-
From the
Annotation section of the
action bar,
click
Tolerancing Advisor.
-
Select multiple holes as shown below.

-
In the
Semantic Tolerancing Advisor dialog box, click
the
Position Specification:(N cylinders
in Collection (Nx CZ)).
The
Geometrical Tolerance dialog box appears.
-
Under the
Tolerance Value area, specify the required
tolerance value.
-
In the
General tab, select the
Display CZ modifier check box and keep the
remaining options as they are.
You can click
Display median feature symbol to display the
median feature symbol in the tolerance frame.
-
Under
Two Parallel Planes Tolerance Zone, specify
the geometrical tolerance symbols for orientation plane auxiliary plane
indicator. To do so:
-
From the list, select the required auxiliary feature
indicator.
When you select angularity
, a theoretically exact dimension is created between the
constructed geometry and the datum feature.
-
Specify the required datum feature.
If not available, from the list, you can select
Create datum and create it. This datum
feature is not removed even when you delete the specified geometrical
tolerances.
The auxiliary plane indicator,
Orientation plane,
Intersection plane, or
Collection plane, appear automatically
based on the selected elements.
- Optional:
To specify the geometrical tolerance indicators for intersection
plane auxiliary plane indicator:
-
Select the face of the feature as displayed and then the
Straightness Specification
.
-
In the
General tab, under
Toleranced Lines Definition, specify the
geometrical tolerance indicators for intersection plane. To do so:
- From the list, select the required auxiliary feature
indicator.
- Specify the required datum feature.
Note:
The leader extremities of geometrical tolerance are always
a filled circle
except when there are extension lines or when they are
in the alignment of dimensions.
- Optional:
To specify the profile of a line or a surface geometrical
tolerance indicators applied in common zone to several features for collection
plane auxiliary plane indicator:
-
Select multiple faces and then the
Profile-of-Surface specification.
-
In the
Toleranced Feature tab, under
All round, specify the geometrical
tolerance indicators for collection plane. To do so:
- From the list, select the required auxiliary feature
indicator.
- Specify the required datum feature.
Note:
All the auxiliary feature indicators become invalid when you
switch to ASME standard.
-
In the
Tolerance Zone tab,
-
Click
Projected Tolerance Zone.
-
Click
Create/Edit available next to the
Extended Cylinder Selection list.
The
Extended Cylinder Construction Geometry
dialog box appears.
-
In the
Reference plane box, select the reference
face on which the hole is created.
-
In the
Length and
Offset boxes, enter the required length
and offset of the extended cylinder from the reference plane respectively.
-
Click
OK.
-
In the
Geometrical Tolerance dialog box, select the
Show length and offset in tolerance frame
check box.
The length and offset values are displayed in the
tolerance frame.
-
In the
Notes tab,
-
Enter the required information in the various text editors
available.
-
Select the
Automatic display of Nx at check box and
select the
upper bottom in the list.
The number of selected components or elements is
displayed in the upper bottom text editor.
Note:
You can also select
<nbr> in the
Insert list to specify the number of
components in the selected text editor.
-
Click
OK.
The geometrical tolerance feature is created on the
selected holes.
-
Click
Close in the
Semantic Tolerancing Advisor dialog box.
-
For the selected semantic geometrical tolerance, datum target
annotation, and the datum systems, to modify the numerical display properties
specified under
Geometrical Tolerance and Datum Target,
available in
expander:
-
Right-click the datum target annotation and select
Properties.
-
In the
Properties dialog box, click the
Numerical Display tab.
-
Under
Numerical Display and
Format, modify the required options.
For more information about numerical display properties defined
in
,
see
Geometrical Tolerance, Datum Target, and Datum System.
The datum target annotations are displayed according to the
modified display properties.
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