Creating an FD&T View

This task shows how to generate a view and the associated annotations from the 3D (Functional Dimensioning and Tolerancing workbench).

An FD&T view is a view that is extracted from a 3D part that is assigned 3D tolerance specifications and annotations.

Before You Begin, make sure you customized the following settings:

Grid:
De-activate the Grid icon from the Tools toolbar (bottom right).

View names and scaling factors:
Go to Tools->Options->Mechanical Design -> Drafting(Layout tab) and check the View name and Scaling factor options.

3D colors inheritance
Go to Tools->Options->Mechanical Design->Drafting option (Generation tab) and un-check the 3D colors inheritance option.

Open the GenDrafting_part_FDT.CATPart document.

Before You Begin:

Tile the screen horizontally:
Select Window -> Tile Horizontally option from the menu bar.

In addition: make sure the standard used in the CATDrawing document and in the CATPart (annotations) is the same. Otherwise, both the view and the annotation will not be possibly generated.

Go to Tools -> Customize... menu bar options (Commands tab) and select the Hide/Show 3D Annotations command. Then, press the CLOSE switch button. The Hide/Show 3D Annotations command automatically appears in the workbench. Make sure it is active.OR
Go to Start -> Mechanical Design -> Functional Dimensioning and Tolerancing (menubar) and activate the Hide/Show 3D Annotations command.

1. Click the View From 3D icon

from the Views toolbar (Projections subtoolbar).

2. Select a view from the 3D, either in the specification tree or on the part. In this case, select the third Front View in the specification tree.

The view to be created is previewed (included annotations) on the drawing. You cannot modify the view orientation.

3. Click on the drawing to create the new view.

	The annotations can be moved or modified. They are not associative to the geometry (except if you key in "`c: Force Update`", in which case, the view is updated and all the modifications possibly applied to the annotations are lost). We advise you perform modification on the 3D part.
	When you created a section cut in the 3D instead of clicking on the drawing to generate the view, you can click on another view in which the callout will be positioned.
	If you go to `Tools -> Customize...` menu bar options (`Commands` tab) and select the `Unable/Disable 3D Annotation queries` command, press the `CLOSE` switch button and make sure the `Unable/Disable 3D Annotation queries`command is active, whenever you will select an annotation, the surface this annotation is linked to will highlight. Note you can also go to `Start -> Mechanical Design -> Functional Dimensioning and Tolerancing` (menu bar) and activate the `Unable/Disable 3D Annotation queries`command.
	FD&T views cannot not be rotated. In other words, when you edit the properties of this view (`Edit -> Properties`), the `Angle` field is set to the gray color.