As you've noticed, there is no polygon tool in the sketcher ATM. There is one in the Draft module, but the Draft module doesn't work like the sketcher. You cannot link to external geometry (edges).
Still a Draft polygon can be drawn pretty quickly, and it's compatible with Part Design features. If you don't mind having to place it through its coordinates, and to edit them manually again whenever you make other changes in your model, it's the fastest way.
Click on the face you want to draw the polygon on, switch to the Draft workbench then start the polygon tool. The working plane will be automatically set to the face, which links/maps the polygon to the face. Draw the polygon, then change its coordinates, go back to Part Design, and click on the pocket tool.
To facilitate the placement of the hexagon, you could first create a sketch on the face of your part with some guiding geometry, like lines or a rectangle. You can add reference geometry (by copying edges) and add dimension constraints to it. But your guiding geometry should not be construction line or they will be hidden once you quit the sketch edit mode.
Then you start the polygon tool, and snap on an end point or midpoint of your sketch guide geometry. The drawback to this is if you change the size of your part, the sketch will update but the polygon won't, it will keep its coordinates.
Or if you want to keep working in the Part Design workbench, you will have to draw the polygon the "hard way". The trick with constraining a polygon is to inscribe it in a construction circle (see attached example). To place the polygon in reference to your face you add distance constraints to the circle's center point.
Did you know that you can copy-paste sketches between FreeCAD documents? I suggest you draw and constrain your hexagon in an empty document and save it so you can reuse it as a template. Copy the sketch, and paste it in the document where your part resides. Next you need to map the sketch to a face, or you will get an error that you need a sketch supported by a solid.
Mapping an unlinked sketch to a part's face
This is useful for sketches pasted from other documents but also for sketches that have somehow lost their link to their support face, or if you want to change the support face for your sketch. In those last two cases, it is recommended to edit them first to delete reference (magenta) geometry, as once the sketch is remapped to a new face, the existing reference geometry will not be recognized and this will mess up the sketch. To the point that if you attempt to edit it, it may occasionally crash FreeCAD.
- Select the face of your part you want the sketch to be mapped to
- Click on the "Map sketch to face" icon in the Sketcher toolbar
- A small dialog pops up. In the drop down list, select the sketch to be mapped and click OK.
- The sketch opens in Edit mode. Add required constraints to fully constrain the sketch.