Create and modify 3D models > Modify 3D geometry > Modify 3D geometry using dimensions > Create a dimension (3D annotation)
Create a dimension (3D annotation)
Creo Elements/Direct Modeling allows you to create a dimension (3D annotation) without activating the 3D Documentation module.
To create a dimension,
1. Click Feature and then, in the Annotation 3D group, click New.
2. Move the cursor over elements in the viewport. The visual feedback shows appropriate dimensions as you move the cursor over different elements in the viewport. For example, if you move the cursor over a straight edge, the visual feedback shows a linear dimension.
3. Click a reference element in the viewport. If the first element is suitable for a dimension, the visual feedback shows a dimension which moves with the cursor. For a single-reference dimension, continue with step 5. To create a dimension referencing two elements, move the cursor over the second element. An appropriate distance or angle dimension will appear. Select the second element to proceed with that dimension.
4. Move the cursor to position the dimension and click a point in the viewport to create the dimension.
5. Click to complete the operation.
If the first element that you select is a sphere, torus, cylinder, or a circular edge, the visual feedback shows a radial dimension. Depending on the second element that you select, a distance or an angle dimension is created.
If you select a straight edge with parallel faces on both sides as the first element, Creo Elements/Direct Modeling tries to create a linear dimension without selecting a second element. In this case, Creo Elements/Direct Modeling automatically selects the two parallel faces as reference elements.
You can use the Option Mini Toolbar (OMT) (see Using the 2D CoPilot Option Mini Toolbar) to perform the following actions:
Position a dimension on a geometric element (face or edge) instead of using that element as the second reference element.
Choose between radial or diameter type of dimension.
Choose between major and minor dimension when you create a major radius or a minor radius dimension on a torus as shown in the following image (last two options on the right-hand side).
Choose between direct, opposite, adjacent plus, adjacent minus, opposite, and swap angle dimension options as shown in the image below.
You can click Feature and then, in the Annotation 3D group, click Position to dynamically move an existing annotation in different ways. For more details about this implicit repositioning mechanism from 3D Documentation, see Extended Modules > 3D Documentation > Modify 3D documentation > Move annotations in the Help.
You can use this 3D Annotation to modify the geometry of the part. See Modify 3D geometry using dimensions (3D annotations).
Reference elements and reference vertices are highlighted.
You can only select a face or an edge as a reference element. You cannot select a vertex as a reference element.
You can only create a linear dimension between the following elements:
Two parallel plane faces
Two parallel straight edges
A plane face and a straight edge where the face is normal to the edge
A plane face or a straight edge and a cylinder, sphere, torus, or circular edge
Two cylinder faces, sphere faces, torus faces, or circular edges (if the axes are parallel)
If you select a full cylinder or a full circular edge, Creo Elements/Direct Modeling creates a diameter dimension. If not, Creo Elements/Direct Modeling creates a radial dimension.
You can add a 3D Annotation to a read-only part if the assembly that owns the part is writable.