Set a velocity inlet and a pressure outlet

The commonest pair. One patch fixes the speed, the other fixes the pressure level, and the application fans each one out across every field the case solves.

Runs on the free tier.

The inlet

1. Select Boundary conditions, then the inlet patch in the tree beneath it.
2. Set Type to Velocity inlet.
3. Set Velocity, in m/s.
4. Under Turbulence, set Intensity (%) and Length scale (m). The hint gives roughly 7% of the body length, computed for this case. The read-out below converts the pair into k, ω and ε so you can sanity-check them.
5. If the energy equation is on, set Temperature.

The outlet

1. Select the outlet patch.
2. Set Type to Pressure outlet.
3. Set Gauge pressure, in Pa. The writes label shows the kinematic value that reaches 0/p, which is what OpenFOAM stores for an incompressible case.

A pressure outlet needs no velocity and no turbulence specification — the flow leaves on whatever the interior gives it.

What each type needs

Type	Velocity	Pressure	Turbulence
Velocity inlet	yes	—	yes
Pressure inlet	—	yes	yes
Pressure outlet	—	yes	—
Far field	yes (Freestream speed)	yes	yes
Outflow	—	—	—

Outflow, Symmetry, Periodic, Empty (2D) and Wedge (axisymmetric) take no parameters at all: they are purely geometric and are applied to every field.

Check it worked

• The This writes block at the bottom of each patch lists a type against every field, with no —.
• The row for each patch in the Boundary conditions list summarises it — a velocity inlet reads back as its speed, intensity and length scale.
• The Problems tab is clear. Every patch must have a condition on every field before the case can run, and it says so per patch rather than letting the solver find out.
• If the patch names do not match the generated mesh, a warning appears at the top of the list with the mesh’s own names, and Use the mesh’s patches adopts them.