In a single dialog box, you can create both "generic" dimensions and GD&T dimensions. The GD&T type of dimensions follow the built-in "advisor" rules and checks, and use the Creo Elements/Direct Modeling custom feature structure. Generic dimensions are not features, but straightforward annotations of your model.
The basic process to create dimensions is the same in both cases, and done in the same dialog box. Creating dimensions is outlined below:
1. Select the type of dimension to be created; Generic (non-GD&T) or GD&T dimensions.
2. Specify the dimension's references, which can be faces, edges, vertices or features. When you click a reference, the selection catches to the nearest vertex, but you can also catch to the center of a circular loop, or to the near or far tangent of a loop (to create tangential dimensioning). Reference points can be changed while the current dimension remains active.
3. Click a position for the dimension label. After placing the dimension label, you can click it to activate it and move it again. You can also click a different label to move it.
4. Specify whether the dimension should be measured with respect to a docuplane or be free.
5. Specify other information for the dimension, such as tolerance values and text fixes.
When you modify the referenced geometry of a dimension, the system automatically updates the dimension value and the position of the dimension label. You can also change the references themselves while creating dimensions, and also on existing dimensions.
If you are using the Creo Elements/Direct Annotation module, you can transfer 3D Dimensions to your drawing.
GD&T dimensions are also types of design information features, therefore you can report, highlight, or show them as described in the following sections.
The elements of dimensioning
Depending on the options you choose, dimensions can consist of the following elements:
Dimension text
Dimension value:
The numerical value assigned to the geometry element which specifies a distance, angle, radius, or diameter. The value can be imperial, metric, or angular, depending on the current units setting.
Tolerance:
Information about the tolerance allowed in the dimension value. This could be a basic tolerance, general tolerance, a plus and minus tolerance (for example, 80 +/-0.25), an upper and lower tolerance (for example, 80 +0.25/-0.5), or a limit tolerance (for example, 80.5/79.6).
Prefix:
Any additional information before the dimension value. Examples are "max." and "min.".
Postfix:
Any additional information after the dimension value. Examples are "equally spaced" or "concentric".
Subfix:
Any additional information below the dimension value.
Superfix:
Any additional information above the dimension value.
Dimension geometry
Dimension lines:
Lines with arrows which show the direction and extent of a dimension. The size and type of the arrow can be adjusted.
Extension lines:
Lines which extend from the geometry elements to the ends of the dimension line.
Docuplane connectors:
Lines which extend from the dimension references to the base of the extension lines when the dimension is placed on a docuplane.
Frame:
An optional box or balloon that surrounds the dimension text.
Index:
A numerical reference used to catalog the dimension.
A note on ownership of 3D dimensions
You create a dimension by clicking references on parts or profile geometry. You can choose to attach the new dimension to a docuplane, a defined plane in 3D similar to a workplane, used for organizing 3D annos; otherwise you can create a free dimension. The owner of a docuplane, if specified, becomes the owner of the new dimension.
In the case of free generic dimensions, Creo Elements/Direct Modeling automatically selects the owner of the dimension based on the context implied by the references. In particular, references specified on one part produce a dimension belonging to that part. If you attach a dimension to two parts within an assembly, the assembly is selected as owner.
For free GD&T dimensions, however, you must first specify the owning assembly to attach a dimension to it. The datum the dimension refers to must also belong to this assembly.
You can also attach dimensions to profile geometry in a single workplane or between workplanes in a workplane set. In all cases, Creo Elements/Direct Modeling selects the lowest possible owner in the implied context; however, you can always change the automatically-selected owner to any other higher-level owner (such as a higher assembly).
When you save a part, assembly, or workplane, 3D Dimensions are saved with it. When loading the item all dimension values are recalculated using the current system units.