silhouette edge for revolved parts

lonnie_1

Is there any work flow to address working with cylindrical parts and need to constrain to the silhouette edge?
I turned on the origional sketch to but I could not snap to it when creating geometry.  I could constrain to the sketch after I created the geometry.  Does this sound like the proper work flow?  or am I missing something?

traveler_hauptman

Currently Onshape does not snap to background geometry (intentionally to keep the snapping unobtrusive until they can support per user settings of this sort of thing).

The workflow is to either use the 'use (project/convert)' tool on the silhouette or draw your geometry without snapping and add constraints to the underlying geometry.

For instance, for the end view of the cylinder, draw a circle and then create a 'coincident' constraint between the silhouette and your drawn circle.

traveler_hauptman

Currently Onshape does not snap to background geometry (intentionally to keep the snapping unobtrusive until they can support per user settings of this sort of thing).

The workflow is to either use the 'use (project/convert)' tool on the silhouette or draw your geometry without snapping and add constraints to the underlying geometry.

For instance, for the end view of the cylinder, draw a circle and then create a 'coincident' constraint between the silhouette and your drawn circle.

lonnie_1

thank you

andrew_troup

I wonder if "silhouette" is being used here to signify the sketch profile which will be revolved? I would suggest 'revolve profile' or similar, to avoid confusion.

In Solidworks and some other modellers, the 'silhouette' word has a different significance (and an important one):

it represents an outline (analogous to the skyline of a hill) of a solid body which does NOT necessarily result from an edge, but is the projection, in a direction normal to the sketch plane, of the maximum extent of any curved face. This does not apply only to the cylindrical case; any complex curved face has a silhouette.

And even in the case of a cylindrical revolved sketch, the resulting solid will have silhouette edges which do not coincide with the revolve profile, except in the special case of a sketch plane which lies parallel to that profile's plane.

It is not currently possible to constrain to silhouette edges (defined this way) in Onshape, nor is it possible to Use/Project them, but they will become important, and I think the terminology should be reserved.

Firstly because there is no other obvious candidate, and secondly because this is exactly what the original word meant.

lonnie_1

andrew_troup said:

I wonder if "silhouette" is being used here to signify the sketch profile which will be revolved? I would suggest 'revolve profile' or similar, to avoid confusion.

In Solidworks and some other modellers, the 'silhouette' word has a different significance (and an important one):

it represents an outline (analogous to the skyline of a hill) of a solid body which does NOT necessarily result from an edge, but is the projection, in a direction normal to the sketch plane, of the maximum extent of any curved face. This does not apply only to the cylindrical case; any complex curved face has a silhouette.

And even in the case of a cylindrical revolved sketch, the resulting solid will have silhouette edges which do not coincide with the revolve profile, except in the special case of a sketch plane which lies parallel to that profile's plane.

It is not currently possible to constrain to silhouette edges (defined this way) in Onshape, nor is it possible to Use/Project them, but they will become important, and I think the terminology should be reserved.

Firstly because there is no other obvious candidate, and secondly because this is exactly what the original word meant.

Andrew, 
nope I am not talking about the sketch profile for the revolve.  I am talking about being in a new sketch and being able to constrain to the silhouette edge of  a revolved body as I do in SW.  I am referring to the silhouette edge of the solid body.  

However I have been able to project them.  So I am a little confused by your statement about not being able to project. them.

andrew_troup

lonnie_1 said:

Andrew, 
nope I am not talking about the sketch profile for the revolve.  I am talking about being in a new sketch and being able to constrain to the silhouette edge of  a revolved body as I do in SW.  I am referring to the silhouette edge of the solid body.  

However I have been able to project them.  So I am a little confused by your statement about not being able to project. them.

Lonnie. You're quite right. This capability was added only recently, and either flew under my radar or I failed to lock onto it.

Before posting, I checked Onshape help for silhouette edge (Search didn't find it, but that's presumably because my browser was getting chronically stuck in endless loops, because now I do find an entry - see note below)

I then opened an existing document (which I now realise pre-dated the new functionality) and could not get silhouette edges to work for me.

To top it all off, I had apparently mistaken your message in your original post and title, which seemed to suggest silhouette edges would also not work for you. So ... I fell into the error of deciding, on the evidence, it did not yet work.

I'm still having browser troubles so I cannot currently get it to work for me even with a new document. Hopefully someone more qualified to help you with workflow recommendations will chime in.

NOTE: this capability seems to have been enhanced since it was first implemented, because originally (according to the "What's New") it was restricted to cylindrical solid faces. In contrast, here's an excerpt from current Help:

• Supported silhouettes include: cylinders, cones, tori, spheres, extruded surfaces, and any surface with one silhouette.
• Silhouettes that are self-intersecting after projection are not usable.

lonnie_1

@andrew_troup, I am not sure I exactly understand it yet.:)   I would prefer to not have to project them and just have them available similar to other systems.  But there may be better methods and I am willing to learn new ways

andrew_troup

OK, I got it working for me (kind of - at first it wouldn't work unless the plane was away from the silhouette)

It does seem that silhouette edges are not available in the same way as in Solidworks, as a dormant entity available on demand for constraining geometry to: you have to create them (as you have found) with "Use/Project". However you can then extend them, and they bridge over holes in the face, so it seems to me there's little disadvantage to creating the geometry this way, rather than trying to constrain virgin geometry.

Here's the latest guff:
https://cad.onshape.com/help/#sketch-tools-use.htm?TocPath=Modeling%20in%20Onshape|Part%20Studio|Sketch%20Tools|_____15

and here's the original implementation (scroll down to third item) 
https://www.onshape.com/cad-blog/whats-new-6-29-15