Simple Polyline Sketch Example on Selected Plane

thomas_allsup

I can't find a Featurescript example where the user picks the plane or face in the precondition area.  All the examples I find use the "TOP" but I want to select one of the datums or an existing face to create my canned polyline logo.  Help!

NeilCooke

You just need to query a planar face, like this:

        annotation { "Name" : "Plane", "Filter" : EntityType.FACE && GeometryType.PLANE, "MaxNumberOfPicks" : 1 }
        definition.plane is Query;

thomas_allsup

Yes - I got that part working.  I can select the various planes and faces of a cube.  My problem is the execution part, I put:

        var face = definition.face;  //in your example, this would have been "plane"

               

        var sketch1 = newSketchOnPlane(context, id + "sketch1", {"sketchPlane" : face});   // if I change this "TOP" like all the examples, it will draw on the top plane 
                                

        skPolyline(sketch1, "polyline1", {"points" : [vector( 0,  0) * inch, vector( 1, 1) * inch, vector( 2,0) * inch, vector( 0,  0) * inch]}); // drawing a simple triangle  - this is where I would put my logo or other shape

        

        skSolve(sketch1);

        

        opExtrude(context, id + "extrude", {"entities" : qSketchRegion(id+"sketch1") , "endBound" : BoundingType.BLIND,"endDepth" : 1 * inch });


Thanks for the insights (I love the videos by the way and I have watched almost all of them).

NeilCooke

        var face = evPlane(context, { "face" : definition.face }); // definition.face is a Query, not a plane

        var sketch1 = newSketchOnPlane(context, id + "sketch1", { "sketchPlane" : face });

        skPolyline(sketch1, "polyline1", { "points" : [vector(0, 0) * inch, vector(1, 1) * inch, vector(2, 0) * inch, vector(0, 0) * inch] });

        skSolve(sketch1);

        opExtrude(context, id + "extrude1", {
                    "entities" : qCreatedBy(id + "sketch1", EntityType.FACE),
                    "direction" : face.normal,
                    "endBound" : BoundingType.BLIND,
                    "endDepth" : 1 * inch
                });

thomas_allsup

Wow - that fixed it and it makes complete sense.  I have to get queries straight.  THANKS!!!!

Jake_Rosenfeld

@NeilCooke @thomas_allsup

The right thing to do here is to use `newSketch` rather than `newSketchOnPlane`.  The former takes a face query and the latter takes a mathematical definition of a plane.  If you use the former, you will not need to call `evPlane`.

https://cad.onshape.com/FsDoc/library.html#newSketch-Context-Id-map
https://cad.onshape.com/FsDoc/library.html#newSketchOnPlane-Context-Id-map