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.

Reply to
Andrew Troup
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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 ". 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)

Reply to
Andrew Troup

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