Using Hole Series

	The new concept of "hole series" lets you create different holes cutting the individual parts of an assembly. The "series" option, available in the Hole command lets you determine the parts that are to be cut or not, and the hole types to define for these parts. In this task, you will create one assembly hole feature composed of three different holes cutting four parts.
	Open the AssemblyHole2.CATProduct document.
	1.	Click the `Hole` icon .
	2.	Select the upper purple face to define the location of the hole: The Hole Definition and Assembly Features Definition dialog boxes appear. The Assembly Features Definition dialog box displays the names as well as the paths of the parts that may be affected by the hole creation. For more details, refer to the task "Assembly Hole".
	3.	Click the button to move all parts to the list 'Affected parts'.
	4.	To define the hole cutting the assembly, set these parameters: " Up to Last", 10 mm as the diameter value, "Counterbored", 18 mm as the diameter option. The application previews the counterbored hole.
		Creating Series A hole series gathers one or more assembly parts that must be cut by a hole different from the hole previously defined.
	5.	Click the button "Add Series". A new tab "Series 1" displays, containing all parts selected in the "affected parts" field of the Default tab.

	6.	To identify the parts you wish to include in Series 1, multi-select Part5 and Part6 then click the Select button. The mention "Yes" now displayed in the Selected field, confirms that Series 1 includes these parts that will be cut by a hole which parameters are still to be defined.
		Series 1 then includes two parts through which the hole will pass. On the contrary, Part7 and Purple part are excluded from the series as indicated by the mention "No".

	7.	To define the hole you need for Series 1, enter these parameters: "Up to Last", 12 mm as diameter value and "Simple" in the Hole Definition dialog box.
		The application previews this hole type on the purple face.
	8.	Click the button "Add Series" again to create another series. A new tab "Series 2" displays, containing all parts selected in the "affected parts" field of the Default tab..
	9.	Select Part 7 then click the Select button to set this part as the only part composing the series. The mention "Yes" confirms that this part will be cut by a new hole which parameters are still to be defined.
		Another way of selecting the part is to double-click its name.
	10.	To define the hole you need for Series 2, enter these parameters: "Blind", 10 mm as diameter value, 160mm as depth value, "V-Bottom", "Simple", "Threaded" and the thread values of your choice in the Hole Definition dialog box.
		The application previews this hole type on the purple face.
		Note that the Default button removes one part from a series.
	11.	Click OK to confirm. The hole defined through three series cuts the assembly.
		In the specification tree, the Assembly Hole node displays the different parts cut by the Hole feature. Note that the icon identifying the threaded hole differs from the other icons.

Using Hole Series

Creating Series