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Why can't shell remove all the sides of a box and just leave the top and bottom? Bug or feature?

Member Posts: 89 ✭✭
in Using Onshape


is good but add the back right side to the list and it fails.


I want to shell my surfboard profile and remove the side walls to generate the top and bottom skins. But because of the above limitation I can't seperate the top and bottom. I could #featurescript it but it seems an extravagence.

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  • Member Posts: 1,221 ✭✭✭✭✭
    why not to thicken top and bottom face with "new" option and delete the source body? possibly shell is not supposed to create new bodies
  • Onshape Employees Posts: 126
    Yes indeed, @konstantin_shiriazdanov. Shelling will not split a part into two. 'Thicken' would likely achieve the intended result.

    Paul Chastell
    TVP, Onshape R&D
  • Member Posts: 89 ✭✭
    That will only work of the faces are 90 degrees. If the faces have an internal angle greater than 90 degrees you can't just subtract and get the same effect as shelling and removing all walls. It would create jaggy steps at the corners.

    You can see the effect here. This is the side view. The bottom floor has been thickened up normal to the surface. The white area is the resulting solid. It can't be subtracted cleanly from the large blue solid.

     

  • Member Posts: 1,221 ✭✭✭✭✭
    then try boolean substract, you can set an offset to the particular faces of tool body
  • Member Posts: 89 ✭✭
    With regards to the answers "Shelling will not split an object in two" I might add that OnShape could do better with diagnostic errors.



    Leaves the user puzzled as to what has gone wrong
  • Member Posts: 89 ✭✭
    edited September 2017 Answer ✓
    This can be solved with a combination of move face and boolean against the original shape



    I'll probably featurescript it up.

    The above solution is
    at 

    https://cad.onshape.com/documents/f10a4813ff92ed33c78811e0/w/c09220311df8c0606b87d4af/e/5f770e7e954ddd09414b3645
  • Member Posts: 89 ✭✭
    Feature scripted

    function clone(context, query, id)
    {
        opPattern(context, id, {
                    "entities" : query,
                    "transforms" : [transform(vector(0, 0, 0) * inch)],
                    "instanceNames" : ["x"]
                }
            );
    }


    annotation { "Feature Type Name" : "Skin Face" }
    export const skinFaceFeature = defineFeature(function(context is Context, id is Id, definition is map)
        precondition
        {
            // Define the parameters of the feature type
            annotation { "Name" : "Face to skin", "Filter" : EntityType.FACE, "MaxNumberOfPicks" : 1 }
            definition.face is Query;

            annotation { "Name" : "Flip" }
            definition.flip is boolean;

            annotation { "Name" : "Thickness" }
            isLength(definition.thickness, LENGTH_BOUNDS);

            annotation { "Name" : "Keep object" }
            definition.keepObject is boolean;




        }
        {
            var solid = qOwnerBody(definition.face);

            var idTrans = id + "clone0";
            clone(context, solid, idTrans);

            if (definition.keepObject)
            {
                clone(context, solid, id + "clone1");
                //solid = dummyQuery(id + "clone1", EntityType.BODY);
            }

            var idMove = id + "FK4o00V6g8JW8BT_1";
            moveFace(context, idMove,
                    { "outputType" : MoveFaceOutputType.MOVE,
                        "moveFaces" : definition.face,
                        "surfacesAndFaces" : qUnion([]),
                        "moveFaceType" : MoveFaceType.OFFSET,
                        "direction" : qUnion([]),

                        "limitType" : MoveFaceBoundingType.BLIND,


                        "offsetDistance" : definition.thickness,
                        "oppositeDirection" : definition.flip,

                        "hasOffset" : false,
                        "offset" : definition.thickness,
                        "oppositeOffsetDirection" : definition.flip,
                        "reFillet" : false });


            opBoolean(context, id + "boolean1", {
                        "tools" : qCreatedBy(idTrans, EntityType.BODY),
                        "targets" : solid,
                        "operationType" : BooleanOperationType.SUBTRACTION

                    }
                );

            if (definition.keepObject)
            {

            }

        });

  • Moderator, Onshape Employees, Developers Posts: 1,646
    Hey Brad, Nice Job!

    The best way to share a Custom Feature is to write it in a public document (make sure to create a version when you're done) and copy/paste the link to that document.  That way other users who may want to use your feature can just open your document and add the feature to their toolbar like so:


    Jake Rosenfeld - Modeling Team
  • Member Posts: 89 ✭✭
    Jake_Rosenfeld said:
    Hey Brad, Nice Job!

    The best way to share a Custom Feature is to write it in a public document (make sure to create a version when you're done) and copy/paste the link to that document.  


    https://cad.onshape.com/documents/83f268820b92e08f4f30db06/w/ec7ac3c9e66d4c5dc475d388/e/e85455e9a0f5ab76faab2043
  • Member, Moderator, Onshape Employees, Developers, csevp, pcbaevp Posts: 2,011
    konstantin_shiriazdanov said:
    why not to thicken top and bottom face with "new" option and delete the source body? possibly shell is not supposed to create new bodies
    Or just thicken the top and bottom with the intersect option. 
    Lou Gallo / PD/UX - Support - Community / Onshape, Inc.
  • Member Posts: 89 ✭✭
    lougallo said:
    show previous quotes
    Or just thicken the top and bottom with the intersect option. 

    As I have shown in answers above. This does not work if the angle between faces is not 90degrees. Move face is the solution.
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