Overview#
Every drawing starts with a base view: the first orthographic or isometric representation of the model. Projected views are then derived from an existing view by projecting orthogonally (or diagonally for isometrics) in a direction you choose. Because projected views are linked to their parent, they inherit scale and alignment and stay aligned when you move the parent.
Plan the layout before you place views: pick the view that shows the most characteristic profile as the Front view, and keep the number of views to the minimum needed to fully define the part.
Where to find it#
- Drawing workspace toolbar, Create panel: Base View, Projected View.
- Double-click a base, projected, section or detail view to reopen the Drawing View dialog and change scale or style. Orientation, reference and representation can be set only when a base view is first created.
When you create a drawing with the Manual type, Fusion prompts for the base view automatically.
Step by step: base view#
- Choose Base View.
- In the Drawing View dialog, set the Reference: Create New adds a reference node to the browser, Existing Reference attaches the view to one already there. Which components appear (the whole assembly, visible components, or selected ones) is decided in the Create Drawing dialog.
- Set Representation: Model (the static assembly) or Storyboard (an animation).
- Choose Orientation: a Named View defined in the design, Top, Bottom, Left, Right, Front, Back, or SW, SE, NE or NW Isometric.
- Set Scale from the dropdown or type your own. Autodesk accepts ratios (1:48, 1/4"=1'), fractions (1/48) and decimals (.125).
- Set Style: Visible Edges, Visible Edges and Hidden Edges, Shaded, or Shaded with Hidden Edges. For shaded styles, Improve View Quality helps designs that mix long thin and thick parts but increases file size and can slow performance.
- Under Edge Visibility set Tangent Edges (Full Length, Shortened or Off), Interference Edges and Thread Edges.
- Click on the sheet to place the view. If the view does not fit, adjust scale or sheet size, then click OK.
Step by step: projected views#
- Choose Projected View and click the parent view.
- Move the cursor in the direction you want to project. Autodesk defines eight orientations by drag direction: right (0 degrees) gives Right, upper right NE Isometric, up Top, upper left NW Isometric, left Left, lower left SW Isometric, down Bottom, lower right SE Isometric.
- Click to place each view. The parent can be a base, projected or section view.
- Press Enter or click OK to finish.
The drawing's Projection Angle (First Angle for ISO, Third Angle for ASME) is shown read-only in Document Settings and is fixed when the drawing is created. Check the result against your standard.
Isometric and pictorial views#
A diagonal projection creates an isometric view (NE, NW, SW or SE). Isometric views are normally shown in a shaded style, often at a smaller scale than the principal views. Autodesk states you can dimension only orthogonal views, not isometric ones. Another way is a separate base view whose orientation is one of the four isometric choices or a Named View, or a base view with the Storyboard representation to show an exploded layout. A Perspective View command (with a Narrow or Wide focal length) is also documented.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Reference | Create New or Existing Reference | Set only at creation |
| Representation | Model or Storyboard | Set only at creation |
| Orientation | Named View, Top, Bottom, Left, Right, Front, Back, four isometrics | Set only at creation |
| Scale | Display ratio (ratio, fraction or decimal) | Projected views inherit parent properties unless you override them |
| Style | From Parent (derived views), Visible Edges, Visible Edges and Hidden Edges, Shaded, Shaded with Hidden Edges | Hidden lines should be used sparingly |
| Improve View Quality | Better shaded display for mixed thin and thick parts | Larger file, may slow performance |
| Tangent Edges | Full Length, Shortened or Off | Off gives a cleaner look on filleted parts; standards often show them |
| Interference Edges | Show edges where components intersect | Check box |
| Thread Edges | Show threads on threaded edges | Check box |
| Center Marks | Automatic marks for Hole, Round Extrudes, Round Cuts, Pattern, Fillet | Fillet has minimum and maximum radius limits |
| Center Lines | Automatic lines for Hole, Round Extrudes, Round Cuts |
Moving, aligning, and editing views#
- Moving: Drag a view to reposition it. A projected view keeps a parent/child relationship with the view it came from.
- Inheritance: A projected view inherits the properties of its parent. If you override a property on the projected view, later changes to that property on the parent no longer reach it.
- Changing scale: Edit the base view; dependent projected views follow unless overridden. For individual views at a different scale (such as a detail view) set scale on that view.
- Crop/Break: Use Crop View to remove an unwanted part of a view (a view can be cropped only once) and Break View to shorten long parts (covered in the next page).
Note: not confirmed in Autodesk's documentation: how to break the alignment of a projected view, or what happens to children when a parent view is deleted.
Using components and configurations#
For assemblies, you can create views of individual components. Place a base view with Source set to a component to get a part-level drawing from the assembly. The part's drawing then references the assembly design file and component. If you plan to publish a part drawing, a cleaner approach is to open the part in its own design and draw it there.
Note: Autodesk documents creating drawings of configurations and a tabulated drawing for a configured design (see the Create drawings of configurations topics). Which license tier includes configurations is not covered in the Drawing help.
Tips and pitfalls#
Tip: Choose a scale that gives a whole number ratio such as 1:2 or 2:1. Odd scales (1:3.7) are hard to measure from a print.
Tip: Use the minimum views. Many turned parts need one view; sheet-metal flat parts need one flat pattern view plus a bend table.
Tip: Make Front the view with the most features visible. If none of the standard orientations suits, save a named view in the design and choose it as the base view orientation.
Warning: Hidden-line style on a complex assembly creates clutter and slow performance. Use sections instead.
Warning: Large assemblies produce slow-regenerating views. Hide unnecessary components in the design, or draw from a lightweight simplified design.
Warning: When the 3D model changes drastically (features removed), views may need to be rebuilt; dimensions attached to deleted edges will break.
Representations and edge visibility#
The base view's Representation is Model or Storyboard (an animation, used for exploded views built in the Animation workspace). What the view contains is decided in the Create Drawing dialog: Contents (Full Assembly, Visible Only or Select) picks the components, and for sheet-metal components Representation chooses Folded Model or Flat Pattern. The Assembly, Component, Folded Component, Flat Pattern and Storyboard list belongs to the Placeholder View dialog used when building templates. The Drawing View dialog also exposes edge visibility switches and automatic center marks and center lines for the hole types you choose, which saves a lot of manual annotation on plates.
Worked example: laying out three views on A3#
A part is 160 x 90 x 40 mm (width x height x depth) and the sheet is A3 landscape, with roughly 400 x 277 mm of usable area after the border. Third-angle layout puts the Front view at lower left, Top above it, Right to its right. At 1:1 the three views occupy: Front 160 x 90, Top 160 x 40, Right 40 x 90. Total width is 160 + 40 = 200 mm plus gaps; total height is 90 + 40 = 130 mm plus gaps. Leaving 40 mm between views for dimensions gives 240 x 170 mm, comfortably inside the sheet, so 1:1 works and 2:1 would not (480 mm wide). A useful quick test is to add up widths and heights, add 40 mm per gap and compare with the sheet. If you must choose between 1:1 and 1:2 on a smaller A4 sheet (about 277 x 190 mm usable), the same part at 1:1 needs 240 x 170 mm and barely fits, with no room for notes; 1:2 would need 120 x 85 mm and leaves space but makes 2 mm details tiny. Pick based on the smallest feature you must dimension.
Placing an isometric well#
A diagonal projected view creates an isometric. Set it to shaded and at a smaller scale than the principal views, commonly half. Keep it out of the alignment of the others by placing it in the empty upper-right corner, where it also helps readers connect the 2D views to the 3D shape. Do not dimension it; isometric views cannot be dimensioned. If the isometric hides the feature you want to show, create a separate base view with a different isometric orientation (SW, SE, NE or NW) or a Named View saved in the design.
Failure modes and fixes#
| Symptom | Likely cause | Fix |
|---|---|---|
| Front view shows the wrong face | Front is defined by the design | Delete the view and create a new base view with another orientation or a Named View (orientation cannot be edited later) |
| Projected view will not move sideways | Projected views keep a parent/child relationship with their parent | Place it in the other projection direction, or create a separate base view |
| Thread edges missing | Thread Edges unchecked, or no thread in the design | Check Thread Edges and add a thread in the design |
| Tangent lines clutter a filleted part | Tangent edges shown | Set Tangent Edges to Off or Shortened, unless your standard requires them |
| Views slow to regenerate | Large assembly | Hide fasteners in the design or use a simplified copy |
| Hidden lines everywhere | Visible and Hidden style on an assembly | Use a section view instead |
| A diagonal click gave an isometric when you wanted a side view | Cursor not aligned | Hold the cursor along one axis before clicking |
Workflow advice#
Choose the Front view by asking which view shows the most distinguishing outline and the greatest number of features. Place one base view, then ask what is missing: a hidden internal feature (section), a tiny feature (detail), an inclined face (auxiliary). Add only those views. A common beginner mistake is placing six principal views by habit; a turned part usually needs one, a plate two, and a bent bracket three. Before dimensioning, move views to their final places and fix their scale, because moving a view later drags dimension positions with it.
Name the representation and orientation in your notes when you work on a series of related parts, so that every drawing in the set uses the same Front convention. If you routinely draw from assemblies, keep a part-only design for the final release drawing rather than referencing a component inside the assembly, as the latter breaks when the assembly is restructured.
Practice exercise#
- Use the Bracket design. Create a base view with Front orientation at 1:1, style Visible Edges, tangent edges off.
- Add Top and Right projected views. Check that placement matches your template's projection angle, and measure the gaps between views.
- Add a diagonal projected view for an isometric, set it to shaded at 1:2 and drag it to the empty upper-right area.
- Turn on automatic center marks for through holes in the base view dialog and confirm the holes gain cross marks.
- Edit the base view to 2:1 and decide which views still fit. Revert to the largest scale where all three views fit with 30 mm gaps. Write down the sum of widths and heights that justified your choice.
- Double-click the base view and change Tangent Edges between Full Length, Shortened and Off; note the effect on the filleted edges.
- Expected result: three aligned orthographic views and one shaded isometric, center marks on the holes, and a measured justification for the scale.
Related#
- Section, detail, auxiliary, and break views
- Dimensions and tolerances
- Sheets and exploded drawings