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opExtrude UP_TO_FACE Issue

aaron_skidmore
aaron_skidmore Member Posts: 34 ✭✭
in FeatureScript
Hi there, when I opExtrude as per below if the regionToExtrude is within the boundaries of the bottomface, it works ok, but if the regionToExtrude is outside the boundaries of the bottomface it doesnt work, is this expected behavior?  

opExtrude(context, id + "extrude1",
       { "entities" : regionToExtrude, 
        "direction" : zDirection *-1,
        "endBound" : BoundingType.UP_TO_FACE,   
        "endBoundEntity" : qNthElement(bottomface, 0),
        "operationType" : NewBodyOperationType.NEW,
        "defaultScope" : true
    });
Tagged:

Comments

  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,092 image
    Yes it is. If in doubt, try to replicate your use case using the regular modelling tools. 
    Senior Director, Technical Services, EMEA
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    Thanks Neil, so would I need to create a plane on the bottomface, then set endBoundEntity to that plane?
  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,092 image
    Is bottomface planar? If so, that would work. If bottomface is parallel to your sketch plane, measure the distance and use blind. 
    Senior Director, Technical Services, EMEA
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    Thanks Neil, I will go with measuring the distance and blind
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    @aaron_skidmore

    UP_TO_FACE is a deprecated option.  Please use UP_TO_SURFACE instead, which will expand the given face to its infinite boundary, if possible.  See: https://cad.onshape.com/FsDoc/library.html#BoundingType

    Internally, when selecting the "Up to face" option in the extrude feature, you are actually selecting UP_TO_SURFACE enum.  See the implementation here:
    https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/0ef5bec0909d4235a5ca1ebb
    Jake Rosenfeld - Modeling Team
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    Thanks I have that all running now. :)

    I am now struggling to find a way to get a solid bodies that intersection another solid body, via evCollision ? Or qIntersection ?
  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,092 image
    evCollision tells you if the bodies collide. If you want to find the resultant body created by the intersection of two bodies use opBoolean. qIntersection is the intersection of two queries (not what you want here). 
    Senior Director, Technical Services, EMEA
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    Ni Neil, I am not after the intersection between the 2 bodies, I need given bodyA, what other bodies are intersecting bodyA, do I need to get all bodies and  recursively run evCollision to test which ones intersect bodyA? 
  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,092 image
    evCollision will return an array of all collisions.
    Senior Director, Technical Services, EMEA
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    So I could try to cycle through bodies 1 at a time testing evCollision against the selected body - if there is any collision arrays then that body intersects? Could the same thing be done with multiple qIntersextion?
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    edited October 2020
    @aaron_skidmore

    qIntersection is not a geometric concept.  It is just a simple set intersection.  For example if I had two queries that represented:

    [face1, face3, face5] and [face1, face2, face3]

    The intersection of those two queries is [face1, face3]

    Similar to qUnion and qSubtraction, it is just a way to combine, find the overlap, or remove queries from each other.  See: https://cad.onshape.com/FsDoc/library.html#qIntersection-array

    evCollision ( https://cad.onshape.com/FsDoc/library.html#evCollision-Context-map ) will happily collide with multiple bodies at once.  
    const collisions = evCollision(context, { "tools" : bodyA, "targets" : qEverything(EntityType.BODY) -> qBodyType(BodyType.SOLID) });

var targetBodyArray = [];
for (var collision in collisions)
{
    targetBodyArray = append(targetBodyArray, collision.targetBody)
}

// To de-duplicate, since collisions are per-face/edge
const allTargetBodies = qUnion(targetBodyArray);

debug(context, allTargetBodies);


    Jake Rosenfeld - Modeling Team
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    The weird -> thing is supposed to just be "->".  Not sure what's going on there...
    Jake Rosenfeld - Modeling Team
  • aaron_skidmore
    aaron_skidmore Member Posts: 34 ✭✭
    Thanks for you help guys - I will try and get that to work - i think I have bitten off more than I can chew for my first go at a FeatureScript!

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