Creating a hole consists in
removing material from a body. Various shapes of standard holes
can be created. These holes are: |
|
|
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. |
 |
-
Click the Hole
icon
to create a hole in Functional Molded Part.
-
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:
|
|
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.
-
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:
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)
|
|
 |
|
-
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. |
|
|
|
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
|
|
-
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.
|
|
|
-
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.
|
 |
|
-
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.
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.
|