Unable to fillet an existing object - Need help

andrew_hastings190

Hi,

I am unable to fillet an existing object, it always throws up errors and ive tried everything to get around this such as trying to draw arcs with lines so i wouldnt have to fillet after i extrude to no avail.

Here is my code:

var length = 100*millimeter;

        var depth = 50*millimeter;

        var width = 500*millimeter;

        var thickness = 5*millimeter;

        

        

        var sketch1 = newSketch(context, id + "sketch1", {

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

        });

        

        skRectangle(sketch1, "rectangle1", {

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

                "secondCorner" : vector(width,length)

        });

        

        skSolve(sketch1);

        

        extrude(context, id + "extrude1", {

                "entities" : qSketchRegion(id + "sketch1"),

                "endBound" : BoundingType.BLIND,

                "oppositeDirection" : true,

                "depth" : depth

        });

        

        var sketch2 = newSketch(context, id + "sketch2", {

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

        });

        

        skRectangle(sketch2, "rectangle2", {

                "firstCorner" : vector(thickness,thickness),

                "secondCorner" : vector(depth,length-thickness)

        });

        

        skSolve(sketch2);

        

        extrude(context, id + "extrude2", {

                "entities" : qSketchRegion(id + "sketch2"),

                "endBound" : BoundingType.BLIND,

                "operationType" : NewBodyOperationType.REMOVE,

                "depth" : width

        });

        

        opFillet(context, id + "fillet1", {

                "entities" : qCreatedBy(id + "extrude2", EntityType.EDGE),

                "radius" : 2.5*millimeter

        });

        

There arent any preconditions, im unsure how to find out which edges to fillet manually and I want it all in one feature. I just want the the inner edges (the concave ones) to be filleted rather than all the edges around it.

Thanks,

ilya_baran

It can be a little tricky to select just the edges you want and there are usually several ways.  For example, the following code creates a query for all edges such that both adjacent faces are created by extrude2 (this resolves to the two edges you want):

        var facesNotByExtrude2 = qSubtraction(qEverything(EntityType.FACE), qCreatedBy(id + "extrude2", EntityType.FACE));

        var adjacentEdges = qEdgeAdjacent(facesNotByExtrude2, EntityType.EDGE);

        var innerEdges = qSubtraction(qCreatedBy(id + "extrude2", EntityType.EDGE), adjacentEdges);

Another way is to look for all concave edges among those created by extrude2:

        var concaveEdges = [];

        for (var edge in evaluateQuery(context, qCreatedBy(id + "extrude2", EntityType.EDGE)))        

        {

            if (evEdgeConvexity(context, { "edge" : edge}) == EdgeConvexityType.CONCAVE)

                concaveEdges = append(concaveEdges, edge);

        }

        

        opFillet(context, id + "fillet1", {

                "entities" : qUnion(concaveEdges),

                "radius" : 2.5*millimeter

        });

Yet another way is to do the fillet manually and munge the code from the part studio -- you get something like:

        var e1 = makeQuery(id + "extrude2.boolean.opBoolean", "COPY", EntityType.EDGE, { "derivedFrom" : makeQuery(id + "extrude2.opExtrude", "SWEPT_EDGE", EntityType.EDGE, { "disambiguationData" : [originalSetDisambiguation([sketchEntityQuery(id + "sketch2.wireOp", EntityType.EDGE, "rectangle2.left"), sketchEntityQuery(id + "sketch2.wireOp", EntityType.EDGE, "rectangle2.bottom")])] }) });

        var e2 = makeQuery(id + "extrude2.boolean.opBoolean", "COPY", EntityType.EDGE, { "derivedFrom" : makeQuery(id + "extrude2.opExtrude", "SWEPT_EDGE", EntityType.EDGE, { "disambiguationData" : [originalSetDisambiguation([sketchEntityQuery(id + "sketch2.wireOp", EntityType.EDGE, "rectangle2.left"), sketchEntityQuery(id + "sketch2.wireOp", EntityType.EDGE, "rectangle2.top")])] }) });

        

        opFillet(context, id + "fillet1", {

                    "entities" : qUnion([e1, e2]),

                    "radius" : 2.5 * millimeter

                });

This approach is a last resort -- the result is nearly unreadable, but has the advantage that it lets you pick specific edges without any rule or logic that ties them together.

andrew_hastings190

Thank you very much! It has filleted the parts out properly