Simple Polyline Sketch Example on Selected Plane

Comments

• NeilCooke Moderator, Onshape Employees Posts: 5,922

  April 2020

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

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

  
  

  Senior Director, Technical Services, EMEA

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• thomas_allsup Member, User Group Leader Posts: 4 ✭

  April 2020

  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).

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• NeilCooke Moderator, Onshape Employees Posts: 5,922

  April 2020

          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
                  });

  
  

  Senior Director, Technical Services, EMEA

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• thomas_allsup Member, User Group Leader Posts: 4 ✭

  April 2020

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

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• Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646

  May 2020

  @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
  

  Jake Rosenfeld - Modeling Team

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