Yes, but not all components are critical at all for positioning.
Says who? If you do this for work and someone else has to read the board, then it’s possible that they are mandatory (if the size and the component density of the board allows). Otherwise you are free to choose.
Silkscreen isn’t usually critical, and the manufacturers won’t complain if the text isn’t fully readable everywhere. I would say 0.8 mm height is still OK (IIRC I have used even 0.7 with JLCPCB and the text was decipherable). “Width:height” means actually line width (KiCad “thickness”, not character width. In KiCad you can set character width the same or a bit smaller than height. Narrower text may give you a bit more space.
Also the silk/pad clearance sounds a bit exaggerated, although it’s more important than legibility.
For silk editing for the whole board I use certain Appearance settings. For top layer,
- F.Mask
- F.Silkscreen
- Edge.Cuts
- (Objects → ) Vias
- Footprints
- Pads
- Footprint text
- Texts
are visible. Other layers than those three are not visible.
In the Selection filter only Text is active. This makes moving the reference designators very easy.
Now it’s easy to see only the relevant information for positioning the reference designators. This works for most cases because usually you don’t have to see any copper, not even pads. The mask openings cover the pads and the silk must avoid those mask openings. If the footprints have high quality silk markings, you can also see or imagine the component outlines there (roughly).
Note that for legibility you should avoid placing a silkcreen character’s line right on a via hole. That’s why I make vias visible. Sometimes I even position a character’s middle opening, like the center of 0, U, C etc., directly on a via hole so that the via doesn’t cut the character’s line.
I also use the 3D view. It gives another “opinion” to understand what the final board will look like. Because it’s more realistic, it may be easier to see problems – or non-problems – with the silk markings.
