You could apply the displacement in a command snippet in the second load step which gets each node's current location, then uses the D command to set the same displacement.
As far as using strictly workbench and Mechanical GUI-allowed abilities, link Solution cell to Model cell. You will also link an "External Data" to the downstream "Setup cell":
In the upstream model, you right click on the 3 X, Y, Z normal stresses and 3 XY, YZ, XZ shear stress to "Export Text File":
In the External Data system, one file must be marked as Master:
Insert an initial stress under the imported load folder in Mechanical. Alternatively, you could have exported strains and inserted an initial strain in Mechanical. You should not use both since this can cause overconstraint.
When Solution cell is linked to Model cell to transform deformed geometry, the initial stress import “Weighting” only accepts "direct assignment" import no matter whether “Mapping Control” is set to “Program Controlled” or “Manual.” This matches up data at node IDs, so you must only tag the node Id column and stress value column.
(When deformed data is transferred through an unlinked method, such as through STL, pmdb, cdb, you will be able to set mapping methods, instead of direct assignment, and you must specify the X,Y,Z locations column in the "External Data." You will need to use a command snippet to export the 6 stress components at the deformed locations.)
In the “Imported Initial Stress” in Mechanical you must set the 6 columns:
You are navigating away from the AIS Discovery experience
