Create drawings from models (Creo Elements/Direct Annotation) > Modify drawings > Add and modify symbols > Create a symbol
  
Create a symbol
Creo Elements/Direct Annotation provides the following types of symbols:
GD & T
The orientation and position of the datum symbols and their reference lines, if drawn, depend on the drawing elements to which they are attached.
The datum targets in particular denote specific points, lines, or areas on a view that are used in establishing a datum reference frame.
The GD & T menu contains the tolerance symbols. You can add modifiers and datums to tolerance symbols to build up geometric tolerance groups.
GD & T symbols are contained in the hp_symbols2 font (which has the filename hp_symbols2.fnt). When you add these symbols to a drawing, Creo Elements/Direct Annotation uses this font.
Datum
Datum target
Datum target area
Datum target point
Tolerance
Surface
Welding
User defined
Each of these is created in a separate menu.
To create a symbol,
1. Click Annotation and then, in the Annotate group, click the arrow next to Symbol.
2. Click Create Symbol.
3. Double-click the desired symbol in the Template Browser or select an existing symbol on the sheet. The dialog box for that symbol appears, displaying the default values, and the symbol appears on the cursor when it is placed in the Creo Elements/Direct Annotation viewport.
4. If needed, click Owner and specify the owner of the symbol.
5. Position the symbol in the viewport.
You can drag the symbol to a new position at any time.
6. Complete the operation as described below.
To specify symbol parameters,
1. Choose among the following:
For a Datum symbol, enter a datum text for the symbol in the Datum box.
For a Datum Target symbol, enter a name in the Name box, and/or enter a value in the Value box. To add a diameter symbol (Ø) to the specified value, click the Ø switch on.
For a Datum Target Area symbol, enter a radius for the target area symbol in the Radius box.
For a GD & T tolerance symbol, specify the following parameters:
Tolerance
Select the type of tolerance symbol.
Composite
Toggle between normal and composite symbol. Normal symbols are as high as one line of text, whereas composite symbols are the height of two lines of text. This form allows you to create two lines of tolerance information (see below).
Proj Dist
Click on and enter the distance for a projected tolerance.
Shape
Select the shape for the tolerance zone.
Value
Type the tolerance value.
Modifier
Select a modifier symbol for the tolerance value.
Modifier Add
Select an additional modifier symbol for the tolerance value.
Datums
Type or select the Primary, Secondary, and Tertiary datums, and select a modifier symbol for each. To specify multiple datum references and modifiers, click Primary, Secondary or Tertiary. The TextEditor window opens. Type the datum reference characters and type or select modifiers. If modifiers are typed or selected then the Modifier parameter disables for the respective datum.
When Composite is switched on, click Switch to 2nd Line to edit the second line of the symbol. The GD&T menu contracts to show only the fields for the 2nd Tolerance Zone and Datums for the second line. To return to the first line, click Switch to 1st Line.
You can also create a multiple-tier tolerance symbol:
Click Insert in the Parameters section to add another tier to the symbol. Click and to switch tiers. Click Delete to remove a tier.
For a Surface symbol,
Two versions of the surface symbol are available in the Template Browser: Surface (1992) and Surface (2002). Double-click any one symbol in the Template Browser and specify the following parameters in the Surface task panel:
Form
Select the surface symbol form.
Unit of Proposal
Select the unit of proposal. This determines which sets of predefined parameters appear in some menus below.
Upper Val a1
Enter the upper roughness value.
* 
The position of Upper Val a1 is different in Surface (1992) and Surface (2002) versions.
Lower Val a2
Enter the lower roughness value.
* 
The position of Lower Val a2 is different in Surface (1992) and Surface (2002) versions.
Process b
Enter the manufacturing process code.
Cov Length c
Enter the covered length.
* 
Specify Cov Length c only in the Surface (1992) version. This parameter is not available in the Surface (2002) version.
Measure f
Enter another roughness measure.
* 
Specify Measure f only in the Surface (1992) version. This parameter is not available in the Surface (2002) version.
Allowance e
Enter the machining allowance.
Groove Dir d
Specify the groove direction.
Standard
Specify the surface symbol version 1992 or 2002.
Depending on the default Standard setting, you can select any one or both the surface symbol versions. See Set default symbol parameters. If the default Standard setting is All, you can change any symbol to the other version. However,
If the default setting is ISO 1302 - 1992, show only, you can only change a Surface (2002) symbol to Surface (1992).
If the default setting is ISO 1302 - 2002, show only, you can only change a Surface (1992) symbol to Surface (2002).
Note that the horizontal bar of the symbol is not drawn if none of the b, c, and f values is given for the Surface (1992) version.
For a Welding symbol,
Specify the following parameters:
Shape
Select the type of welding symbol.
Position
Select the orientation of the symbol.
Geo Var
Toggle the menu to display the geometric variable fields g1 to g7. Select the required geometry elements from the cascade lists. The elements comply with the DIN 18800-1 standard.
Text Var
Toggle the menu to display the text variable fields t1 to t7. Enter the required values in the data entry fields.
If you are modifying a welding symbol, you can click Swap Side to exchange parameters between the arrow side and other side of the welding symbol.
2. Under Appearance, at any time during creation of the text, you may specify various attributes. Most of these settings are intuitive, but it may be helpful to know:
Style:
Select Default (no Style), Datum Target, or Surface.
* 
Because Surface and Datum Target symbols have settings that other symbols do not, Creo Elements/Direct Annotation does not use the default style specified in the Default Settings Table for these symbols.
Angle:
Specifies the angle between the text base line and the horizontal.
If you set the value of the angle to Auto, Creo Elements/Direct Annotation will use the angle of the selected element to set the angle of the symbol. The Get Angle button will change to Flip Symbol so you can position the symbol on the other side of the element.
Size:
Whether the size of the symbol is relative
Ratio:
The ratio of character width to height.
Slant:
The deviation from vertical of the characters in the text; values must be between -80 and +80 degrees (approximately ±1.39 rad or ±88.88 grad).
3. You may change any parameters for the symbol until you click Position Next Symbol or OK.
4. To add another symbol, click Position Next Symbol, specify its position, and edit as required.
5. Click to complete the operation.
The Ref Line button is active when the owner of the symbol is a valid reference line owner (a view or a sketch). Click it to open the Create Ref Line dialog box and draw a reference line from the current symbol to a target element in the drawing.
Limitations
Creo Elements/Direct Modeling splits multiple-tier GD&T symbols into separate symbols when you save your drawing to a format older than 2008.