Reference Topics > Change 3D Documentation settings
Change 3D Documentation settings
The 3D Documentation settings define the look of annotations. Labels, reference lines, text, and so on are controlled by a number of parameters. All annotation parameters have default settings that can be changed at any time. In addition, the settings of existing annotations can be changed in the same settings menu.
To change the default annotation settings, click File > Settings > Annotation 3D. The Annotation 3D Settings dialog box opens. Select the type of annotation in the left pane:
GD&T Symbol
Text/Label (including customer feature labels)
Surface Symbol
Welding Symbol
Other Symbol
For the first three types above, many of the parameters are common and described together below.
To change the properties of existing annotations:
1. Click 3D Documentation and then, in the Annotate group, click the arrow next to More.
2. Click Annotation 3D (under Properties). The Annotation 3D Properties dialog box opens.
3. Select one or more annotations in the viewport. The Annotation 3D Properties dialog box shows the properties of the selected annotation.
Adjust the parameters as described below. The additional Chained check box can be used to change the settings of only the individual selected annotation, or the entire chain if that annotation belongs to coordinate or baseline dimensioning.
To change the properties of existing annotations, you can also:
Select the annotation in the viewport and click on the Command Mini Toolbar (CMT).
Select the annotation in the viewport, right-click, and select Annotation 3D Properties from the context menu.
Creo Elements/Direct Annotation parameters
Color sets the color of dimensions using the Color Selector tool.
Frame sets a box, balloon or basic frame (or no frame) to surround the dimension text.
For dimensions in basic frames, the tolerance is automatically set to Basic. If you change a basic frame to any other frame, the tolerance is automatically set to None. You cannot set a frame to Basic in the default Annotation 3D settings.
Display Mode sets the display method for dimension labels: In Plane shows labels in the plane in which they were created; In View shows them always facing the viewport's view, so that they are always readable.
Line parameters
Extension (available only for Dimension settings) sets an offset of the dimension extension lines from the dimension line. The offset value given represents the distance from the dimension line to the end of the extension lines.
Arrow Mode (available only for Dimension settings) sets the arrows to be placed inside or outside the extension lines; or to be determined automatically.
Anchor Pnt sets the anchor position on the label of the reference line. The line can emerge from the upper or lower part of the label, or from its middle.
Arrow Size sets the length of the arrow tip.
1st Type and 2nd Type set the arrowheads for the first and second specified dimension references. The arrow types are assigned in the order the respective references are clicked, or determined automatically by Creo Elements/Direct Modeling when only one point is required.
Filled sets the arrowheads to be solid when the option is switched on, or outlined when switched off.
Text parameters for dimension settings only
Location sets the positioning of the dimension text with respect to the dimension line. The options are to place the text above, below, or on the dimension line.
Space sets the distance between the dimension text and the dimension line. This option has no effect when the dimension text is drawn on the dimension line.
Gap sets the gap between the dimension text and the broken dimension line; that is, the distance between the dimension text and the continuation of the dimension line on either side of it. This setting is only relevant for dimension text located on the dimension line, and is ignored when the text location is above or below the dimension line.
Orientation sets the dimension text orientation to be parallel or perpendicular, relative to the dimension line.
Type sets as "active" one of the six elements of dimension text to be acted on by the following text parameter options. Select one of prefix, postfix, subfix, superfix, tolerance, or the dimension value itself, and then set its Size, Font, and Format.
Format sets the format for numbers in the dimension text (only available for the Dimension and GD&T symbol types).
Text parameters for all annotation settings
Size sets the height of an upper case text character.
Font sets the text font. You can select one of the following:
hp_block_v: Block font with variable character spacing
hp_i3098_v: ISO3098 font with variable character spacing
Miscellaneous settings
Anno Owner By default, an annotation belongs to the Contents information of its owner, but you can optionally choose to save it to the Instance of the owner (except for GD&T symbols which always belong to the contents information). This option is especially important when you attach annotations to shared parts, assemblies or workplanes. Dimensions belonging to one instance of a shared component will not be attached to the other instances. On the other hand, attaching annotations to the contents of the owner means that they will be shared with all instances of the owner. In particular, one advantage of attaching to the instance information is that you can add annotations to read-only parts. The current Owner setting is displayed in dimension creation menus for your information. (Note that this setting is only available as a default setting.)
Centerline: For radius and diameter dimensions, you have the option to include a line passing through the center of the circular object being dimensioned. This general setting determines whether the Centerline switch is on or off when you open a dimension creation dialog box, but you can always change the setting again within the dialog box. (Note that the Centerline setting is only available as a default setting and cannot be changed later.
CustFeat Colors: Specify the colors of GD&T owned by assemblies and invalid GD&T (such as tolerances referring to missing datums). This setting applies also to 3D Notes and all other custom features. The system default colors are purple and red, respectively.
Docuplane Connectors: By default, the lines that extend from the annotation's references to the base of the dimension extension lines on the docuplane ("docuplane connectors") are dimmed (colored gray) in the viewport. However, you can choose not to show them at all by clearing the Show check box. Note that this is a toggle switch on the display of all docuplane connectors, both existing and subsequently created.
Color: You can select a different color from the default gray to use when displaying docuplane connectors. This can be useful to avoid clashing with your Creo Elements/Direct Modeling background color.
Thickness: Click this check box to give 3D annotations thicker, more easily viewable geometry, reference lines, and text.
Surface, Welding, and Other Symbols
Text Color This setting applies to the text within surface, welding and other symbols. Click to check the box, and then select a color other than that defined under Anno Parameters in the Annotation 3D Settings dialog box.
Geo Color Give surface, welding, and other symbol geometry a different color than that defined under Anno Parameters in the Annotation 3D Settings dialog box. Click to check the box, and then select a color.
Predefined values
Grab grabs the settings of an existing dimension and applies them in the Annotation 3D Settings or Annotation 3D Properties dialog boxes. Click Grab in the dialog box, and click a dimension in the viewport. The fields in the dialog box are updated to reflect the parameters of the selected dimension. You can then accept or edit the settings as required.
Default The default settings for 3D annotations can also be applied when you modify existing dimensions. Click Default to adopt these settings.
Format table
The Format dialog box provides the format options for the display of numbers in dimension and tolerance values. You can set the following format aspects:
The number of decimal places: Enter the required number of decimal places in the Decimals box. The default is 2 decimal places.
Zero Suppression:
Click Right on to suppress the decimal zeros at the end of the value; for example, 2.100 or 2.1.
Click Left on to suppress the zero on the left side of the decimal point; for example, 0.25 or .25.
Decimal Punctuation: Click either Point or Comma to specify the type of decimal punctuation.
Click Reset to restore the settings of a single category, selected categories, or all categories of options to the Site, Corp, or Factory default settings. The Reset Annotation 3D Settings dialog box opens. The current category is selected by default when you click Reset.