How to Create a Non-Standard Drawing View in SOLIDWORKS

When creating a technical drawing in SOLIDWORKS, standard views such as Front, Top, Right, Left, and Isometric are usually enough. But what happens when your part contains an angled face, inclined hole, or feature that cannot be clearly shown using standard orientations?

This is where non-standard drawing views become useful. A custom or non-standard view allows you to present a model from a specific orientation so that critical geometry can be accurately displayed and dimensioned. SOLIDWORKS provides several ways to achieve this, including Auxiliary View, Current View, and Relative to Model View.

What Is a Non-Standard Drawing View?

A non-standard drawing view does not follow conventional orthographic (Front, Top, Right) or Isometric alignments. For example, if a mechanical component has a face angled at 35°, standard views foreshorten that face, preventing accurate dimensioning.

Creating a view normal to the angled geometry provides several key advantages:

• Easier to understand
• Easier and more accurate to dimension
• Reduces drawing clutter
• Ensures precision for manufacturing and inspection
• Improves organization for complex components

Method 1: Create an Auxiliary View

An Auxiliary View is designed to project a view perpendicular (normal) to an angled edge or face by unfolding it relative to selected reference geometry.

1. Open Your Drawing: Open the drawing sheet containing the view with the angled feature.
2. Select Auxiliary View: From the CommandManager, go to Drawing ? Auxiliary View, or use the menu: Insert ? Drawing View ? Auxiliary.
3. Select a Reference Edge: Choose the angled edge representing your reference plane. The reference can be:
   • A model edge
   • A silhouette edge
   • An axis
   • A sketched line
   Note: Avoid horizontal or vertical edges, as these generate standard projections rather than an angled auxiliary orientation.
4. Position the View: Drag your cursor into position and click to place the unfolded view on the sheet.
5. Add Dimensions: Dimension the true surface area and geometry directly without foreshortening errors.

Method 2: Use a Custom Current View

This method pulls a custom orientation directly from the active 3D model viewport into the drawing sheet.

1. Open the 3D Model: Switch to the referenced part or assembly file.
2. Orient the Model: Rotate the model to the exact visual orientation required. You can also select a planar surface and click Normal To to align directly to it.
3. Return to the Drawing: Switch back to your drawing sheet document.
4. Open the View Palette: Click the View Palette tab in the Task Pane on the right.
5. Insert Current View: Select Current View from the list and drag it onto your drawing sheet.

Method 3: Create a Relative to Model View

The Relative to Model tool establishes an orthographic view defined by two perpendicular model faces or planes, retaining associativity if the model geometry changes.

1. Select Relative View: Go to Insert ? Drawing View ? Relative To Model.
2. Choose the First Orientation: In the PropertyManager, select the primary direction (e.g., Front, Top) and select the corresponding planar face or reference plane on the model.
3. Choose the Second Orientation: Select an orthogonal secondary orientation (perpendicular to the first) and pick the matching model face.
4. Place the View: Click OK and position the resulting custom view on the drawing sheet.

Method Comparison

Common Issues and Troubleshooting

• Inverted or Incorrect View Rotation: Check the selected reference edge or reverse direction in the PropertyManager. Alignment options can also be adjusted post-placement.
• Face Remains Foreshortened: Ensure the reference entity is truly parallel to the intended viewing direction. Use the Normal To command or Relative View if edge references fail.
• Sheet Crowding: Place only the custom views necessary for manufacturing callouts. Avoid redundant standard views when an auxiliary view covers the required detail.
• Dimensioning Difficulties: If dimensions show incorrect values or won't align, confirm that the drawing view is truly planar and perpendicular to the measured face.

Best Practices for Clearer Technical Drawings

• Prioritize Simplicity: Do not use complex custom views if standard projected views adequately communicate the design.
• Rely on Auxiliary Views for Angled Geometry: It remains the cleanest standard for single-angle callouts.
• Maintain Alignment: Keep projected and auxiliary views aligned with their parent views whenever possible for clear visual tracking.
• Eliminate Visual Redundancy: Every view on the sheet should communicate unique, actionable manufacturing or inspection data.