Inventor: Derive a 2D drawing from a 3D model

A derived drawing automatically stays consistent with the 3D model.

In Autodesk Inventor you do not draw separately in 2D. You derive the detail drawing from an existing 3D model, a part (.ipt) or assembly (.iam). The views in the drawing (.idw or .dwg) are associatively linked to the model: if you modify the model, the views and dimensions update with it. This prevents a drawing from no longer matching the component after a design change.

Inventor has four document types: part (.ipt), assembly (.iam), drawing (.idw or .dwg) and presentation (.ipn). The drawing is created from the part or assembly; use the presentation for exploded views. This workflow, first 3D then 2D, is the opposite of classic drafting, where you draw each line individually, as with the TRIM command in AutoCAD.

Start a drawing with an IDW or DWG template.

First create an empty drawing file:

1. Choose File > New (or New on the start screen).
2. Select a drawing template: Standard.idw or Standard.dwg. Both derive views; DWG is useful if you want to open the file later in AutoCAD, while IDW is the original Inventor format.
3. Preferably use a company template with the correct drawing frame, title block and drawing standard.

The drawing standard determines the projection method. In Europe, ISO drawings use first-angle projection; in the US, ANSI drawings use third-angle projection. You can check or change the standard on the Manage > Styles Editor tab or through Document Settings. If the projection method is wrong, your projected views will be placed on the wrong side.

A drawing file contains one or more sheets. Each sheet has a sheet size (A4, A3, A2), a border and a title block with project data. In the browser on the left, manage the sheets: right-click Sheet to add a new sheet, change the size or choose a different title block. Put your company logo and standard fields in a template, and you will not need to set them up again for each drawing.

Place the first view with Base on the Place Views tab.

The base view is the first, main view from which you derive the rest. Place it as follows:

1. Go to the Place Views tab, Create panel, and click Base.
2. In the Drawing View window, on the Component tab, choose the model from the list of open files, or click the folder icon to open a model file.
3. Set the Orientation (for example Front, Top or an isometric view) and the Scale.
4. Under Style, choose Hidden Line, Hidden Line Removed or Shaded.
5. Drag the preview to the desired position on the sheet and click to place the view.

Place Views > Create > Base > (choose model, orientation, scale, style) > place

Choose the most recognisable view as the base, usually the front view. The scale and style you set here are inherited by the projected views.

Derive top, side and isometric views with Projected.

From the base view you project the remaining views:

1. Click Place Views > Create > Projected.
2. Select the base view as the parent view.
3. Move the mouse up, down or sideways for orthographic views, or diagonally for an isometric view, and click each time to place.
4. Right-click and choose Create to finish the projection.

Place Views > Create > Projected > choose base view > click directions > right-click > Create

Projected views are aligned with the base view and inherit its scale and display settings. If you move the base view, the aligned views move with it. To detach a view, right-click and remove the alignment (Break Alignment).

Control what a view shows using representations, model state and edge display.

In the Drawing View window you determine not only the orientation, but also exactly what is visible. These settings help keep a drawing readable:

• Design View Representation: shows a saved combination of visible and hidden components. In an assembly view, for example, you can leave out the housing.
• Model State: for a part with multiple versions, choose which variant the view shows; for sheet metal, choose between the folded state and the flat pattern.
• Tangent Edges: turn tangent lines on or off to show or hide transitions between fillets as lines.
• Thread Feature and Weld Annotations: choose whether threads and weld seams are included in the view.

For sheet metal, the flat pattern matters: you send that blank to the cutting or punching process. For the base view of a sheet metal part, choose the Flat Pattern model state to show the unwrapped blank with bend lines. This way a single model file provides both the 3D view and the production drawing.

Add sections, details and auxiliary views where they make the drawing clearer.

For complex components, the standard views are not enough. Inventor offers extra view types on the Create panel for this:

For a section view, choose Section, draw a section line across an existing view and place the result. For a detail view, choose Detail, mark a circle or rectangle and specify a larger scale. These derived views also remain linked to the model.

Add extra views only where they add value. A drawing with too many sections becomes unreadable; a drawing with too few leaves questions on the shop floor. A good order is: first the three main views, then an isometric view for overview, and only then sections and details for areas that would otherwise remain unclear. Each section and detail view automatically gets a label (A-A, B-B) that refers to the section line or detail boundary, so the reader can link the views together.

Retrieve model dimensions or place drawing dimensions on the Annotate tab.

Without dimensions a drawing is not complete. On the Annotate tab you have two routes:

• Retrieve model dimensions: with Retrieve Model Annotations (Retrieve Dimensions) you show the dimensions already sketched in the 3D model. These are two-way: if you change the dimension in the drawing, the model changes with it.
• Place drawing dimensions: with Dimension (shortcut D) you add separate dimensions that exist only in the drawing. These are associative but cannot drive the model.

Add hole and thread notes, chamfers, centre lines and surface roughness symbols. Place dimensions consistently and avoid duplicate dimensioning so the drawing is unambiguous for the workshop.

Use Baseline or Ordinate dimensioning when a component has many dimensions from a common datum; this keeps the drawing clear and avoids accumulated tolerances. Place centre marks on holes and bores so the position of each hole is unambiguous. To show tolerances, set them per dimension in the dimension window or centrally through the drawing standard, so the whole drawing follows the same conventions. A consistently formatted drawing saves questions and measurement errors in production.

Add a parts list and balloons to an assembly.

If you derive a drawing from an assembly (.iam), it should include a parts list. On the Annotate tab:

1. Choose Parts List and click a view; Inventor places a table with all components, quantities and part numbers.
2. Choose Balloon or Auto Balloon to give each component in the view an item number that references the parts list.

The parts list reads the data directly from the assembly. If you add a component later, it automatically appears in the list with the correct quantity after updating. For an exploded view, choose a presentation (.ipn) instead of the model for the base view, so the components are shown pulled apart.

The drawing updates automatically and you export it to PDF or DWG.

Because the drawing is associative, after a model change a message appears that the views are out of date. Inventor updates them as soon as you open the drawing or via Update. This keeps the documentation in sync with the design without redrawing views.

Note that a drawing references the model file through a path. If you move or rename the part or assembly outside Inventor, the link is lost and a message appears that the model cannot be found. Use Vault or Save As with references to keep file moves clean, similar to how you keep source data in a fixed location in other packages.

For delivery, export the drawing:

• PDF: via File > Export > Export to PDF, where you set sheets, scale and colour.
• DWG: via File > Export > Export to DWG for exchange with AutoCAD users.

The official steps for base and projected views are in the Autodesk documentation on Base and Projected Views. If you then want to present the model photorealistically, the explanation about reducing Arnold noise in 3ds Max follows on from this.