The Model-Based Definition (MBD), which deals with the definition of products through annotated 3D CAD models rather than traditional 2D drawings, is supported in CATIA by the Functional Tolerancing and Annotation (FT&A) workbench. The FT&A workbench enables the designers to embed the 3D Annotations, such as dimensions, GD&T symbols, etc., directly into CATIA 3D models, providing the ‘single source of truth’ for the manufacturing engineers and machinists.
Many large enterprises across the globe have adopted the MBD approach, so they no longer send 2D drawings to their suppliers. This presents a challenge for the suppliers, which is the ability to open and read the manufacturing information provided by their OEMs.
One obvious solution for the supplier would be to purchase CATIA software and use it to open and read the native CATIA models, including 3D Annotations. The problem for the smaller machine shops, however, could be the software cost.
Fortunately, there is another solution to this problem, which is using a neutral format such as STEP for data exchange. The STEP format has been around since 1994, but things have changed considerably with the advent of the STEP 242 protocol, which offers dedicated MBD support.
In this blog post, I will explain how to export CATIA’s 3D Annotations to a STEP file using the 242 protocol.
First, the pre-requisite is that you must have a proper license to be able to export, which is the SXT (Extended STEP Interface) add-on product. Having the ST1 (STEP Core Interface) license, included in most CATIA configurations, is not enough. Also note that the FTA (3D Functional Tolerancing & Annotation) license is not necessary. As you see below, I will be using the basic MD2 configuration along with the SXT license in my examples.
Second, you must activate some settings. Go to Tools > Options > Compatibility > STEP, activate the 3D annotations toggle, and select 242 ed1 in the Application Protocol pull-down list, as shown below.
Now let’s see how the export works for the part shown below.
Select File > Save As and select stp (*.stp) in the Save as type pull-down list. Click Save to save the STEP file.
Now open the saved STEP file in CATIA, as shown below. As you can see, the annotations came through just fine.
Note that the exported annotations are stored in the Annotation Set Result.1, which means they are not editable and cannot be deleted. However, the result annotations can be hidden if desired.
Things become a little trickier if you want to export an assembly with annotations, rather than a single part. As an example, let’s see how the export works on the product shown below, in which we have annotations on the product level as well as on the part level.
The export result is shown below. As you see, no annotations came through.
Turns out CATIA’s annotation export to STEP has some limitations, one of those being that the annotations on the product level cannot be exported. Specifically, this is what CATIA documentation says.
But what about annotations on the part level? To export those, you need to activate yet another option in the Tools > Options > Compatibility > STEP, which is Global nested assembly, instead of the default One STEP file.
Now the exported to STEP assembly opens as shown below. As you can see, the annotations on the part level have come through just fine.
The use of MBD and 3D Annotations is covered in the Rand 3D class: CATIA Functional Tolerancing & Annotation.
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