Simcenter 3D Solutions Simcenter 3D FEM with a Simcenter FloEFD pressure, or temperature, field.

Summary

There are basically two ways to export the resulting temperature and pressure fields in Simcenter FloEFD. Depending on the method used the import of the loads into Simcenter 3D is different as well. a) Mapping the resulting fields on a NASTRAN mesh by adding or replacing the loads. The NASTRAN mesh must be defined and exported in Simcenter 3D and reimported after the mapping is done. b) Exporting a pressure or temperature field as Simcenter Field File. These fields are exported in a csv format and are added as new load – temperature or pressure field – to a specific surface of the parts in Simcenter 3D.

Details

While Simcenter 3D and Simcenter FloEFD can both be used for CFD and FEM analyses, there is a difference regarding the focus of the feature set.
The focus of Simcenter FloEFD is on the CFD analysis, whereas Simcenter 3D has the clearly superior state-of-the-art FEA solver for more complex mechanical analysis.
For this reason, it is beneficial to make use of both software packages in a co-simulation. Especially if both are using the Simcenter NX CAD kernel.

How is it done?
There are basically two ways to export the resulting temperature and pressure fields in Simcenter FloEFD. Depending on the method used the import of the loads into Simcenter 3D is different as well.

1. Mapping the resulting fields on a NASTRAN mesh by adding or replacing the loads. The NASTRAN mesh must be defined and exported in Simcenter 3D and reimported after the mapping is done.
2. Exporting a pressure or temperature field as Simcenter Field File. These fields are exported in a csv format and are added as new load – temperature or pressure field – to a specific surface of the parts in Simcenter 3D.

Mapping to a NASTRAN mesh
Mapping the fields to a NASTRAN mesh requires an existing simulation in Simcenter 3D. Nevertheless, in terms of efficiency, it is better to set up the Simcenter FloEFD simulation first and then use the computation time of the CFD project to define the FEA simulation.
With this in mind, the workflow looks like this:

1. Fully define the project in Simcenter FloEFD and run it.
2. Define the simulation in Simcenter 3D.
   1. Mesh, materials, constraints and from the CFD solution independent loads.
3. Export the NASTRAN à File/export/simulation
   1. Change the units to (N)(m)(kg).
   2. Leave everything else as default.
   3. File format name.dat.

           

1. Back in Simcenter FloEFD load the results and insert “Export Results”: 
   1. Export to NASTRAN
   2. Input file:
      1. NASTRAN Mesh
      2. Point to the exported file: name.dat
   3. Loads:
      1. Structural (and/or)
         1. Pressure (relative)
         2. Temperature
      2. Fluid to solid.
   4. Output file:
      1. Add loads
      2. (m), (Pa), (°C)
      3. Name.nas
   5. Click export.
   6. Leave with okay.

1. Back in Simcenter 3D import the name.nas file:
   1. File/import/simulation

1. Select Solver: Simcenter NASTRAN
2. Import Simulation:
   1. Mode: general
   2. Change the unit system to (m),(Pa),(kg)
   3. Leave everything else on default.
   4. Point to the file: name.nas
   5. Click okay.
   6. A new simulation will be created.
      1. Change the name or place and
      2. Click okay.
3. Check the new simulation and run it.

          

Exporting to a Simcenter Field File
Exporting a pressure or temperature field as Simcenter Field File. These fields are exported in a csv format and are added as new load – temperature or pressure field – to a specific surface of the parts in Simcenter 3D.
With this method, the export of the loads is independent of an existing Simcenter 3D mesh.

1. Fully define the project in Simcenter FloEFD and run it.
2. With loaded results insert “Export Results”: 
   1. Export to “Simcenter FLD”:
      1. Use entire geometry, or parts of it.
         1. Loads: Relative pressure
         2. Output file: name.fld
         3. Click export.
         4. Click okay.

1. Open the location of name.fld and change the type to name.csv
2. Open the file name.csv with Excel and
   1. Convert the length from [m] to [mm] x1E3
   2. Convert the pressure [Pa] to [MPa] x1E-6
   3. Copy the table without the headers.
   4. Open Simcenter 3D
   5. Open the simulation file
   6. Add loads:      
      1. Eg. Pressure: Load Container/new load/pressure      
      2. Normal pressure on 2D or 3D element faces.
      3. Name: Optionally change the name.
      4. Model Objects: Select the object(s).      
      5. Magnitude: MPa=new field/table     
      6. Most used: Cartesian à next
      7. Leave the default. à next
      8. Edit table in spread sheet (Excel icon top-middle).     
      9. Paste the data and close the spread sheet without saving.
      10. In the upcoming window hit okay.
      11. Hit okay to finish the definition of the load.
      12. The import is done, continue as usual in Simcenter 3D.

                              

Alternatively:

1. Import the field file: File/Import//Fields
   1. Toggle to (icon top left corner): import user field file
   2. Load the field file.
   3. Leave the default settings and click okay.
   4. Edit the new entry
      1. Adjust the unit settings with the right mouse
         1. change units
         2. or convert units.
   5. Add new load/pressure/select existing field.
   6. Click okay to accept the field.
   7. Click okay to accept the new load.