Hopp til innhold

Forsiden / Blogg / ANSYS-bloggen / ANSYS Update Geometry Based on Results  

+47 67 57 21 00

+46 21 470 35 50


ANSYS V13 New Feature: Update Geometry Based on Results

In one of our previous ANSYS Blog articles we presented a method to update geometry based on results in Workbench. That method is to combine usages of MAPDL and FE Modeler.

That method is to combine usages of MAPDL and FE Modeler. Firstly add displacements from a previous analysis and updates the geometry of the finite element model to the deformed configuration in MAPDL with command UPGEOM. Then recover the updated geometry in FE Modeler and transfer it to Mechanical. V13 we can do it directly inside Mechanical. Here we demonstrate the detailed procedure.

For the present it is a Beta option. So we have to turn on Beta options first. In Project page, go to Tools -> Options -> Appearance and check Beta Options:

Now we can start Mechanical and run the analysis as usual:

We get contour plot for Total Deformations. Here we set displacement multiplier as 1 and true displacement is plotted:

Then right click on Geometry and choose Update Geometry From Results File (BETA) for updating the whole model:

Or just update one or more selected parts:

After selecting targeted result file, a control panel opens and we can decide which load step should be imported and whether to update mesh with geometry:

The geometry is now updated as the deformed configuration:

However if we take look of mesh, it is not updated. The green dotted wireframe shows the present geometry:

And the load still remains in the original location:

So we have to clear this mesh and then re-generate the mesh to make it fit the new geometry:

And re-apply existing load to the updated location. If necessary we can add new loads and boundary conditions:

Remember: it is the geometry of the finite element model which is updated, not the real geometry. If we want to get back the original geometry, right click on Geometry and choose Refresh Geometry.

We can also update results based on Modal or Linear Buckling analyses. However since displacements from such analyses are not real and are exaggerated extremely, it is meaningless to do so.

Since this is still a Beta function, there are some limitations such as the inability to choose and import substep results and no magnification for displacement being added. Hopefully they will be fixed in the next release.