Create a base view
Learn how to create a base view on a sheet in the Drawing workspace in Fusion.
Select Create > Base View .
The Drawing View dialog displays and a preview of the base view displays at the cursor.
Click to place the base view on the sheet.
In the Drawing View dialog, select the Reference.
- Create New: Adds a new reference to the browser.
- Existing Reference: Adds the base view to the selected existing reference in the browser.
Select the Representation.
Adjust the Appearance settings:
- Orientation: Select one of the standard orthographic views or a named view.
- Style: Select a display style.
- Visible Edges
- Visible and Hidden Edges
- Shaded
- Shaded with Hidden Edges
- Improve View Quality (Shaded and Shaded with Hidden Edges): Select to improve the appearance of shaded views. May affect performance.
- Scale: Select a scale.
Adjust the Edge Visibility settings:
- Tangent Edges: Select a display style for tangent edges.
- Full Length
- Shortened
- Off
- Interference Edges: Check to display interference edges.
- Thread Edges: Check to display threaded edges.
Specify the automatic creation of Center Marks and Center Lines:
- Center Marks: Choose the hole types that receive automated center marks.
- Hole: Creates a center mark for hole features.
- Round Extrudes: Creates a center mark for round extrudes.
- Round Cuts: Creates a center mark for round cuts.
- Fillet: Creates a center mark for fillets.
- Minimum fillet radius: Specify the minimum fillet radius for a center mark to be created.
- Maximum fillet radius: Specify the maximum fillet radius for a center mark to be created.
- Center Lines: Choose the hole types that receive automated center lines.
- Hole: Creates a center line for hole features.
- Round Extrudes: Creates a center line for round extrudes.
- Round Cuts: Creates a center line for round cuts.
Select OK.
The base view displays on the current sheet.