Views

Place a view of the model (part, surface, assembly, sketch, curve, composite part, or flat sheet metal pattern) on the active sheet; use the dialog to select the desired part, sketch, or flat sheet metal pattern, including version and orientation. By default, the label and scale are off. To see the scale, double-click the view: the View properties dialog opens to the top left of the drawing.

1. Click Insert view in the Toolbar:



2. Click the Insert button in the dialog (shown in the left image below) to open the Select a part or assembly dialog (shown in the right image below). Search the Part Studios and Assemblies in the current (or other) document(s) for parts, surfaces, assemblies, curves, or sketches (or versions thereof):

   

   1. Select to insert from the Current workspace (in Part Studios or Assemblies in this document):

      

      By default, the selected filter is Parts, but you can also search for an entire Part Studio, Assemblies, surfaces, sketches, curves, composite parts, and sheet metal flat patterns. These filter icons appear only when the selected Part Studio or Assembly contains these types of entities:

      

   2. Or, click Other documents to use the familiar filters to search for and then select from a version in a different document:

      

   3. Once a document is selected, if it has versions, click to open the Version graph and select the version or workspace from which to select a part or assembly:

      

      You can also select to view only released items , and to create a version.

3. Once a Part Studio or Assembly is selected, select a view using the Insert view dialog:

   

   The screenshot on the left shows the Insert view dialog for a Part Studio; the one on the right shows the dialog for an Assembly

   For Part Studios and Assemblies:

   • Select the View orientation: Top, Left, Right, Front (default), Back, Bottom, or Isometric. You can also select existing Named views (with and without section planes), if applicable.

   • Select the View scale dropdown to select a specific scale for the view.

   • Select the View simplification: None, Absolute, Ratio to studio, Ratio to part, or Auto (default). This simplifies the geometry shown in the drawing by setting a threshold below which features are hidden. This setting only affects newly inserted views. See Insert view defaults for more information.

   • Optionally, select the checkbox next to Show sketch appearances to show the appearances from the Part Studio or Assembly you are inserting from.

   

   For Assemblies, if available:

   • Select the View orientation: Top, Left, Right, Front (default), Back, Bottom, or Isometric. You can also select existing Named views (with and without section planes), if applicable.

   • Select an exploded view / named position using the Explode/Position dropdown.

   • Select a display state using the Display state dropdown.

If a named view, exploded view/named position, and/or display state is active when creating a Drawing tab for the first time, the Insert view dialog fields are pre-populated with that view, position, and/or state.

4. Once you have the intended entity selected, click on the drawing to place the view. A preview appears as you place the view.

Deleting views

1. Select the view to delete using any selection method.
2. Press the Delete key or right-click to activate the context menu and select Delete.

Moving a view

1. Select the view.
2. Drag to the desired placement.

Moving a view to another sheet

You can move any view to another, pre-existing sheet in your drawing through three ways: use the Move to sheet command on the context menu, select a new sheet in the Sheet dropdown in the View properties dialog, and by dragging the view to another sheet in the Sheets panel.

When a view is moved to another sheet, all related entities (labels, dimensions, etc) move with it.
When moving an auxiliary view, the parent view is not moved.
When moving a parent view, the auxiliary view is not moved.

Moving a linked view to another sheet

If a view is linked to another view, for example a Section view is created from a Front view, and one of these views is moved to another sheet, the view displays an arrow at the top right corner of the view icon in the Sheets panel, to indicate it is linked to a view in an external sheet:

The Section view in Sheet 2 is linked to the Front view in Sheet 1.

Note the following:

• Updating a reference for a linked view also updates all views to which it is linked.

• Currently, it is not possible to unlink a view. It must first be deleted, and then a new view added into the sheet in question.

Copying a view

Copy and paste views from one location to another in the same sheet, from one sheet to another in the same drawing, or from a sheet in one drawing to a sheet in another drawing in the same workspace. You cannot copy and paste views from one workspace to another, for example, from one document to another.

To copy any view:

1. Click the view to select it.

2. Right-click and select Copy (Ctrl+C) from the context menu.

3. With the cursor over the new location, right-click and select Paste (Ctrl+V) to place the copied view.

You can also copy a view by holding the Alt key, then selecting and dragging the view you want to copy.

Select a view, right-click, and select View properties. Alternatively, you can double-click a view to open the View properties dialog:

You can select a Display state (when available) and the views update accordingly.

When multiple views with differing values for their properties are selected, the appropriate fields in the dialog display multiple values, as shown below:

For Detail and Section views, there are additional View label options, explained below.

For Projected views created from Section views, there is an additional option for working with cuts, explained below.

• Document - The name of the document the part or assembly resides in.
• Workspace or Version - The workspace name if the part or assembly is from the current document. The version name if the part or assembly is in a different document (when Part Studios or Assemblies are moved to another document, that document is automatically versioned).
• Type - Whether the drawing is of a part or an assembly.
• Reference - The name of the part or assembly of the drawing, with a link to open the referencing document and Part Studio or Assembly tab.
• View orientation - To change the view from one perspective to another, select from the dropdown: Top, Left, Right, Front, Back, Bottom, Isometric, or Named.

If a Named view was inserted and then subsequently deleted from the workspace, it is grayed out in the context menu list. You can select a different view orientation or leave the current view as is.

• Scale - Set the scale of the drawing. Input is in an N:N or N/N format. For user input values, the second digit or denominator is always set to 1, and you can double-click the Scale label to edit it. By default, the scale of a Projected view is always set to Parent (the same scale as the parent view).
• Rotation angle - Use this to rotate the angle of view (in default units). The arrow reverses the direction of the angle. All views, when created, have a rotation angle of 0 degrees. You can change this value only if the view has no parent (is not a 'child'), is not a parent (has no 'children'), or if the alignment with a parent is suppressed.

  Valid values are between 0 and 360 degrees.

  Views that may be rotated may also be Aligned view vertically or horizontally along a selected straight edge.

• Tangent edges - Select the visual treatment of tangent edges in the view:
  • Hidden - Tangent edges are visually removed from the drawing:

    

  • Solid - Tangent edges are shown by solid lines:

    

  • Phantom - Tangent edges are shown by broken lines:

    

• View render mode - Select the type of render mode you wish: Best quality or Best performance. Drawings views default to Best performance. If, in certain cases, some edges are not displayed correctly, you should change the View render mode to Best quality. The rendering mode setting applies to both drawing views within Onshape and views in exported drawings.
• View simplification - This feature allows users to simplify the geometry shown in the drawing by setting a threshold below which features will be hidden.

  • Auto - Default. Finds the best view simplification settings based on the geometry of the part and automatically uses those settings to display the part or assembly.

  • Absolute - Enter a number in the length units of the drawing to indicate that any feature smaller than the value will be simplified within the view. If whole parts are smaller than the threshold value, those parts will be missing from the view. This is useful for removing excessive details not needed for drawing purposes (for example, a large number of very small features or components).

  • Ratio to studio - Enter a percentage of the size of the Part Studio or Assembly below which the feature will be simplified within the view. If whole parts are smaller than the threshold value, those parts will be missing from the view. This is useful for removing excessive details not needed for drawing purposes (for example, a large number of very small features or components).

  • Ratio to part - Enter a percentage of the size of the part below which the feature will be simplified within the view. This setting aims to preserve parts in a view, while simplifying the detail within those parts. This is useful if you intend to ensure all the parts are present to facilitate detailing actions, such as placing callouts.

  All child views will receive the View simplification setting of their parent view, but any child view can be independently changed later and not affect the rest of the view settings in the parent/child dependency.

• Sheet - The name of the current sheet shown; use the dropdown to move the view to another sheet.
• Name - The name of the view in the format <view perspective>-<part name>. Changing the name of the view does not alter the view perspective or the part name.

  With a single view selected in the Sheet/Views list, you are able to use Shift+N to open the Rename dialog.

• View label - All views (Projected, Auxiliary, Section, and Detail) allow you to place a View label below the view in the drawing. View labels are applied automatically when adding a Detail or Section view. To apply View labels to Projected and Auxiliary views, open their Property dialog, check View label, and provide a label name.
  
  For Detail and Section views you may optionally specify a custom prefix and suffix for the label, creating a multi-line label. Changing the letter also changes the letter of the view referenced (the parent of the Detail view or the cutting line of a Section view, for instance).

  

• Scale label - Check to display the scale label below the view.
• Show sketch appearances - Check to show the sketch appearances from the Part Studio or Assembly in the Drawing.
• Move to sheet - Opens a dialog with a dropdown listing all available sheets. Select a sheet to move the currently selected view to.
• BOM table reference - Select the assembly the BOM table should reference.
• Cut list table reference - Select the cut list table that should be referenced.
• Apply parent view section cut - When creating a Projected view from a Section view, toggle this option to create the Projected view with the cuts from the parent view.

You can also open the Part Studio or Assembly that the view is from, and specify a scale, rotation angle, and scale label.

Select Parent scale to link the view's scale to its parent’s scale or Sheet scale to link the view’s scale to the sheet scale.

Notes

• The view rotates around the center of the view rectangle, which changes size as needed. For detail views, the view rotates about the center of the circle surrounding the detail view; the visible geometry stays the same and the circle stays the same size.
• When the Rotation angle is not 0 degrees, then the view properties to reconnect alignment are disabled. Similarly, the commands to reconnect alignment with the parent are also disabled. You must change the Rotation angle to 0 degrees before the view can reconnect with the parent.
• All dimensions adjust when a Rotation angle changes. Vertical and horizontal linear dimensions remain vertical and horizontal. Aligned and rotated linear dimensions remain aligned and rotated to their view geometry.
• View scale and label location change to be centered below the new view rectangle or detail view circle.
• Use Suppress alignment with parent to remove the alignment of the view to its parent. If there are no dependencies, that is, if the view has no children, then you can use the Rotation angle field once the alignment is broken. However, if there are other issues blocking the view from being rotated (that is, if it has children), then the view cannot be rotated. Keep in mind, that if a view has children it cannot be rotated even if you suppress alignment.
• Copy a view label using Ctrl+C to copy the label and apply the default properties of Notes (from the Property panel). Use Alt+drag to copy a view label keeping the view label properties.