Dimensioning gives you the means to describe elements of your drawings in detail, providing valuable additional information about your model.
To create a dimension,
1. Click Annotation and then, in the Annotate group, click the arrow next to Linear or Circular. You can also click Angular in the Annotate group.
2. Click the appropriate linear or circular dimension
Dimension types under Linear or Circular respectively. The respective dialog box for the linear, circular, or angular dimension opens.
3. Enter the following as necessary:
◦ For diameter
To dimension circular geometry where a tangential span exists and has unique center point, click Tangential Mode on the Diameter Dim dialog box.
◦ For radius and diameter
To pass the radius line through the element's center, click Centerline on the Radius Dimension or Diameter Dim dialog box.
◦ For tangent
To dimension a circle, arc, fillet, ellipse, or a B-spline (closed, both interpolation and control), click Tangential, right-click the viewport and select the required orientation for the dimension from the context menu.
Extremum
This option dimensions between the extremum points of the circular elements; it measures the longest or shortest possible distance, whichever is applicable. (This is the default option.)
Inclined
This option allows you to orient the dimension at an angle to its extremum position. Creo Elements/Direct Annotation converts any value of the specified angle between 360 and -360 degrees.
Horizontal
This option allows you to orient the dimension in horizontal plane.
Vertical
This option allows you to orient the dimension in vertical plane.
Parallel to
This option allows you to orient the dimension parallel to a reference line on your drawing.
Perpendicular to
This option allows you to orient the dimension perpendicular to a reference line on your drawing.
• Extremum and Inclined are not available in Tangential Mode under Diameter.
• Tangential dimensions are not possible for open B-splines.
Creo Elements/Direct Annotation always chooses the extreme tangent points of a closed B-spline which has more than two tangent points at the specified angle. If you select the points on a closed B-spline and a circle, arc, line, fillet or an ellipse, Creo Elements/Direct Annotation automatically chooses the tangent point which is closest to the selected point on that B-spline.
4. If required, type a Prefix, Basic prefix, Postfix, Basic postfix, Subfix, or Superfix. Thread dimension properties are shown as keywords in the Prefix and Postfix fields.
Basic prefix and Basic postfix are available only if you select a basic tolerance.
5. If required, select a type of tolerance from the Tol Type box and type tolerance values.
6. Click + or - under Decimal Places to increase or decrease the number of decimal places. Click the middle button to return to the default number of decimal places.
7. Click the begin point for the dimensioning (or use box selection). For all types of dimensioning, you can specify a number of dimension points at the same time by drawing a selection box around them. Creo Elements/Direct Annotation determines the possible dimension points and creates the dimensioning automatically. Unless automatic placement mode is enabled, you then click the position for all dimension texts en masse. It is likely that some of the dimensions will need to be adjusted.
For some dimensioning (such as single dimensions) you can specify a selection box from the start; but for others (such as datum dimensions) you must click the first point before drawing a box.
When creating dimensions by box selection, the dimension reference elements cannot be re-selected during dimension creation.
◦ for angle dimensions, click one side of the angle.
◦ for tangential dimensions, click geometry where a tangential span exists.
◦ for a chamfer, click a chamfered edge.
8. Enter the following as necessary:
◦ For a single dimension
Click the end point.
◦ For a chained dimension
Click the first chain dimension point. Continue clicking chain dimension points and clicking the text positions as required. At any time while creating a chain dimension, you can undo the previously specified dimension point. Right-click and click Back to remove the last point, and then continue as normal.
◦ For a symmetry dimension
1. If you clicked Sym Single, click the end point. The dimension reference elements stay highlighted until you create the next dimension.
2. If you clicked Sym Long, click the first symmetric datum point. The dimension reference elements stay highlighted until you create the next dimension. At any time while creating symmetry long dimensions, you can undo the previously specified dimension point. Right-click and click Back to remove the last point, and then continue as normal.
◦ For a datum dimension
Continue clicking datum dimension points and clicking the text positions as required. At any time while creating datum dimensioning, you can undo the previously specified dimension point. Right-click and click Back to remove the last point, and then continue as normal.
◦ For an angle dimension
Click the other side of the angle. If you have clicked the angle references in the wrong order, click Swap to take the angle that would arise if the two sides had been clicked in the opposite order.
◦ For a circular dimension
1. If you clicked Radius or Diameter, click a circle, arc, or fillet.
2. If you clicked Arc, click the Length or the Angle check box to dimension the length or the angle of the arc. Click the two end points on an arc.
Right-click the viewport, select Length or Angle dimension from the context menu.
The order in which you select the endpoints determines whether the major or minor arc is dimensioned:
Clicking clockwise along the arc measures the major arc.
Clicking counterclockwise along the arc measures the minor arc.
9. Under Appearance, at any time during creation of the dimension, you may specify various attributes. Most of these settings are intuitive, but it may be helpful to know:
Style:
Select a style to apply to the dimension.
Color:
Specify the color for the dimension.
Font:
Select the font for the dimension.
Fill:
Specify whether block fonts or arrows should be filled.
Frame:
Select the dimension frame.
Arrow Appearance
For dimensions that have two lines, you can specify the 1st arrow type for one end of the line that connects them and a 2nd arrow type for the other end.
1st Type:
Radius and Chamfer dimensions have only the 1st Type box.
2nd Type:
Sym Single and Coordinate dimensions have only the 2nd Type box.
10. Click the position for the dimension text. A box representing the text follows the cursor until you specify the position.
11. Continue adding dimensioning to the drawing, or click to complete the operation.
When you create a new thread dimension, change the pitch in Creo Elements/Direct Modeling, and update the view in Creo Elements/Direct Annotation, the dimension also updates accordingly.
If you have an old thread dimension, this update will not occur. After an update all user data in old thread dimensions are lost. You must use the
Convert thread dimensions command to change the thread dimension.
Linear or 
Circular. You can also click 
Angular in the Annotate group.
to complete the operation.