About Holes

There are a few things that you need to know about creating a hole.

This page discusses:

See Also
Creating Holes on Non-planar Faces
Locating Holes
Creating Threaded Holes

Hole Definition Options

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 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 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.
  • You can set new standards using Data Setup.

Threaded Hole Parameters

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.

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

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.