PartDesign ShapeBinder

Description
Creates a datum shape binder inside the active Body. A shape binder is a reference object that links to edges or faces from another Body. It also can be used to link a sketch from one body to another body. The shape binder object displays as translucent yellow in the 3D view.

Examples of use would be to build a box with fitting cover in two different bodies or to make holes that are aligned between different bodies.



Usage

 * 1) Activate the Body the ShapeBinder should be nested in.
 * 2) Optionally select a single object, or one or more subelements (faces, edges or vertices) belonging to the same parent object. Subelements can only be selected in the 3D view.
 * 3) There are several ways to invoke the tool:
 * 4) * Press the button.
 * 5) * Select the option from the menu.
 * 6) The  task panel opens.
 * 7) Optionally select an object:
 * 8) Press the  button.
 * 9) Select an object in the Tree view or the 3D view.
 * 10) Any previously selected subelements will be removed.
 * 11) Optionally select subelements:
 * 12) Press the  button.
 * 13) Select a subelement in the 3D view.
 * 14) The  button has to be pressed for every subelement you want to add.
 * 15) Only subelements belonging to the same parent object can be selected. If required use the  button to select a different parent object.
 * 16) Optionally remove subelements:
 * 17) Press the  button.
 * 18) Select a subelement in the 3D view.
 * 19) The  button has to be pressed for every subelement you want to remove.
 * 20) Press the  button.

Options
Double-click a ShapeBinder in the Tree view, or right-click it and select from the context menu, to edit its parameters.

PartDesign SubShapeBinder vs. PartDesign ShapeBinder
See PartDesign_SubShapeBinder.

Properties

 * : support for the geometry.
 * : Default is . When, the shape binder does observe relative placements of the parts and bodies (by manipulating values of its hidden property).

Example
The example uses the ShapeBinder feature to make a hole (with or without threads) through more than one body. Normally the Hole function of the Part Design workbench is limited to a single body. The example uses two cubes facing each other but misaligned in an arbitrary way. The holes are created with sketches containing a circle for every hole (the diameter is ignored by the hole function). When you copy the sketch to the other cube it will be at the same position in the local cube coordinate system. In the image this is shown by the white circle on the back cube. This is not what we want, because the hole at that position would not be aligned to the hole in the front cube.



Here is how you use the ShapeBinder Feature to achieve it:
 * 1) Prepare a scene as per the above image. If you use the cubes from the Part workbench, remember that you must put them into a "body" container. Each one in a single body container. Otherwise the PartDesign functions would not work. If you build them from sketches the system should create body containers by default.
 * 2) Select the Properties Dialog Tab then Data to move the second cube to touch the first cube with a side displacement.
 * 3) Select the PartDesign workbench
 * 4) Create a sketch on the front face of the first cube and place a circle anywhere and close the sketch
 * 5) Select the sketch in the tree and press the Hole function button. Before make sure the first body is the active body (double-click).
 * 6) Select a hole of appropriate size. The image above had also counterbore selected. Close the Hole function.
 * Now the image should look as above. When you hide the first cube (select and press space) you can see that the hole does not reach the second cube. It will not, even when you select "Through All", or when you enter a really large distance in the Hole dialog. The hole dialog is always limited to a single body.
 * Here is where our ShapeBinder comes in.
 * 1) First select the back cube. This is the target where the ShapeBinder will be added. It must be actived before, so be sure it has been double-clicked.
 * 2) In the tree select the sketch we used for the hole. It's important to not activate the first body.
 * 3) Select the shapeBinder function.
 * A dialog should open. In the line "Object" the name of our sketch should be visible. If you had selected the function without selecting the sketch, you could press "Object" and then select the sketch from the list. It's recommended to select it first in order to get the right one, especially if you have many sketches with automatically generated names Sketch001,.. The "Add Geometry" is not useful for us, because we want to select the whole sketch. "AddGeometry" is used if only parts should be selected.
 * 1) Press  to close the dialog and check that a new item has been added to the tree of the second cube.
 * When you toggle the visibility of the ShapeBinder it is shown yellow in the 3D view. However it's on the wrong position, just as the white circle in the image above. That is because of the default setting for the Trace parameter.
 * 1) In the PropertyView of the ShapeBinder in the Data tab set the Trace Support parameter to true. The default was false.
 * With Trace Support true, the ShapeBinder in not affected by local transformations of the target body, e.g. our translations. The shape remains exactly where the original front object shape has been. Try moving the front object around and you can see that the ShapeBinder always follows to the new position.
 * 1) Select the ShapeBinder in the tree and press the Hole function button. If you enter the same values as for the initial hole you will notice that no hole is created in the second cube. This is because a ShapeBinder in some cases has an opposite "tool direction" compared to the referenced sketch. To solve this check the Reverse checkbox. Press OK to finish.
 * 2) You now have linked holes in two different bodies. If you change the position of the circle in the sketch, both holes will adapt. You can even add new circles in the sketch to create additional linked holes.