You can fake this pretty effectively in Altium Designer.
Altium has what they term "Recyclable Schematics" - Schematic layouts that you can paste into larger schematics and treat as components.
Duplicating the PCB end is a bit more work, but definitely doable (I've done it). Basically, you route the DC-DC on one board, and then simply copy-and-paste the design into whatever new board you have. This will move the component footprints, and traces, but not the nets. Then, assuming you have the corresponding schematic entity, the next time you synchronize the schematic and PCB, Altium will match the free-floating footprints to their schematic entities, and add the netlabels to the existing copper.
Alternatively, assuming you are OK with not being able to edit the DC-DC layout in situ (on the PCB), you can just paste the layout into a footprint library, and define where you want input and outputs to be.
In this case, you would edit the library file, and then propagate the changes out with the "Update from PCB libraries". You can also modify the primitives of a component once it has been placed, but changes there will not propagate back to other places you have the component.
Third, Altium can embed one board into another - I use it for panelizing things, but I think you could probably also use it for embedding one functional section into another. It wouldn't tie into the schematic, though.
It's worth noting that I do the first two of these regularly at my job (usually with FTDI USB-Interface circuitry) - It's definitely a viable approach.