View Navigation and Viewing Parts

The mouse wheel direction for zoom is configurable in user account preferences.

To zoom:

• Zoom to fit (shortcut: f, double-click scroll wheel) - Select this command or use the shortcut key to zoom the entire Part Studio, Assembly or Drawing into view.
• Zoom to window (shortcut: w) - Select this command, then click+drag a box around the area you want to zoom to in a Part Studio, Assembly or Drawing. The shortcut key toggles the feature on and off.
• Zoom to selection - Select this command to zoom to the selected entities.

Detect and view the interference between parts in a Part Studio or Assembly.

1. With more than one part in the Part Studio or Assembly, select Interference detection from the View tools menu:

   

2. Select two or more parts among which to view any interfering mass.

   

   The interference is shown in red, as above, and the parts involved are listed in the Interferences section of the dialog.

   Hover over the part name in the dialog to see cross-highlighting in the graphics area when and vice versa. When the focus is on the Interferences field in the dialog box, the graphics area zooms to fit the selected interference. Hover over the Interferences field in the dialog box and a bounding box appears in the graphics area, surrounding the interference in the model. In the dialog box, the length/width/height of the bounding box also appears on hover:

   

   You can use box select to select entities for interference detection: drag from top left to lower right to include only parts or bodies fully encompassed by the box. Drag from lower right to top left to include any parts or bodies touched by the selection box.

Tangent edges are edges formed between a curve and linear edge; for example, from fillets or smooth edges.

To select the visual treatment of tangent lines, select from the following three view modes:

• Visible - Tangent edges are shown as solid lines. This is the default.
• Phantom - Tangent edges are displayed as dashed lines; also known as Font in some systems.
• Hidden - Tangent edges are visually removed from view.

Three different tangent edge options, from left to right: Visible (default), Phantom, and Hidden.

Tangent edges are currently only available for newly created models in a Part Studio or Assembly, and only on the browser platform.

Opens the Curvature visualization dialog, which represents the reflection of a striped room on the current model. This allows you to see whether or not the curvature across edges is aligned and continuous:

• Stripe count - Number of curvature stripes displayed on each surface

• Flip stripes - Reverses curvature stripes.

• Show edges - Displays the edges between part faces (default). When unchecked, the part edges are hidden. Hiding these edges improves the curve visualization between part faces in certain situations.

When the curvature is aligned across an edge, the edge is smooth and the stripes line up, and then veer off across the edge:

When the curvature is continuous across an edge, the edge is smooth and there is no change in curvature across the edge. Stripes line up and do not veer off across the edge:

Examples:

No curvature	Default curvature: 35 stripes
10 stripes	35 stripes; flipped

Use Draft analysis to find faces in the model that do not meet a specified minimum amount of draft, discover undercut regions, and see the potential parting line locations for selected geometries.

Select Draft analysis from the View tools menu:

1. In the dialog, indicate the Mold split direction by selecting a plane, face, or edge.

   

2. Specify the minimum draft angle.
3. Select the part or parts to check.
4. Optionally turn off the indication of red undercut faces (Show undercut regions check box).

Notice the draft analysis flyout in the bottom right corner of the window.

• Faces in blue indicate they meet the specified minimum angle for the draft.
• Faces in yellow indicate they are too steep (i.e. less than the minimum specified draft).
• Faces in red indicate undercut faces.

You can view the exact angle of individual drafts by moving the cursor over the model:

As with other visualization modes, draft analysis remains active until you select something else. While it is active, you are able to edit the part to correct the drafts and see the immediate result of your actions. You are also able to use section views to view places on the model that might otherwise be difficult to see.

To change the details of the draft analysis, click Edit draft analysis in the lower right corner:

Draft analysis works automatically in both directions. Onshape displays acceptable draft in different colors to indicate direction: light blue for side one (positive direction) and dark blue for side two (negative direction). The manipulator arrow points to side one and you can flip it using the directional arrow in the dialog, as shown above next to the Mold split direction field.

The image above shows the draft angle after the directional arrow was clicked to flip the direction of the analysis: the light blue shows the positive direction and the angle is shown as a positive angle. By contrast, the image preceding, the dark blue shows the negative direction and the angle is shown as a negative angle.

Set the level of transparency of a part through the Part context menu; right-click on a part name in the Parts list and select Appearance editor. See Customizing Parts, Faces, and Features: Appearance for more information.

Section view is available from the View Tools cube, allowing you to select one or many planes, mate connectors, cylindrical faces, conical faces, or planar faces to use for sectioning.

You can also use the context menu for a plane to select Section view and turn this view type on.

Once the manipulator is visible, you may move it via the ball (open circle at its center) and snap it to any inference point on the part, surface, or assembly. You can view sectioned items in both Part Studios and Assemblies:

1. Select one or many planes, mate connectors, cylindrical faces, conical faces, or planar faces on the part or surface.
2. Expand the menu on the View Tools cube and select Section view.

   

You can alternately select the Turn section view on command before making any selections.

3. The part/surface is sectioned at the point you chose in step 1 above (cylindrical face, conical face, planar face, plane, or mate connector). A manipulator appears at the last location selected and a dialog opens listing selections:

   

Intersecting parts, if they exist, are rendered in red.

4. Click and drag the open circle (ball) of the manipulator to position it. Notice you can snap it to any inference point on the part or assembly, including the centroids of cylinders (the white marks below indicate inference points):

   

   

5. Use the manipulator to change the depth and/or angle of the section.
   1. Use the arrow to change the depth, dragging in one direction or another. Click the manipulator to flip the direction of the view.
   2. Use the angle indicators to drag at an angle.
   3. Use the numeric field to type the depth or angle of the view.

    

   

6. To select a different sectioning plane, click the selection in the dialog box to activate the manipulator:

   

7. To view the section normal to the section view plane, use shortcut key n or right-click and select View normal to from the context menu.
8. To exclude a part or parts (surface or surfaces) from being sectioned, activate the Items to exclude field then make your selections in the graphics area:

   

9. To include a part or parts (surface or surfaces) in the section, select the Include tab, then select the items to include in the graphics area:

   

10. Select Turn off Section view when you're finished.

You can use Section view and then save the view as a Named View.

Keyboard shortcuts for view

• Front view = Shift 1
• Back view = Shift 2
• Left view = Shift 3
• Right view = Shift 4
• Top view = Shift 5
• Bottom view = Shift 6
• Isometric view = Shift 7
• Section view = Shift X
• Named view = Shift V

Use Zoom to selection to change the view to a close-up of the selected entities.

Make a selection in the graphics area:

Expand the View menu and select Zoom to selection:

Onshape displays holes and disconnects in a model, including laminar edges of surfaces, that may be in need of repair when you select Highlight boundary edges. This feature is especially helpful when importing parts that require repairing surfaces.

Select Highlight boundary edges in the View tools menu. Edges that may require repair are highlighted in solid red lines when the edges are visible and dashed red lines when the edges are hidden:

This tool is available only in Part Studios. For more information, see Repairing Imported Models.

shift+r

Toggle to select/deselect the highest available quality tessellation view for the currently active Part Studio or Assembly. Be aware that this may result in a slight degradation of performance. When you turn this option on, the blue notifications are displayed as shown below:

For more information on how this view mode may affect performance, see High quality mode.

3D Rotate Lock, when active, locks the user's ability to 3D rotate the graphics area. This is particularly useful when attempting to select and drag an entity.

It is located directly above the View Cube in both Part Studios and Assemblies.

To activate the 3D Rotate Lock, tap the button. To deactivate, tap the button again or commit a feature.

3D Rotate Lock activates by default in certain situations:

• Part Studio - If a sketch is open and an entity is selected, the 3D Rotate Lock turns on by default. This allows for the selection to be dragged without the view rotating. Unlock by tapping the button.
• Assembly - If an instance, mate connector, or entity is selected, the 3D Rotate Lock turns on by default. This allows for the selection to be dragged without the view rotating. Unlock by tapping the button.

The View cube is located in the upper right corner of the graphics area. When selected, a list of different viewing options appears. Select one to change the view of your graphics area or the view settings of your part(s). This is an easy and quick way to get a well-oriented view of your part(s) without having to 2D/3D rotate or zoom.

Steps

1. Tap the View cube. A list of options appears.

   

2. Tap to select a view option or select Cancel.
3. Scroll to see more options.

Options explained

• Top, Bottom, Front, Back, Right, and Left - Select any of these options for a front-facing view of the respective plane.
• Isometric, Dimetric, Trimetric - Select any of these for the respective angled view.
• Zoom to fit - Select to resize the graphics area to fit the screen. This could result in the view zooming in or out.
• Perspective View - Toggle perspective view on and off. Perspective view shows the relative distance from the point of view to the model, and creates a vanishing point as the point of view (or imaginary camera) approaches the model. The images below show a front view of the same part without perspective view and with perspective view, respectively.

  

  

• Shaded - Select to show the part with shaded faces and edges. (Default)

  

• Shaded without edges - Select to show part shaded, without edges.

  

• Shaded with hidden edges - Select to show the part shaded and to show hidden edges (edges that aren't in the direct line of sight).

  

• Hidden edges removed - Select to show the part unshaded, with the hidden edges (edges not in direct line of sight) removed.

  

• Hidden edges visible - Select to show the part unshaded, with the hidden edges (edges not in direct line of sight) visible.

  

• Translucent - Select to show the part as translucent.

  

• Section View - Select to access a manipulator that allows you to adjust a section view of a part, via a plane or planar face.

  

  You must preselect a plane or planar face before selecting Section View.
  Drag the arrow or either directional manipulator to adjust the section view plane that is created from the preselected plane or planar face. In this case, the Front plane is used to create a section view roughly halfway through the parts.