TIP: An alternative to "Hide Solid Body / Bodies": Paint it WHITE!

LONG TIP WARNING: make a coffee and get comfortable!

When modelling parts where features are highly interdependent, and subject
to strenuous development, it's generally recognised that sketch relations
should be established to previous sketch entities, axes or construction
planes, rather than to solid edges, vertices etc. This greatly reduces
future time wasted repairing dangling relations, and (more crucially) the
likelihood of unnoticed errors creeping in, when changes cause those solid
features to move about or disappear. It also makes unwanted child
dependencies much less frequent and troublesome.

Trouble is: with a model rich with visible edges, you must keep temporarily
hiding the solid body, so you can see previous sketches clearly, to create
these relations safely. This can be painful in SldWks *when rolled back*,
because the Hide/Show state of solid body/bodies is captured separately at
each rollback waypoint. Unless you are disciplined enough to "Show" again
immediately you finish with each "Hide", you quickly end up with a model
whose solid bodies randomly appear and disappear, flickering like the
eyelids of a spastic parrot, whenever you roll up and down the tree.
Furthermore, this functionality seems to experience frequent bugs (such as
the one reported recently by Paul S). Finally, it is laborious scrolling to
the solid bodies folder and RMBing on each body each time you want to change
their visibility.

Luckily, there's a sneaky way to instantly and reliably toggle visibility On
and Off for ALL solid features and bodies in a part, which can be set up in
a part template, and gets around these difficulties.

First ensure "Tools/Options/Document Properties/Colors/Apply same color to
wireframe, HLR and shaded" is turned on.

In the same "Colors" dialog, now set the "Wireframe/HLR/shaded" colour to
WHITE, then (under FM "Lighting") turn all the lights down low.

The part will revert to a normal grey appearance (or coloured, if you use
coloured lighting) in "Shaded" view.

As long as you stay with "Shaded" view, the edges will show in your
specified "HLR edges in shaded mode" colour, per System Options. This colour
overrides the White while "Shaded".

(NB: if you use a background screen colour other than white, set that same
colour for "Wireframe/ HLR/shaded". This method does not work as well if you
use a gradient background, but still well enough)

If you now flick to "Hidden Lines Removed" (ie the wireframe "visible lines
only" icon in the View toolbar), the solid body/bodies will (hey, presto!)
disappear, and any sketches which are turned on will be revealed with all
the delicacy of trombones in a string quartet.

The reason is that even a white face will (in SldWks) show as grey in low
light, but a white wireframe edge will always show as white, hence disappear
against a white background.

The neat thing about this method is that the solids will obligingly REMAIN
disappeared at ALL stages of rollback, until such time as you revert to
"Shaded". Furthermore, mouse activity to achieve the Hide/Show is
simplified, and the toggle can easily have hot keys assigned to it.

Be warned: for REALLY complex models, my workaround does not disable the
inadvertent creation of relations to solid edges and vertices. This is not
normally a problem, because the edges temporarily reappear (in a contrasting
colour) if the cursor hovers over them, so you would know you were selecting
a non-sketch entity, but if the model is riddled with edges, it can be
problematic. In this case, set the Selection Filter to "Filter Sketch
Segments" and/or "Filter Sketch Points"

PS: When you finish the model, be sure to hide all sketches again before
creating a drawing from it. Trust me!

Naturally, you will also most likely wish to assign a non-white colour to
the part before adding it to an assembly.

 

Take my advice, I'm not using it!

I just got bitten since posting the above, for having created a relation to
an edge instead of to corresponding sketch geometry further up the tree.
Now that relation has gone dangling, and it's an order of magnitude more
difficult to troubleshoot, for lots of reasons, but one very basic one is
that when you use "Display/Delete Relations" to audit the edge, it
identifies it only as "Edge of <partname>". Because that is dangling, it
doesn't highlight in the correct place when I click on it.
If it was a sketch entity, the "Entity" box would identify which entity in
which sketch was dangling.

Of course, it takes more time to do it the "right" way

(in the short term)