'use feature' to project lines into perpindicular plan

brett_sutton

I'm trying to model a 1940s ceiling rose from my lounge room as I want to make a mould to make a print on our drive way.

So anyway, I'm new to Onshape and new to CAD, although I've use OpenSCAD for a couple of years to do some 3d printing.

The problem is that my model has a number of 'sun beams' radiating out from the top left of the model. Each of these sun beams needs to be shaped with a slope.

You can see the document with one of the rays lofted.

https://cad.onshape.com/documents/fae3550df7c64658a6c35c9c/w/888bd5116d12448a95970bdd

So I've managed to use a loft to create a shape for the beams by creating two sketches perpendicular to the lines of the sun beams.

My problem is that I'm trying to create a 'coincident' between a corner of one of the profiles for the loft and the sun beam's radiating lines and onshape refused to create the coincidence.

I've also tried 'projecting' the sun beam into the new sketch but it also refuses to do that.

Am I doing something wrong? Is there a better way of doing this?

andrew_troup

You're on the right track, @brett_sutton
The relation* constraint you need is called "Pierce"
What it does is compute the location of the point where a line passes through the sketch plane.
A coincident constraint between a point on a plane, and a line (A) which is not perpendicular to the plane, will allow the point to slide along the line (B) which represents a perpendicular projection of line A onto the sketch plane.
A "Use (Project/Convert)" will represent line A ( by producing line B ) as a perpendicular projection on the sketch plane.

* I edited this, because in Onshape, the term "relation" is reserved for one aspect of the mating process in assemblies.

andrew_troup

You're on the right track, @brett_sutton
The relation* constraint you need is called "Pierce"
What it does is compute the location of the point where a line passes through the sketch plane.
A coincident constraint between a point on a plane, and a line (A) which is not perpendicular to the plane, will allow the point to slide along the line (B) which represents a perpendicular projection of line A onto the sketch plane.
A "Use (Project/Convert)" will represent line A ( by producing line B ) as a perpendicular projection on the sketch plane.

* I edited this, because in Onshape, the term "relation" is reserved for one aspect of the mating process in assemblies.

brett_sutton

Andrew,
thanks for the response.
The pierce constraint solved my problem very nicely.

I still not certain I understand you 'use' example but I will have a play on a simple model and come back when I understand a bit more.

Again, thanks for your assistance.

Brett

andrew_troup

@brett_sutton

when I said perpendicular projection, I should have made it clear what the projection was perpendicular to. In the case of "Use", the projection is perpendicular to the sketch plane (which is effectively the 'destination' plane).

This is an important distinction, not specific to Onshape.

Contrasting two similar operations which produce different results: if you have two planes (a 'source' plane and a 'destination' plane) which are not parallel, and a line "A" on the source plane, you can project it to the destination plane by two methods. If you want the projection to be perpendicular to the source plane, you can extrude a surface, picking that line, "up to" the other plane. Then the far edge of that surface will represent the line you seek (call it "B1").

Whereas if you start a sketch on the destination plane, select line "A" and "Use" it, a line "B2" will be created on the destination plane, which is a projection of line "A" normal to the destination plane.