Translations:PartDesign ShapeBinder/20/en

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 PropertiesDialog/Data Tab 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 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.
 * Unfortunately we can not select the ShapeBinder for a Hole. Therefore we create a local sketch and use that for our hole in the second cube.
 * 1) Select the front face of the back cube and create a new sketch (click  for the suggestion in the dialog)
 * 2) Make all geometry invisible and the ShapeBinder visible. Now you can use the external geometry function and select the circle in the shape binder. We need the center point of that circle.
 * 3) Create a new circle and put it at the center point of the ShapeBinders circle. The radius is not important. The Hole function only uses the center points of the circles (note: single points are ignored by the Hole function, we must use circles)
 * 4) Close the sketch and click Hole. Set the dialog to the same values as the initial hole and press OK.