Learning Forum

[floatingstones]

Hello all,nI am trying to apply pressures contained in an external data file (.csv) on a geometry in Ansys Mechanical 2021 R1. Setup in Workbench below:nWhen trying to import this loading, two errors appear:nAn error occured while importing the data. Additional information may be available in the Load Transfer Summary.nNo data was imported on the target mesh. Please ensure that the number of nodes mapped count is greater than zero in the Imported Data Transfer Summary.nnThe Imported Load Transfer Summary states the following - and, indeed, no nodes were mapped.nUsing multiple cores: [Yes]nNumber of cores requested: 8nMaximum source mesh bounding box length: 40.5232 (m)nMaximum range used in sorting closest nodes: 40.5232 (m)nNumber of source nodes: 1110nNumber of target nodes: 1459nNumber of nodes mapped : 0nNumber of nodes not mapped : 1459nNumber of nodes outside : 0nPercent nodes mapped: 0%nWeight calculation time: 6.4e-002 (s)nConverting source element nodal data. Using 'average shared nodes' methodnTime taken to convert source element nodal data using 'average shared nodes' method: 1.e-003 (s)nNumber of variables to interpolate: 1.nInterpolation time: 7.e-003 (s) nnThe pressures come from a Hydrodynamic Time Response in Aqwa, and are related to the elements in the meshed hydrodynamic model. A part of the .csv file is seen below:nnI've seen that, in earlier Ansys versions (I'm using 2021 R1), Aqwa's .csv pressure file didn't refer to Element ID and its centroid coordinates. Instead, it had a pressure for each node and its corresponding XYZ coordinates. Maybe this could be problem, that Ansys Mechanical is not recognizing nodes because the .csv file refers to elements? nAny help would be appreciated. nn

[Aniket]

What happens when you do not use element IDs (i.e. mark element ID column as Not Used) and just use the centroids?
-Aniket
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum

[floatingstones]

Hey Array,
It shows a similar error in the Import Load Transfer Summary. Difference is in the final lines:
Percent nodes mapped: 0%
Weight calculation time: 8.9e-002 (s)
Number of variables to interpolate: 1.
Interpolation time: 0. (s)

[Aniket]

Under Graphics controls of Imported pressure, you have the display source point option, kindly turn it on, and see that if it overlaps with the geometry?
-Aniket
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum

[floatingstones]

Aniket right on spot. When I display the source points, I realize they do not overlap with my geometry:

I'd guess that the source points relate to the position of the geometry at the timestep when pressure .csv file was obtained...

[Aniket]

You can either shift the source points, or you can transform the geometry so that they overlap each other using transform feature in Mechanical https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_part_transform.html.
-Aniket
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum

[floatingstones]

Array Is the Transform feature on DesignModeler (/Space Claim) or in Mechanical?
I think it would be easier to directly change the centroid's coordinates/normal vectors of the .csv file. I would change them for the original (equilibrium) coordinates of the elements of my hydrodynamic mesh. Do you know if it's possible to obtain elements' XYZ coordinates from AQWA?

[Aniket]

Transform feature is available in all three.
Mechanical: https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_part_transform.html
But the Mechanical one would be most useful to you in my opinion. Not sure about AQWA query, but as you have element IDs, wouldn't it be possible to export the same data at earlier time point and later combine with results from later time point?

-Aniket
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum

[floatingstones]

Thank you for the help Array your tip worked! I exported a pressure plot at t = 0, when structural and hydro meshes still overlapped, and copied the equilibrium coordinates. Then pasting them over the 'shifted' coordinates solved the problem.

[Mike Pettit]

Hi Array,
Just out of interest - did you try linking the Hydrodynamic Response system directly to the Static Structural system? This should be possible in Release 2021 R1, and does all of the import/transforms for you. Unless you had a problem with it, in which case please let me know!
Cheers, Mike

[floatingstones]

Hey MikePettit, your suggestion worked perfectly. Much better ;)

[Mike Pettit]

floatingstones great, happy to help!