Extended modules > 3D Documenation > Create 3D dimension labels > Create coordinate and baseline dimensions
  
Create coordinate and baseline dimensions
Coordinate dimensioning creates a series of "chained" dimensions having a common origin and single dimension line. Baseline dimensioning creates dimensions from a common origin using long or short baselines, and where the dimension labels are on unique but parallel dimension lines.
The figures below shows an example of coordinate and baseline dimensions:
Coordinate Dimension
Short and Long Baseline Dimension
Coordinate and baseline dimensioning is useful to mark holes and other features on a part. Normally, design engineers use this type of dimensioning for parts that will be NC-machined.
To insert further dimensions into an existing coordinate or baseline dimension chain, simply click an existing dimension of the chain as the first reference. The chain's settings are displayed in the menu, and you can click further references as required.
To create a coordinate or baseline dimension,
1. Click 3D Documentation and then, in the Annotate group, click Coordinate or Datum Long. The Create Coordinate Dim or Create Baseline 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. For baseline dimensions, specify if you want Long or Short baselines.
4. Select the origin for the dimension:
Generic: Click the reference in the viewport.
GD&T: Select the datum reference.
5. If necessary, click Catch repeatedly to change the catch focus of the selected reference, or select the focus directly from the list. This option is available when there is a choice of catch points; for example, on circular edges, you can choose to catch to the center of the edge or at its vertex. You can also select Vertex in the Catch box, even if it is the only option, to activate the selection of a different vertex on the reference face.
6. Define the second reference point as above. The selected references are highlighted, the extension lines of the dimension label snap to the nearest vertices of the selected references, 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.
7. 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".
8. Continue clicking references comprising the dimension chain. The dimension labels are placed automatically, parallel to the position of the first label.
9. The measure direction of the chain is determined automatically, but you can change this if necessary at any time during the creation of the dimensions:
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.
10. If necessary, you can add tolerancing information to the dimension.
11. 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.
12. 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 dialog box and used for the current dimension.
13. 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.
14. 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.
15. You can end the current dimension chain in one of two ways:
Click Next to complete the current dimension chain and continue creating new chains with the same tolerance and text fixes.
Click Reset to cancel the current dimension chain but keep the menu open with the same tolerance and text fixes.
16. When you are finished creating the dimension chain, click to complete the operation.
Before you have specified three references of the dimension chain, you can still change its origin by clicking Datum and clicking new reference geometry. In the same way, you can always change the previously placed reference by clicking Element and specifying a new reference.