Using a closed loop sketch as path for opSweep

mortezaPourmohamadi

Hi,
I'm trying to use a sketch inside FS as a path for the opSweep function. 
It works fine when the sketch contains a few connected lines, but it throws an error as soon as it becomes a closed-loop (e.g. a rectangular path). 
Any idea how it can be resolved?

        var path1 = newSketch(context, id + "path1", {

                "sketchPlane" : qCreatedBy(makeId("Front"), EntityType.FACE)

            });

        skRectangle(path1, "rectangle1", {

                    "firstCorner" : vector(0, 0) * inch,

                    "secondCorner" : vector(10, 10) * inch

                });

        // Create sketch entities here

        skSolve(path1);

        var profile1 = newSketch(context, id + "profile1", {

                "sketchPlane" : qCreatedBy(makeId("Top"), EntityType.FACE)

            });

        skCircle(profile1, "circle1", {

                    "center" : vector(0, 0) * inch,

                    "radius" : 0.5 * inch

                });

        // Create sketch entities here

        skSolve(profile1);

        opSweep(context, id + "sweep1", { // @opSweep: SWEEP_SELECT_PATH

                    "bodytype" : ToolBodyType.SOLID,

                    "operationType" : NewBodyOperationType.NEW,

                    "profiles" : qCreatedBy(id + "profile1", EntityType.FACE),

                    "path" : qCreatedBy(id + "path1", EntityType.EDGE)

                });



and the error message:

@opSweep: SWEEP_PATH_FAILEDonshape/std/geomOperations.fs (const opSweep)onshape/std/feature.fs (defineFeature)Case Carcass (const plyBody)

Jacob_Corder

@mortezaPourmohamadi

Did you try Kontstantins solution? When sketches are solved, the entites become wire bodies. It is also true that multiple edges are created as Konstantin stated above.

for the profile you could use
sketchEntityQuery(id+"profile1", EntityType.EDGE, "circle1");
or
qAdjacent(qCreatedBy(id+"profile1",EntityType.FACE),AdjacencyType.EDGE,EntityType.EDGE)
  
for the path if it is closed, qAdjacent(qCreatedBy(id+"path1",EntityType.FACE),AdjacencyType.EDGE,EntityType.EDGE)
or
sketchEntityQuery(id+"path1", EntityType.EDGE, "rectangle1");

konstantin_shiriazdanov

I think it is because closed sketch creates multiple coinciding edges. Try this:

"path" : qCreatedBy(id + "path1", EntityType.BODY)-> qBodyType(BodyType.WIRE)->qOwnedByBody(EntityType.EDGE)

mortezaPourmohamadi

Thanks @konstantin_shiriazdanov

This didn't solve the issue, though. There is no BODY in the "path1" sketch, so the resulting WIRE and EDGE list would be empty.

Jacob_Corder

@mortezaPourmohamadi

Did you try Kontstantins solution? When sketches are solved, the entites become wire bodies. It is also true that multiple edges are created as Konstantin stated above.

for the profile you could use
sketchEntityQuery(id+"profile1", EntityType.EDGE, "circle1");
or
qAdjacent(qCreatedBy(id+"profile1",EntityType.FACE),AdjacencyType.EDGE,EntityType.EDGE)
  
for the path if it is closed, qAdjacent(qCreatedBy(id+"path1",EntityType.FACE),AdjacencyType.EDGE,EntityType.EDGE)
or
sketchEntityQuery(id+"path1", EntityType.EDGE, "rectangle1");

mortezaPourmohamadi

Thanks @Jacob_Corder

This worked beautifully!