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

brad_phelan

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.

brad_phelan

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

konstantin_shiriazdanov

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

paul_chastell

Yes indeed, @konstantin_shiriazdanov. Shelling will not split a part into two. 'Thicken' would likely achieve the intended result.

brad_phelan

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.

 

konstantin_shiriazdanov

then try boolean substract, you can set an offset to the particular faces of tool body

brad_phelan

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

brad_phelan

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

brad_phelan

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)

        {

        }

    });

Jake_Rosenfeld

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:

brad_phelan

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

lougallo

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. 

brad_phelan

lougallo said:

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. 

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