No matter how polished your 3D model is, getting it manufactured and assembled on the shop floor always comes back to one thing: a 2D drawing. CATIA’s Drafting workbench is fully associative with your 3D model — it automatically generates orthographic views, section views, and detail views, and lets you add dimensions and annotations on top of them.
“Get your Front View right, and the rest — projections, sections, details — practically build themselves.”
This article walks through everything you need to know for real-world use: entering the Drafting workbench, creating drawing views, adding dimensions, setting up the title block, and auto-generating a BOM.
1. Entering the Drafting Workbench
- Open the 3D part (.CATPart) or assembly (.CATProduct) file you want to draw. Make sure the 3D objects are in Design Mode (green icon in the spec tree). If any components are in CGR mode (blue/grey icon), CATIA won’t be able to recognize their geometry when generating views.
- Go to Start > Mechanical Design > Drafting.
- In the “New Drawing” dialog, select your Drawing Standard and sheet size (Sheet Style), then click OK.
The Drawing Standard isn’t just about projection direction. It defines every visual rule on your drawing — dimension text size, arrowhead style, line weights, linetypes, hatch patterns, and more — all at once.
If you try to switch standards after you’ve already placed views and dimensions, everything breaks. You’ll likely need to start from scratch. Lock in the standard before you do anything else.
2. Creating Drawing Views — Orthographic, Section, and Detail
Creating a drawing view in Drafting is fundamentally about deciding which face of the 3D model to show, and from which angle.
| View Type | Command | Description |
|---|---|---|
| Front View | Front View | The primary view everything else is based on. Click the icon, select a reference face or plane on the 3D model, and it projects onto the sheet automatically. You can fine-tune the angle using the compass. |
| Projection View | Projection View | Move your cursor up, down, left, or right from the Front View to automatically generate a top, bottom, or side view. Once the Front View is set correctly, these take just a few clicks. |
| Section View | Offset Section View | Draw a cut line across an existing view and a cross-section is generated automatically along that cut. Essential for showing internal geometry — holes, pockets, bores. |
| Detail View | Detail View | Draw a circle around a small area on an existing view, and CATIA generates an enlarged close-up of that area as a separate view. Ideal for small fillets, threads, tapped holes, and other fine features. |
| Isometric View | Isometric View | A 3D-looking axonometric view placed on the 2D drawing. Often used as a supplementary view to help readers quickly understand the overall shape. |
Where Projection Views land on your sheet depends on which projection method is active — First Angle (ISO/European) or Third Angle (ANSI/American). For example, in Third Angle projection, moving the cursor to the right of the Front View gives you the Right Side View. In First Angle, it gives you the Left Side View instead.
You can change the projection method after creating the sheet via sheet Properties, but it must be set before placing any views.
① Place the Front View → ② Use Projection View to generate the top and side views → ③ Add Section Views for internal geometry → ④ Add Detail Views for fine features.
All other views are linked to the Front View, so getting the Front View orientation right from the start is the most critical step. As a general rule, choose the face that best communicates the overall shape of the part or assembly.
3. Adding Dimensions
Once your views are placed, you need to dimension the drawing so the part can actually be manufactured.
| Dimension Type | How to Use |
|---|---|
| Linear | Click the Dimensions icon → click two lines or two points in sequence → position the dimension line where you want it. |
| Radius | Click an arc — CATIA automatically creates a radius dimension with the standard R notation. |
| Diameter | Click a circle — CATIA automatically creates a diameter dimension with the standard ⌀ notation. Clicking a cylindrical bore in a section view also works. |
| Angle | Click two straight lines in sequence, and CATIA generates the angle between them automatically. |
Right-click any dimension → Properties to adjust text height, arrowhead style, tolerance values, and more. Since every company has its own drawing standards, setting up a consistent style at the start will save you a lot of rework later.
Drawing standard management: Tools > Standards (ISO, ANSI, JIS, etc.)
⚠️ To edit and save standards in that menu, CATIA must be running in Admin Mode. In normal mode, you can view the settings but cannot modify them.
How to launch Admin Mode:
Right-click the CATIA shortcut → Properties. In the “Target” field, you’ll see the launch path ending in something like:
… \intel_a\code\bin\CNEXT.exe
Add a space and -admin after CNEXT.exe:
… \intel_a\code\bin\CNEXT.exe -admin
Click OK, then launch CATIA using that shortcut. When Admin Mode is active, you’ll see “Administrator Mode” displayed in the menu bar.
4. Drawing Frame & Title Block
Here’s how to add the drawing border (frame) and title block — the area that holds your company name, drawing number, author, date, scale, and revision info.
- Go to Edit > Sheet Background to enter background editing mode. The sheet color will change to indicate you’re now editing the background layer.
- Select Insert > Drawing > Frame and Title Block.
- In the “Manage Frame and Title Block” dialog, choose a style and click Create.
- Double-click any text field in the title block to type in your company name, drawing number, author, and other details.
- When done, go to Edit > Working Views to return to normal drawing mode.
The built-in CATIA title blocks are a starting point at best. In real production environments, every company maintains its own .CATDrawing template file with the company-standard border and title block already in place. Set it up once, and from then on, every new drawing starts from a copy of that template — just open it, place your views, and you’re done. The time savings add up fast.
5. Exporting to PDF
Getting your finished drawing out as a PDF is straightforward.
- Go to File > Print.
- Select a PDF printer (e.g., Microsoft Print to PDF) from the printer list.
- Confirm the paper size (A3, A4, etc.) and orientation, then print.
Alternatively, use File > Save As and set the file type to PDF (.pdf) to save directly without going through the print dialog.
6. Balloons & Bill of Materials (BOM)
When working with an assembly (.CATProduct) drawing, you can attach numbered balloons to each component and auto-generate a full Bill of Materials table.
▶ Step 1: Assign item numbers in the assembly
- In the assembly file, switch to the Product Structure workbench and run Generate Numbering to assign instance numbers to each component.
- These numbers will become the item numbers in your Balloons and BOM table.
▶ Step 2: Place balloons
- Activate the assembly view in Drafting.
- Go to Insert > Generation > Generate Balloons.
- Balloons are placed automatically on every component visible in the view.
- Drag any overlapping or awkwardly placed balloons to reposition them. Adjust font size via Properties.
▶ Step 3: Insert the BOM table
- Go to Insert > Generation > Bill Of Material.
- Click on the sheet to place the BOM table.
- Component data (names, quantities, etc.) from the assembly is populated automatically.
CATIA’s BOM is parametric and fully associative. Add or remove a component in the assembly, and the BOM table and balloons on the drawing update automatically.
You can also open Analyze > Bill of Material and export the list to Excel — handy for generating a purchase order parts list without any manual data entry.
To change the numbering order:
Generate Numbering assigns numbers based on the spec tree order. Reorder the components in the spec tree, then re-run Generate Numbering to reassign. Some versions have a Graph Tree Reordering function in the Product Structure Tools toolbar.
To exclude a component from the BOM and balloons:
Deactivate the component in the assembly — it will be automatically removed from both the BOM and any generated balloons. You can also manually delete individual balloons after generation.
To see which item number corresponds to which part in 3D:
Open Analyze > Bill of Material → click Define formats → find “Number” in the Hidden properties list and move it to Displayed properties → click OK → click Refresh. The item number column will then appear in the BOM. You can add any other properties the same way.
Drafting Commands at a Glance
| Function | Command / Path | Summary |
|---|---|---|
| Front View | Front View | Select a 3D face → auto-projected to 2D |
| Projection View | Projection View | Auto-generates top / side views from the Front View |
| Section View | Offset Section View | Draw a cut line → cross-section generated automatically |
| Detail View | Detail View | Circle a region → enlarged close-up view |
| Dimensioning | Dimensions | Click geometry → auto-recognizes linear, R, ⌀, or angle |
| Drawing Frame & Title Block | Insert > Frame and Title Block | Insert and edit in Sheet Background mode |
| Balloons | Insert > Generation > Generate Balloons | Auto-places item number balloons on assembly view |
| Bill of Materials | Insert > Generation > Bill Of Material | Auto-generates parts list; exportable to Excel |
Wrap-Up
The biggest advantage of CATIA Drafting is that it’s fully associative with the 3D model. Change the geometry in 3D, and your drawing views and dimensions update automatically — no risk of the drawing falling out of sync with the model.
In practice, following this sequence keeps things clean and efficient: ① set the Front View orientation carefully → ② build out your projections, sections, and details → ③ add dimensions thoroughly. Setting up your company’s standard drawing template (.CATDrawing) once will pay dividends on every drawing you create after that — it’s worth the upfront investment.