Running an analysis with Orca3D Marine CFD in waves is quite straightforward, although it does require a few tweaks to the standard workflow. Remember that analysis in waves does require the Premium version of Orca3D Marine CFD.
The information below is related specifically to regular waves, but the process is very similar for irregular waves. As a companion to this article, you may want to watch this video on setting up an analysis in waves.
Start the setup of the analysis in Rhino/Orca3D using the OrcaSimericsAnalysis command as you would for a standard CFD analysis. Remember that because an analysis in waves is a true dynamic analysis in which the vessel does not reach a steady state, the moments of inertia specified as input is more important here than it is for a steady state run. Another thing to consider is whether or not you need a full asymmetric run. If you are running in waves other than head or following seas, the flow field is asymmetric relative to the ship centerline and hence you must run the full ship with both sides in the CFD analysis. After entering all of the input, create the Simerics files and open SimericsMP with those files.
Once you have loaded the project into SimericsMP, there are a few tweaks we need to make to the CFD mesh before running the analysis. The first of these is a change to the meshing. For wave analyses it is important to better resolve the entire free surface, not just the portion of the free surface behind the hull. To do this select the "Built Meshes" item in the Geometric Entities panel. Then, note that the Properties panel now shows the current mesh settings for the analysis. As shown below, change the Setup Options to "Advanced Mode" which exposes a new setting when you expand the "Mesh Size" item. Change the "Extra Wave Refinements" to Yes and set the "extra_wave_zone_height" to a value about 10% larger than the anticipated wave height. So for example if you are intending to run 1 m high regular waves, set this value to 1.1 m. The rest of the mesh settings should be ok as is, but you should give consideration to a few other things.
First try to make sure you have at least 8 cells distributed vertically in the wave refinement zone. If you only have a few cells distributed vertically it is not enough to resolve the flow adequately and your simulation results may be inaccurate. One way to evaluate the meshing is to look at the free surface elevation at the side boundaries to make sure that there is not too much dispersion causing the wave height to be off. If you need to increase wave zone refinement, you can control it in the marine mesher by going to a User-Defined Mesh Size.
Second, the default domain size may be fine as is, but sometimes you can get away with a smaller domain. For example if you are running in head seas at a relatively high speed, you may be able to reduce the width of the domain in order to save cell count and hence improve simulation speed. On the other hand, if you are running in beam seas at fairly long wavelength you may need to increase the width of the domain to accurately capture the behavior. In certain cases it is difficult to know this in advance, so you may need to run a simulation first and look at the results to see if you need to increase the domain size or perhaps get away with a smaller domain size in future runs.
Next look at the Max Pitch Angle and Max Heave in the meshing inputs. The mesher considers these values and accommodates the specified amount of movement in the resulting mesh. If you anticipate larger pitch angles, you should increase the Max Pitch Angle to allow for enough movement of the mesh. Once these settings have been considered and modified as needed, click the "Build Marine Mesh" button to recreate the mesh.
Once you have re-created the CFD mesh, you can move onto setting up the wave parameters for the simulation. Select the Marine module in the Model panel and change the Setup Options in the Properties panel to Extended Mode as shown below. This exposes some new options at the bottom of the Properties panel. The first is a "Wave" option which you should change to "Regular Wave." Next specify the desired wave parameters. It is recommended to use the "Stokes 5th-Order Wave" type as this gives more realistic wave shapes, especially for shorter wave length. Note that for Wave Direction, 0 deg corresponds to head seas. Also, a default Wave Period will show up when you enter a wave height and length. This value corresponds to the linear wave period based on the linear wave dispersion relation. If you are running a simulation with a wave heading that is aft of beam seas (e.g., following seas or stern quartering seas), it is a good idea to check the boundary conditions that are applied on the outside boundaries of the domain. For head seas, the "marine_outside_front" boundary will have a Wave boundary condition since the waves are originating from there, and the "marine_outside_back" boundary has a Farfield Pressure condition since the waves are exiting the domain there. For following seas or any heading aft of beam seas, this should be reversed. To check this, select the boundary in the Geometric Entities tree and look at the "Marine" setting in the Properties panel as shown below where we've set the back boundary to Wave for a following sea.
To avoid numerical wave reflections from the domain boundaries, it is recommended that you use wave damping zones at some of the boundaries. By default, wave damping will be applied at the back of the domain, which is suitable for head seas runs. However if running in beam seas or an oblique wave angle you should enable wave damping zones at the outgoing domain boundary. The damping zone length is typically on the order of 50-100% of the vessel length.
Finally, because this is a truly dynamic simulation where it is important to have very accurate results at every time step, not just after reaching steady state, we must tweak some of the simulation settings to improve resolution. These include shortening the time step, increasing the iteration count, and several other solver tweaks. The easiest way to accomplish this is to select the Marine module in the Model panel, and in the Properties panel change the Numerical Option to one of the Transient options. Start with "Medium (Transient)" as shown above, and see how the simulation looks. If the boat is moving extremely fast or the wave response periods are very short, you may need to consider using Conservative (Transient) settings. It is also worth noting that for resistance runs, you can typically set the ramp time to zero since the model will be affected by the waves immediately anyway.
After making these adjustments go ahead and run the simulation. You will typically need to run the simulation longer than a typical steady state run in order for the model response to reach a periodic behavior. Once you have finished the run, examine the results closely to make sure the flow field and simulation behavior look reasonable. Look for things like reflections from the boundaries, or an unrealistic vessel motion to determine if additional simulation tweaks are needed.