Extended modules > 3D Documenation > Create 3D dimension labels > Create distance dimensions
  
Create distance dimensions
Distance dimensions show the linear distance between two referenced elements. With faces (or edges) as reference elements, the extension line originates in the vertex nearest to the point you click. This vertex defines the reference position.
The figure below shows an example of distance dimensions.
When creating a distance dimension, it is important which of the two reference elements you click first. The order defines the measure direction. For free dimensions, it defines also the display plane which passes through the reference position of the first reference element. You can also specify a docuplane that implies a defined measure direction, if it is valid for the dimension. You can reposition a dimension label only within its display plane or docuplane.
The figure below gives an example of two different results owing to different measure directions.
The measure direction for distance dimensions is basically defined by the following rules:
If both reference elements are plane faces, the measure direction will be normal to the face you click first.
If only one of the reference elements is a plane face, the measure direction will be normal to this face.
If both reference elements are vertices, the measure direction will be direct between these vertices.
You can also specify a docuplane that implies a defined measure direction, if it is valid for the dimension. In all cases Creo Elements/Direct Modeling offers you the option to specify a docuplane that implies a defined measure direction.
You can add dimensions measuring distances to a part, to multiple parts within an assembly, and to profiles; all the while controlling the measure direction of the dimension.
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The measure direction and the docuplane of the dimension must remain parallel.
To create a distance dimension,
1. Click 3D Documentation and then, in the Annotate group, click Linear. The Create Distance Dim dialog box opens.
2. If necessary, specify whether you want to create a Generic dimension or GD&T by clicking the appropriate tab.
3. Select the first reference for the dimension:
Generic: Click the reference in the viewport.
GD&T: Select the faces or features to control.
4. If necessary, click Catch repeatedly to change the catch focus of the selected reference, or select the focus directly in the box. This option is available when there is a choice of catch points; for example, on circular edges, you can choose to catch to the near or far tangent, the center of the edge, or at its vertex. You can also select Vertex from the Catch list, even if it is the only option, to activate the selection of a different vertex on the reference face.
5. Define the second reference point as above; or, for GD&T, specify the datum. The selected references are highlighted, the extension lines of the dimension label snap to the selected vertices, and the dimension label becomes attached to the cursor. Note that the dimension value is displayed in the Dim Value box, which updates dynamically as you alter the current dimension.
6. Specify the measure direction and placement of the dimension:
To create a free dimension, select Free under Orientation/Placement, and click a position for the dimension label. The plane of the dimension is determined by its reference points.
To place the dimension on a docuplane, click Docuplane and specify the docuplane to use (double-click it in the browser, or click it in the viewport). The active docuplane, if present, is selected by default.
After placing the dimension label, you can click it or any other label to move it and click another position. This is allows you to organize labels "on the fly".
7. The measure direction is determined automatically, but you can change this if necessary:
The default option, auto, automatically selects the direction as normal to the first selected reference element.
To specify a different direction, click User def and specify the measure direction with the Direction 3D tool.
When placing the dimension on a docuplane, you can also specify whether the direction between the two points should measured as horizontal or vertical, with respect to the selected docuplane.
8. If necessary, you can add tolerancing information to the dimension.
9. You can include a prefix, postfix, subfix, or superfix with the dimension value by expanding the Text fixes area and entering text into the appropriate boxes.
10. You can use predefined tolerances and/or text fixes in two ways:
Presets: Click this to open a table containing values that were stored earlier.
Grab: Click this and then click an existing dimension in the viewport. The tolerance and text fixes of the selected dimension are copied into the menu and used for the current dimension.
11. If you are creating a GD&T dimension, you must also specify a Name for it. Optionally, you can also include a Descr, dimension critical Identifiers, or Insp. Notes. These will be shown in feature reports.
12. You can add a URL to a dimension text, which can be any file on your local computer, network, or the public Internet. The file will open in its default viewer when you right-click the dimension, then click Display URL.
13. You can end the current dimension in one of two ways:
Click Next to complete the current dimension and continue creating new dimensions with the same tolerance and text fixes.
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You can avoid clicking Next; once the current dimension is complete, simply click new references on the model to define a new dimension. The system will automatically make this the current dimension using the current settings.
Click Reset to cancel the current dimension but keep the menu open with the same tolerance and text fixes.
14. When you are finished creating dimensions, click to complete the operation.