||By default, the application
previews a blind hole whose diameter is 10mm and depth 10mm. Keep the
- Contextual creation commands are available on the 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, see Up to Surface Pad in the Part Design User's
- 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 through material.
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 positive body, that is a body containing
material, the application always trims 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 this example, the hole encounters a fillet placed above the face
initially selected. The application redefines the hole's top onto the
- 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.
To define the shape of the hole's end, you can choose between three
- Flat: the hole is flat.
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 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
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
- 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
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
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.
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.
Contextual commands creating the directions
you need are available from the Direction field:
- Create Line: for more information, see
- Create Plane: see
- 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.
Click the Type tab to access the
type of hole you wish to create. You are going to create a
If you choose to create that hole type,the
countersink diameter must be greater than the hole diameter and the
countersink angle must be greater than 0 and less than 180 degrees.
create such a hole you need to choose two parameters among the following
- Depth & Angle
- Depth & Diameter
- Angle & Diameter
Set the Angle & Diameter parameters in the
You will notice that the image assists you
in defining the desired hole.
Enter 80 degrees in the Angle field.
The preview lets you see the new angle.
Enter 35 mm in the Diameter field.
The preview lets you see the new diameter.
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 FunctionalBody.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.
Various shapes of standard holes
can be created. These holes are:
When creating 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
- 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
You can also define a threaded hole
by clicking the Thread Definition
tab and checking the Threaded button to access the parameters
you need to define.From
V5R16 onward, it is possible to
thread tapered holes.
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 four for defining your tolerance:
Selecting General Tolerance: sets a
pre-defined tolerance class for angular sizes according to the standard
selected for the session. By default, the general tolerance class is ISO
2768 - f.
Selecting Numerical values: 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.
Selecting Tabulated values: uses
Selecting Single limit: just enter a
minimum or maximum value. The Delta/nominal option 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
For more information, see the 3D Tolerancing and Annotations User's
After you set a tolerancing dimension, the icon turns red:
are 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.
Editing hole center points may sometimes take a
long time. Whenever your design includes several holes which center points
need to be edited, we strongly recommend you define intermediate bodies on
which you create the holes. Using intermediate bodies is a way of reducing
the number of operations affected by
changes. Once intermediate bodies are created, just assemble them to the