Hole

Creating a hole consists in removing material from a body. Various shapes of standard holes can be created. These holes are:


Simple	Tapered	Counterbored	Countersunk	Counterdrilled

If you choose to create a...

Counterbored hole: the counterbore diameter must be greater than the hole diameter and the hole depth must be greater than the counterbore depth.

Countersunk hole: the countersink diameter must be greater than the hole diameter and the countersink angle must be greater than 0 and less than 180 degrees.

Counterdrilled hole: the counterdrill diameter must be greater than the hole diameter, the hole depth must be greater than the counter drill depth and the counterdrill angle must be greater than 0 and less than 180 degrees.

Whatever hole you choose, you need to specify the limit you want. There is a variety of limits:


Blind	Up to Next	Up to Last	Up to Plane	Up to Surface

The 'Up to next' limit is the first face the application detects while extruding the profile, but this face must stops the whole extrusion, not only a portion of it, and the hole goes thru material.

Preview

Result

If you wish to use the Up to Plane or Up to Surface option , you can then define an offset between the limit plane (or surface) and the bottom of the hole. For more information, refer to Up to Surface Pad.

You can also choose the shape of the end hole (flat or pointed end hole) and specify a threading.

The application always limits the top of the hole using the Up to Next option. In other words, the next face encountered by the hole limits the hole.

In the following example, the hole encounters a fillet placed above the face initially selected. The application redefines the hole's top onto the fillet.

Creating a Hole

This task illustrates how to create a counterbored hole while constraining its location.

Open the Hole1.CATPart document.

Click the Hole icon

Select the circular edge and upper face as shown.

The application can now define one distance constraint to position the hole to be created. The hole will be concentric to the circular edge.

For more about locating holes, please refer to Locating a Hole .

The Hole Definition dialog box appears and the application previews the hole to be created. The Sketcher grid is displayed to help you create the hole. By default, the application previews a simple hole whose diameter is 10mm and depth 10mm.

Contextual creation commands are available on the BOTTOM text:

Depth

Up to next

Up to last

Up to plane

Up to surface

Now, define the hole you wish to create. Enter 24mm as the diameter value and 25mm as the depth value.

The Limit field is available if you set the "Up to Plane" or Up to Surface" option.

Clicking the icon

opens the Sketcher. You can then constrain the point defining the hole position.

Once you have quit the Sketcher, the Hole Definition dialog box reappears to let you define the hole feature.

Set the Bottom option to V-Bottom to create a pointed hole and enter 110 in the Angle field to define the bottom shape.

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 unchecking the Normal to surface option and selecting an edge or a line.

You can also define a threaded hole by checking the Thread Definition tab and click the Specifications button to access the parameters you need to define.

Now, click the Type tab to access the type of hole you wish to create. You are going to create a countersunk hole.

Using this new product release, to create a countersunk hole you need to choose two parameters among the following options:

	Depth & Angle
	Depth & Diameter
	Angle & Diameter

Set the Angle and Diameter parameters in the Mode field.

You will notice that the glyph assists you in defining the desired hole.

Enter 80degrees in the Angle field. The preview lets you see the new angle.

Enter 35mm in the Diameter field. The preview lets you see the new diameter.

Click OK.

The hole is created. The specification tree indicates this creation.

You will notice that the sketch used to create the hole also appears under the hole's name. This sketch consists of the point at the center of the hole.