In this example we will use a foil/bulb combination as the example geometry as shown below. Start by making sure the geometry forms a closed body in Rhino. If the geometry is an appendage, such as a fin keel on a hull, separate it from the main hull and close the opening. 

Run the OrcaSimericsAnalysis command, then skip to the bottom of the form that opens and choose "Submerged Body" as the Hull Type. Click the "Submerge" button, then fill out the rest of the form as shown below. Note that when using the Submerged Body template, there is no requirement to specify a "deck" face, so it is ok to leave them all as "hull" faces.

Next you will typically need to add one or two grid refinement zones. To enable grid refinement zones click on the Options button and click the Use Grid Refinement Zones as shown below.

Now we define two box refinement zones, one a little larger in size than the other as shown below. Note we are defining these on the port side of the model as this will be a symmetric simulation. For now set the inner and outer refinement zone cell size to 1. These will need adjustment once we can visualize the CFD grid in SimericsMP.

Next click the "Run Simulation" or "Create Files" button, and open the simulation in SimericsMP. The initial fluid domain will likely be larger than you need, so we will make a few adjustments to the grid. To adjust the CFD grid select the "Built Meshes" item in the Geometric Entities panel. The exact settings will depend on the problem being solved but in the example here we changed the domain sizes to 1 in all directions except for the "Up" direction (the domain size is non-dimensionalized as shown in the dialog). In the Up direction we would ideally set the value to 0 to place the top of the foil against the domain boundary. However, the system will not permit zero for this value so instead enter a small value such as 0.0001.  Click the Build Marine Mesh button

The resulting mesh is close to what we might want but we could use a little extra refinement. To make use of the previously defined refinement zones, click Built Meshes and in the Properties panel change the Setup Options to Advanced Mode as shown below. There you can see the two box zones with cell size set to 1. You will need to experiment a little with the sizes depending on your model, but in this example we used 0.02 and 0.01 as shown.

The final mesh is shown below (of course you should always do a grid convergence study to ensure your grid is adequately refined for your problem).

The next step before running the simulation is to enforce the double-body condition at the top boundary. Select the marine boundary, "marine_outside_top" in the Geometric Entities panel. Then in the Properties panel set the boundary condition to "Symmetry" as shown below. 

The final steps are to disable body dynamics by selecting the "Marine" module in the Model panel and setting the Dynamic Option as shown below. Also since there are no dynamics we can set the Ramp Up Time to zero as shown.

 Now the simulation is ready to run.