Thermo-elastic structural simulations is one of my favorite topics! You don't need the plate or the clamps in the model.
I expect the barrel and lenses are all axisymmetric bodies, therefore an axisymmetric model is ideal for your simulation. In CAD, orient the optical axis along the global Y axis, and put the flat mounting surface of the barrel on the XZ plane. Use the XY plane to cut the solids and delete the pieces in +Z. Use the YZ plane to cut the solids and delete the pieces in -X. Now you have a 1/4 model with a set of faces in the XY plane. Copy those faces and paste them in as surfaces. This is easily done in SpaceClaim. Delete the solids. Now you have surface bodies in the XY plane on the +X side of the Y axis. If you were to revolve those surfaces, you would get back the original solids.
Start a new Static Structural model, do not reuse your current model, but you can link the Engineering Data cell from your first model. In Workbench, right click on the Geometry cell and in the Properties window on the right, change the Analysis Type to 2D and import the file with the 2D surfaces. Now open the Model and the geometry will import. In Mechanical, click on the Geometry branch of the Outline. There is a place in the Details window to set the type of 2D analysis. Select Axisymmetric. Now you are ready to define the rest of the model.
Pick the mounting edge of the barrel, and set a displacement of Y=0. That grounds the barrel, but leaves it free to expand radially along the X axis. Define frictional contact at the interface of the barrel and the first optical surface. Define another frictional contact of the first spacer and the second optical surface. Continue creating contacts: the first spacer and the third optical surface and so on. I expect the last spacer screws into the barrel to clamp the stack of lenses. Use bonded contact between the last spacer and the barrel.
Now you have an assembly that can have a temperature load applied and look in detail at the deformation of each optical surface relative to the bottom surface of the barrel. You must of course have the CTE defined for each material and the reference temperature of each material set to 25C and the Environment temperature of the model set to 25C so that there is zero strain at 25C and then you will see the effect when you apply a Thermal load of 90C.