I guess your simulation is 3D and you exporting DPM concentration at various 2D slices? Fluent will simply interpolate to color the contour at your surfaces.

In general, DPM concentration is a "type" of density that relates the mass of particles in cell [kg] divided by the cell volume [m^3]. Units are then [kg/m^3]. This is stored as a Eulerian Field.
Remember that we coloquially call "particles" what actually "parcels" are to the CFD code.
DPM concentration [kg/m^3] = parcels in cell [#] * Parcel mass [kg] / Cell volume [m^3]
Parcel mass [kg] = DPM flow rate [kg/s] * DPM time step / # Streams
Where # Streams depend on the type of injection , PSD distribution, parcel release method ...

For example, for surface injection and standard parcel release method only

The high DPM concentration region (red parallel lines) is due to the smaller cell size at that zone. Activating the 'scale Flow rate by Area' option can remedy this. My example is valid for constant mass in a parcel, which is not necessarily true for other cases. I hope this example illustrates the concept.

Keep in mind that other settings involving PSD, other type of injection, parcel release method, 'scale flow by area' will need other treatment. Perhaps Ansys Staff can jump in to provide more general expression