Assembly Hole 

The Assembly Hole command lets you create holes going thru different parts. You could actually create holes for each part in the Part Design workbench, but the Assembly Hole command available in Assembly Design workbench creates holes more rapidly and more productively: the command creates a hole going thru several parts in only one interaction. 
  You can create distinct shapes of holes going thru the individual parts of an assembly and this, in one shot. To know how to do this, please refer to Using Hole Series.
This task shows you how to create a hole on a product including three parts, but you can create the hole on two parts only.
Open the AssemblyHole.CATProduct document.

  1. Click the Hole icon:

 

  1. Select the purple face as shown to define the location of the hole:
 
 

The Assembly Features Definition dialog box appears.
 
 

The dialog box displays the names as well as the paths of the parts that may be affected by the hole creation. 
 

The assembly feature's name appears in the Name field. If desired, you can edit this name.
 

The frame Affected parts is exclusively reserved for the parts you wish to use. Purple Part is displayed in this frame.
 

Note that the Hole Definition dialog box is displayed.
 

  1. As you wish to create a hole between Part5 and Purple Part, move Part5 to the list Affected parts.
 

The other three buttons lets you move the names of the parts from one list to another too:
 

  • moves all selected parts to the list Affected parts.

  • moves all selected parts to the list Parts possibly affected.

  • moves the selected part to the list Parts possibly affected.
 

  1. Check the option Highlight affected parts to clearly identify the parts.
 

At this point, you can now define the hole you wish.
 

You cannot edit the hole positioning sketch from the assembly hole definition, this why the icon still grayed.
If you wish to edit it, double-click the Positioning Sketch created in the part from which you have defined the assembly hole, or edit the reused hole.
 

Whatever hole you choose, you need to specify the limit you want. If you do not specify a depth value, four types of limits are available:
 
 
Blind Up to Last Up to Plane Up to Surface
 

  1. Set the Up to Last option. The application extends the hole from the sketch plane to the last face encountered.
 

  1. Enter 25mm as the diameter value.
 

By default, the application creates the hole normal to the sketch face. But you can also define a creation direction not normal to the face by deselecting the Normal to surface option and selecting an edge or a line.
 

If you are designing a blind hole, you can set the Bottom option to V-Bottom to create a pointed hole and then enter the angle value of your choice.
 

Clicking the Type tab lets you create the following holes:
 
 
Simple Tapered Counterbored Countersunk Counterdrilled
 

Make sure the option Simple is set.

 

Clicking the Thread Definition tab lets you access to the options defining threads. For more information about threads and holes, please refer to Part Design User's Guide.
 

  1. Click OK to confirm.
 

The hole is created on Part 5 and Purple Part. Conversely, CRIC_FRAME is intact.
 
 

A new entity Assembly features appears in the specification tree. It contains the assembly hole referred to as Assembly Hole.1 and the affected parts.
 

Moreover, this feature has generated a hole in each part. An arrow symbol identifies these holes in the tree, meaning that a link exists between Assembly Hole.1and them.
 

Editing an Assembly Hole
To edit an assembly hole, double-click Assembly Hole.X entity then you can either:
 
  • modify the list of affected parts.
  • edit the hole.
  If you need to cut the link between a generated hole and Assembly Hole.1, just use the Isolate contextual command. Obtain a classical hole as if you have designed it in Part Design and you can edit it in Part Design.
 

Reusing Part Design Holes
  To increase your productivity, you can create Assembly holes from existing Part Design holes, or more precisely by reusing the specifications you entered for designing Part Design holes. To do so, just proceed as follows:
Before reusing Part Design hole, take note that:
  • You cannot reuse hole for which the reference geometry for creation is not a planar surface.
  • You cannot reuse a hole with the Up to next option, because this option is not applicable for assembly hole.
  • You cannot re-affect an assembly hole on the part which contains the part hole, except if the diameter of the assembly hole exceed the diameter of the part hole, or if the assembly hole location is different. In fact, you cannot drill vacuum.
 

  1. Click the Hole icon:

 

  1. Select the Part Design hole of interest.
 

  1. Both the Hole Definition and the Assembly Features Definition dialog boxes display. You then just need to specify the parts to pierce.
 

The assembly hole inherits the specifications as displayed in the Part Design Hole Definition dialog box. You can edit these specifications at any time. Editing an Assembly feature created in this way does not affect the specifications used for the Part Design feature.

Reusing Assembly Design Holes
The application also lets you reuse Assembly Holes' specifications to accelerate the design process. In this case, you just need to select the existing assembly hole, click the Assembly hole icon and then select a face. Only the Assembly Features Definition dialog box appears to let you determine the parts to drill.