holes to points in circular pattern

björn_britz

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

https://cad.onshape.com/documents/77cc24e31e90e449122e77d8/w/d1f202db6eb1dcbbafdfab8b/e/4bdd67a215f757924de91fa5

mahir

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

@mahir

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

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

The syntax for what @mahir mentions is

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

björn_britz

Alright! Now I got it!

Thanks a lot!

mahir

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

@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.

mahir

@Jake_Rosenfeld, gotcha. Thanks. Short version = "cuz"