-
From the Features section of the action bar,
click Hole
.
If your geometry does not have a sketch entity to use as the hole origin, you
need to add a sketch object on the geometry.
-
From the Sketch section of the action bar, click Point
.
-
In the work area, click on the geometry to place the point
where you want the hole.
You can use other sketch commands to create sketch entities on the
geometry, for example, sketch a rectangle to use the four corner
entities as the location for the holes.
-
In the
Hole dialog box, click the
Placement tab.
-
Select a sketch entity from the
work area
to specify the location for the hole.
You can select multiple sketch entities if all the holes have the
same design requirements. If you have a sketch object selected with multiple
entities, all the possible hole positions are selected by default.
Note:
You cannot apply this feature to a sheet metal geometry.
Instead, switch to the xSheetMetal app, and select SheetMetal
Cutout from the SheetMetal section.
- Optional:
Click
Ignore construction geometry to exclude any
construction geometry from your selections.
- Optional:
To skip some of the selected sketch entities in a sketch object,
click
Skip instance.
A marker is displayed on all the sketch entities in the
selected sketch object. Click the marker to prevent that entity from creating a
hole.
-
Click the
Design tab.
-
Select the
Hole Type from the menu.
Option | Description |
---|
|
Straight. Creates a simple
hole. |
---|
| Straight
Tapped. Creates a hole with a straight thread.
|
---|
| Counterbore.
Creates a counterbore hole.
|
---|
| Countersink.
Creates a countersink hole with head clearance. |
---|
| Taper Tap.
Creates a countersink hole with head clearance. |
---|
-
From the
Standard list, select the engineering and
manufacturing standard for dimensioning holes.
Option | Description |
---|
ASME Inch |
General-purpose standard for dimensional inch series
engineering and manufacturing. |
---|
ASME Metric | Metric standards for
worldwide engineering and manufacturing. |
---|
DIN | German Institute for
Standardization (Deutsches Institut für Normung) for engineering and
manufacturing. |
---|
ISO | The International
Organization for Standardization meets the requirements, specifications,
guidelines, or characteristics that ensure that materials are consistent in the
products. |
---|
-
From the
Hardware Type
list, select a type of drill or dowel.
-
From the
Size list, select a size for a hole.
The sizes vary depending on the
Standard selection.
-
From the
Fit list, select the tightness of hole to fit
the hardware.
This option is available only for
Straight,
Counterbore, and,
Countersink hole types.
-
Under
Hole Dimensions, specify the dimensions such
as
Diameter,
Depth,
Distance, and
Bottom treatment for a hole.
Note:
Click to reset the dimensions to the default values.
The Dimension Edit Box is displayed. Type the
value for the dimension and press
Enter.
The
Hole dimension options vary depending on the
selection of hole type.
-
Specify
Near Side Options and
Far Side Options.
-
Click
.
|