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holes to points in circular pattern

björn_britz
björn_britz Posts: 14 EDU
in FeatureScript
i want to do holes. i created points in a circular pattern as the center for the holes.
no i have difficulties defining the locations and the scope in fs for the holes.

                    const anzahl = dimensions.Rotation;
                    for (var i = 0; i < anzahl; i += 1)
                    {
                        const t= rotationAround(rotationAxis, (2*PI* radian) * (i/anzahl) );
                        const point3d = t * patternPoint;
                        const point2d = vector(point3d[0],point3d[1]);
                        skPoint(PointSketch, "point" ~i, {
                                "position" : point2d
                        });
                       
 /*                       hole(context,"hole"~i, {
                       
                        "style" : HoleStyle.SIMPLE,
                        "endStyle" : HoleEndStyle.BLIND,
                        "holeDiameter": 2*millimeter,
                        "holeDepth":3*millimeter,
                        "locations": XX,
                        "scope": XX
                        });
*/
                    }


heres the file:  the problem starts in line 247


Tagged:

Comments

  • mahir
    mahir Posts: 1,324 ✭✭✭✭✭
    edited August 2018
    You need to solve the sketch before the hole feature, not after. For locations, try querying using qCreatedBy(id + "pointSketch", EntityType.VERTEX). For scope, you need to enter a query for the body/bodies you want the hole to go through.
  • björn_britz
    björn_britz Posts: 14 EDU
    Oh right, thanks! I changed the solving thing.

    For locations, I tried your suggestion and for scope i tried  qSketchRegion(id + "sketch")  -- that's the sketch on which all the bodies, i want the holes to go through, are.

    It throws the error:
    throw INVALID_INPUT and throw HOLE_CUT_FAIL
  • mahir
    mahir Posts: 1,324 ✭✭✭✭✭
    edited August 2018
    No, by body I mean a solid body. "Scope" is short for "boolean merge scope". The hole feature wants to know which solid body it should remove material from. So the query needs to look something like qCreatedBy(nameOfFeatureThatCreatedBody, EntityType.BODY && BodyType.SOLID).
  • Jake_Rosenfeld
    Jake_Rosenfeld Posts: 1,646 image
    The syntax for what @mahir mentions is

    qBodyType(qCreatedBy(<someId>, EntityType.BODY), BodyType.SOLID)

    Jake Rosenfeld - Modeling Team
  • björn_britz
    björn_britz Posts: 14 EDU
    Alright! Now I got it!
    Thanks a lot!
  • mahir
    mahir Posts: 1,324 ✭✭✭✭✭
    Jake_Rosenfeld said:
    The syntax for what @mahir mentions is

    qBodyType(qCreatedBy(<someId>, EntityType.BODY), BodyType.SOLID)

    Jake, I'm curious. Why is that preferred to "EntityType.BODY && BodyType.SOLID"? It's what the hole feature uses internally for it's scope query.
  • Jake_Rosenfeld
    Jake_Rosenfeld Posts: 1,646 image
    edited August 2018
    @mahir

    As described in the FS documentation:

    Under the "Queries" section of https://cad.onshape.com/FsDoc/uispec.html

    The `&&` operator in the body of a feature can only take booleans as its left and right hand side.  "EntityType.BODY && BodyType.SOLID" would just be a syntax error because neither of those are booleans.  The &&, ||, and ! operators are special cased for Query Parameter filters, but there is no special case within the code itself, and queries must be composed using the provided query functions.
    Jake Rosenfeld - Modeling Team
  • mahir
    mahir Posts: 1,324 ✭✭✭✭✭
    @Jake_Rosenfeld, gotcha. Thanks. Short version = "cuz" ;)

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