|
This task shows how to re-define a complex
edge into a cylindrical surface and apply a size tolerance to the previous
redefined geometry. |
|
Re-specifying geometry canonicity offers to
re-define user surface or group of surface properties to avoid recognition
problem when selecting a geometry. You can re-define the geometry through an
existing annotation only. |
|
Open the
Tolerancing_Annotations_07 CATPart document. |
|
-
Click the Tolerancing Advisor icon:
-
Select the complex edge as shown on the part.
|
The Semantic Tolerancing Advisor dialog box appears.
Note that no command related to a cylindrical surface is displayed. |
|
-
Click the Text with Leader icon (One surface):
-
Enter Hole in the Text Editor dialog box field
when appears.
-
Click OK in the Text Editor dialog
box and Close in the Semantic Tolerancing Advisor
dialog box.
-
Right-click the annotation as shown on the part and select
the Associated Geometry > Geometry Canonicity Query and
Redefinition from the contextual menu.
|
The Canonicity Redefinition dialog box appears. |
|
-
Select the Redefined by geometry option.
-
Select the yellow axis line on the part associated with
the cylindrical surface definition.
|
The Canonicity Redefinition dialog box is updated.
You can create the axis straightness attribute to the geometry using
this option, but cannot change the feature size. |
-
Select the
Redefined by
mathematical definition option.
This option lets you create spherical and cylindrical attributes.
Select the Feature of Size option, the Size
field is now enabled and set its value to 20mm and click OK.
Click the Tolerancing Advisor icon:
,
the annotation is still selected.
The Semantic Tolerancing Advisor dialog box displays
now command related to a cylindrical surface. |
|
-
Click the Diameter icon (One surface):
-
Click OK in the Limit of Size Definition
dialog box when appears.
The diameter dimension annotation is created. |
|
-
Click Close in the Semantic Tolerancing
Advisor dialog box.
|