The Functional Tolerancing and Annotation (FT&A) workbench is a great way to add 2D drawing information right into the 3D model. Annotation can be added to parts, products, and processes. There are two different workbenches to use depending on what the annotation will be added to. If you are adding annotations to a product be sure to use the product FT&A workbench. These are shown in Figure 1-1.
Figure 1-1
The annotation is added right onto planes that are created within the FT&A workbench, this makes it easy to pull the information and add it into a drawing view. Some scenarios still call for a 2D drawing. There is no need to start a drawing from scratch as the information is right there in the 3D model. There is a way to pull the already created annotation from the 3D model into the 2D drawing.
Open the model that has 3D annotation. Make sure the annotation is turned on as shown in Figure 1-2.
Figure 1-2
Change over to the Generative Drafting workbench as shown in Figure 1-3.
Figure 1-3
From the New Drawing Creation dialog box choose a blank sheet of paper as shown in Figure 1-4. Make sure the FT&A standard that was used matches the drawing standard. If they don’t match you will receive an error message and CATIA will not continue.
Figure 1-4
In the Drafting workbench, find the view toolbar. Select on the Front view flyout. You will find an icon called View From 3D as shown in Figure 1-5. This is the icon that will be used to create the drawing views from the 3D model.
Figure 1-5
In the FT&A workbench designers can create Front views, Section Views, and a Section cuts. In the 3D model none of this matters, it only matters when you pull the views to a 2D drawing. Here are examples of each:
Front View – takes the view from the front face of the model
Front View from 3D Mode Front View from 2D Drawing
Section View – Takes a view from plane location and sections model showing everything behind it.
Section View from 3D Model Section View from 2D Drawing
Section Cut – Takes a view from plane location but only shows in the drawing view what the plane is cutting through. Nothing behind it.
Section Cut from 3D Model Section Cut from 2D Drawing
The model was updated as shown in Figure 1-9. The rectangle cutout was removed from the top.
Figure 1-9
Drawing views will update as shown in Figure 1-10.
Figure 1-10
Now that you understand the difference between the different views, let’s create some. As mentioned earlier, FT&A is added to the 3D model by adding annotation to planes. The way the planes were set up in 3D will correspond to what the drawing view will look like. Our model has 4 different views all in different orientations as shown in Figure 1-11.
Figure 1-11
To create a drawing view, click on the View from 3D icon in the drafting workbench as shown in Figure 1-12:
Figure 1-12
Switch back to the 3D model and select the view from the specification tree as shown in Figure 1-13. In our example, the first one was selected.
Figure 1-13
CATIA will automatically kick you back to the drafting workbench with the drawing view. The drawing view is created based on the selected view and what annotations are on that view as shown in Figure 1-14.
Figure 1-14
Repeat this process for all the annotation planes in the 3D model.
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