You can create holes with different types and standards using
various options:
Hole Shape Parameters
This section provides information about different hole parameters such as type
limits, shape of the hole's end, and direction of the hole.
For any kind of hole (except blind hole) select the bottom limit.
The different types of limits are:
Blind
Up to Next
Up to Last
Up to Plane
Up to Surface
Limit types
To use the Up To
Plane or Up To
Surface option, you can define an offset between the
limit plane (or surface) and the bottom of the hole. For more
information, see Part Design User's Guide: Sketch-Based Features: Creating Pads Using
Limiting Surface.
If you use Up To Surface option, you can
select a face belonging to the current body only.
The Up To Next limit is the first face the
app 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.
Preview
Result
Direction
By default, the app creates the hole normal to the sketch face. But you can also define a
direction at a given angle to the face by selecting an edge or a line.
Contextual commands creating the directions you need are available
from the
Direction box.
Bottom Types
To define the shape of the hole's end, you can choose among three
options:
Flat: the hole is flat.
V-Bottom: the hole is pointed. You need to define how much
it is pointed by specifying an angle value.
Note:
Even if the hole is of the
Up To Surface
or
Up To Plane type, and if an offset value
is set from the target trimming element, the flat or V-bottom shapes are 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.
If the
Up to surface option is chosen, the
selected trimming surface must cover the hole cross-section at the hole's
bottom completely, otherwise the
feature cannot be created.
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
The following contextual creation commands are available on the
BOTTOM text:
Blind
Up To Next
Up To Last
Up To Plane
Up To Surface
Flat bottom
V bottom.
Type Tab
This section contains information about the different hole
types.
Various shapes of standard holes can be created. These holes are:
Simple
Tapered
Counterbored
Countersunk
Counterdrilled.
Simple
Tapered
Counterbored
Countersunk
Counterdrilled
If you choose to create a...
Tapered hole: By default, the diameter value you specify for a
tapered hole applies to the hole's bottom. If you prefer to specify the
diameter value for the hole's upper part, select
Top from the Anchor
point list, and enter the diameter value.
Note:
Blind and Up To holes,
computed radius values applying to the hole bottom may lead to
twisted geometry or auto crossing on profile. The app then generates a tapered hole with the shape of a simple
hole.
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 deg.
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 deg.
If you want to create a counterdrilled
hole with countersunk diameter, the countersunk diameter must be greater than
the hole diameter and smaller than the counterdrill diameter.
The following standards files are available by default for
counterbored holes under the
CounterBoredHole category.
Metric_Cap_Screws.xml
Socket_Head_Cap_Screws.xml
Metric_Cap_Screws Standard
The
Metric_Cap_Screws.xml hole standard uses
the following values.
Description
Diameter (mm)
CounterBored Diameter (mm)
CounterBored Depth (mm)
M1.6-Close
1.8
3.5
1.6
M1.6-Normal
1.95
3.5
1.6
M2-Close
2.2
4.4
2
M2-Normal
2.4
4.4
2
M2.5-Close
2.7
5.4
2.5
M2.5-Normal
3
5.4
2.5
M2.6-Close
3
6
2.6
M2.6-Normal
3.2
6
2.6
M3-Close
3.4
6.5
3
M3-Normal
3.7
6.5
3
M4-Close
4.4
8.25
4
M4-Normal
4.8
8.25
4
M5-Close
5.4
9.75
5
M5-Normal
5.8
9.75
5
M6-Close
6.4
11.2
6
M6-Normal
6.8
11.2
6
M8-Close
8.4
14.5
8
M8-Normal
8.8
14.5
8
M10-Close
10.5
17.5
10
M10-Normal
10.8
17.5
10
M12-Close
12.5
19.5
12
M12-Normal
13
19.5
12
M14-Close
14.5
22.5
14
M14-Normal
15
22.5
14
M16-Close
16.5
25.5
16
M16-Normal
17
25.5
16
M18-Close
18.5
28.5
18
M18-Normal
19
28.5
18
M20-Close
20.5
31.5
20
M20-Normal
21
31.5
20
M24-Close
24.5
37.5
24
M24-Normal
25
37.5
24
M30-Close
31
47.5
30
M30-Normal
31.5
47.5
30
M36-Close
37
56.5
36
M36-Normal
37.5
56.5
36
M42-Close
43
66
42
M42-Normal
44
66
42
M48-Close
49
75
48
M48-Normal
50
75
48
Socket_Head_Cap_Screws Standard
The
Socket_Head_Cap_Screws.xml hole standard
uses the following values.
Description
Diameter (inch)
CounterBored Diameter (inch)
CounterBored Depth (inch)
#0-Close
0.067
0.125
0.06
#0-Normal
0.073
0.125
0.06
#1-Close
0.081
0.15625
0.073
#1-Normal
0.089
0.15625
0.073
#2-Close
0.094
0.1875
0.086
#2-Normal
0.106
0.1875
0.086
#3-Close
0.106
0.21875
0.099
#3-Normal
0.12
0.21875
0.099
#4-Close
0.125
0.21875
0.112
#4-Normal
0.136
0.21875
0.112
#5-Close
0.141
0.25
0.125
#5-Normal
0.154
0.25
0.125
#6-Close
0.154
0.28125
0.138
#6-Normal
0.17
0.28125
0.138
#8-Close
0.18
0.3125
0.164
#8-Normal
0.194
0.3125
0.164
#10-Close
0.206
0.375
0.19
#10-Normal
0.221
0.375
0.19
1/4-Close
0.266
0.4375
0.25
1/4-Normal
0.281
0.4375
0.25
5/16-Close
0.328
0.53125
0.3125
5/16-Normal
0.344
0.53125
0.3125
3/8-Close
0.391
0.625
0.375
3/8-Normal
0.406
0.625
0.375
7/16-Close
0.453
0.71875
0.4375
7/16-Normal
0.469
0.71875
0.4375
1/2-Close
0.516
0.8125
0.5
1/2-Normal
0.531
0.8125
0.5
5/8-Close
0.641
1
0.625
5/8-Normal
0.656
1
0.625
3/4-Close
0.766
1.1875
0.75
3/4-Normal
0.781
1.1875
0.75
7/8-Close
0.891
1.375
0.875
7/8-Normal
0.906
1.375
0.875
1-Close
1.016
1.625
1
1-Normal
1.031
1.625
1
1-1/4-Close
1.281
2
1.25
1-1/4-Normal
1.312
2
1.25
1-1/2-Close
1.531
2.375
1.5
1-1/2-Normal
1.562
2.375
1.5
1-3/4-Close
1.781
2.75
1.75
1-3/4-Normal
1.812
2.75
1.75
2-Close
2.031
3.125
2
2-Normal
2.062
3.125
2
Notes:
You can create new standards as per the requirement. For more information,
see Creating Hole Standards.
This section contains information on different parameters of a threaded hole.
Note:
It is possible to thread tapered holes.
Hole Top
The hole top can be trimmed, depending on whether the hole is created in a positive or
a negative body.
If you create a hole in a positive body, that is a body containing
material, the
app
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 the example below, the hole encounters a
fillet placed above the face initially selected. The
app
redefines the hole's top onto the fillet.
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 app always trims the top of the hole using the Up to
Plane option and the plane used is the sketch plane.
Important:
If you create a Counterbored
type of hole with the Middle anchor point, the
counterbored part is trimmed.
Mechanical Interfaces Tab
Expand the Mechanical Interfaces section to instantiate an
existing simple mechanical interface template associated with different types of
holes and threads/taps and to generate tolerances and annotations at the time of
creation of holes and threads/taps.
Tolerance and annotations Generation
:
This option lets you decide whether to generate tolerances and
annotations or not.
By default, this option is not selected.
Click
to search and select a mechanical interface at the time of
creation of holes and threads/taps.
For the mechanical interface instantiation, a list of all the
existing mechanical interface templates which are associated with the selected
type of hole or thread/tap is displayed.
The simple mechanical interface template can be associated with one
of the following features at the time of template creation.
Hole
Tapered Hole
Counterbored Hole
Countersunk Hole
Counterdrilled Hole
Hole-Threaded
Tapered Hole-Threaded
Counterbored Hole-Threaded
Countersunk Hole-Threaded
Counterdrilled Hole-Threaded
Tap
Thread
To know about the creation of these templates See: Mechanical
Interface Template Capture User's Guide: Creating a Mechanical Interface
Template.
About Threads
You can define threads on a hole.
You can also define a threaded hole by clicking
option to access the parameters you need to define the
threads.
About Locating Holes
You can easily locate the holes on body.
To locate holes, keep in mind that:
The area you click determines the location of the hole, but you can drag the hole onto
desired location during creation using the left mouse button. If
Grid is
activated, you can use its properties.
Selecting a circular face makes the hole concentric with this face.
However, the
app
creates no concentricity
constraint.
Multi-selecting a circular edge and a face makes the hole
concentric to the circular edge. In this case, the
app
creates a concentricity constraint.
The Sketcher
app
provides commands to constrain the point used for locating the hole. See
Sketcher User's Guide: Setting Constraints.
Selecting a line and a face positions the hole along the line.
Editing the line modifies the hole accordingly.
Selecting an edge and a face allows the
app
to create a distance constraint. While creating the hole, you can double-click
this constraint to edit its value.
Methodology
There is certain methodology you have to follow while creating a
hole.
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 3D shape.
:
By default, this option is not selected.
to search and select a mechanical interface at the time of
creation of holes and threads/taps.
option to access the parameters you need to define the
threads.
is
activated, you can use its properties.
