but it is easy to understand the export levels available. It is very easy.

I have come across a somewhat similar issue earlier. If you are using CFD-Post you can try implementing the crisscrossed lines solution with a script using CCL language.

Ref: https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/cfd_post/i1333522.html

I have used it before but for really simple issues such as changing the point location for multiple points and names of points.

My two cents on the issue.