Creating Holes

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
In this section, you will find information about the main parameters you need for creating a hole:
This task illustrates how to create a countersunk hole while constraining its location.
To create a hole in Part Design, just open the Hole1.CATPart document. Otherwise, to create a hole in the Functional Molded Part workbench, sketch a rectangle in the Sketcher workbench then return to the workbench and create a shellable prism.

  1. Click the Hole icon to create a hole in Functional Molded Part.

  2. 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. 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.
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. For more about locating holes, refer to Locating Holes.
 

Extensions

For the Hole Bottom

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

Blind Up to Plane Up to Surface
  By default, the application previews a blind hole whose diameter is 10mm and depth 10mm. Keep the Blind option.
   
  • Contextual creation commands are available on the BOTTOM  text:
    • Blind
    • Up to Plane
    • Up to Surface
    • Flat bottom
    • V bottom
 
  • The Limit field is available if you set the Up to Plane or Up to Surface option.
  • 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 in the Part Design User's Guide.
 

 

Preview

Result
 

For the Hole Top

The hole top is trimmed in two ways depending on whether the hole is created in a positive body or not.

  • If you create a hole in a negative body, that is a body containing no material or a body with a negative feature as its first feature, the application always trims the top of the hole using the Up to Plane option and the plane used is the sketch plane.

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

Tolerancing Dimensions

You can define a tolerancing dimension for the hole diameter just by clicking the icon to the right of the Diameter field. This capability displays the Limit of Size Definition dialog box that enables you to choose one method among three for defining your tolerance:

  • Checking the Numerical values option: uses the values you enter to define the Upper Limit and optionally, the value of the Lower Limit field if you unchecked the Symmetric Lower Limit option.

  • Checking the Tabulated values option: uses normative references.

  • Checking the Single limit option: just enter a minimum or maximum value. The Delta/nominal options lets you enter a value in relation to the nominal diameter value. For example, if the nominal diameter value is 10 and if you enter 1, then the tolerance value will be 11.
 

The Options frame displays options directly linked to the standard used in the application. To know or change that normative reference, select Tools -> Options -> Mechanical Design -> Functional Tolerancing and Annotations, and in the Tolerancing tab enter the new standard in the Default Standard at creation option.
For more information, refer to the 3D Tolerancing and Annotations User's Guide.
After you set a tolerancing dimension, the icon turns red: . Toleranced holes are now identified by a specific icon in the specification tree.

Note that this capability is not available for countersunk and tapered holes and that a 3D Functional Tolerancing and Annotation license is required to be able to access this capability.

Hole Bottom

To define the shape of the hole's end, you can choose between three options:

  • Flat:  the hole is flat.

Even if the hole is of the Up to Plane or Up to Surface type, and even if an offset value is set from the target trimming element, the flat shape is never trimmed. The resulting geometry is therefore fully compliant with mechanical specifications.
   

  • V-Bottom: the hole is pointed. You just need to define how much it is pointed by specifying an angle value.

Even if  the hole is of the 'up to surface' or 'up to plane'  type , and even if an offset value is set from the target trimming element, the V-bottom shape is never trimmed. The resulting geometry is therefore fully compliant with mechanical specifications.

  • Trimmed: this option can be used if the limit chosen for the hole is of the 'Up to Next, 'Up to Last', 'Up to Plane' or 'Up to Surface'  type. The plane or surface used as the limit, trims the hole's bottom.

Note that hole features created with application releases anterior to Release 13 inherit the Trimmed option when necessary. In that case, a warning message is issued by the application.

Example of a Counterbored Hole With a V-bottom Trimmed by a Surface (Section View)
 
 
Example of a Counterbored Hole Trimmed by a Surface (Section View)
 
 

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

Directions
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.
 
  • Contextual commands creating the directions you need are available from the Direction field:
    • Create Line: for more information, see Creating Lines
    • Create Plane: see Creating Planes
    • X Axis: the X axis of the current coordinate system origin (0,0,0) becomes the direction.
    • Y Axis: the Y axis of the current coordinate system origin (0,0,0) becomes the direction.
    • Z Axis: the Z axis of the current coordinate system origin (0,0,0) becomes the direction.

    If you create any of these elements, the application then displays the line or the plane icon in front of the Direction field. Clicking this icon enables you to edit the element.
 

 

Threads

You can also define a threaded hole by clicking the Thread Definition tab and check the Threaded button to access the parameters you need to define.

When a hole defined in Functional Molded Part contains a thread specification, the corresponding thread representation is created in the drawing of the part. The thread representations in the drawing are generated on top view (3/4 of circle) and on lateral view.
 

Hole Types

  1. Click the Type tab to access the type of hole you wish to create.

    • 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.
 

  1. You are going to create a countersunk hole. To create such a hole you need to choose two parameters among the following options:

    • Depth & Angle
    • Depth & Diameter
    • Angle & Diameter

    Set the Angle & Diameter parameters in the Mode field.

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

 

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

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

  3. 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.

    If working in the Functional Molded Part workbench, Hole.X is added to the specification tree in the Solid Functional Set.X node. By default, as a protected feature, holes are in no show mode. To see the red protected area you have just created, set the Show mode.