Analysis Tools

Visualize and analyze curvature using various methods on a sketch or part in a Part Studio. Access the Curve/surface analysis dialog box through shortcut keys (shift+c), the context menu on a sketch, part, or surface, or through the Show analysis tools menu in the bottom right corner of the interface.

When in sketch mode, or while editing a sketch, you can use the shortcut Shift+c to automatically select all sketch curves and open the Curve/surface analysis dialog. Shift+c acts as a toggle: opening and closing the dialog while selections persist.

The Curve/surface analysis tool remains open even after exiting out of the sketch, however, the selection fields are not active. You can add more selections, or remove selections as long as the tool is open. Any changes to selections persist for the next time you invoke the tool. If you make a pre-selection before opening the tool, the tool opens with just that selection, clearing any other selections made previously.

To examine curves and surfaces:

1. Click the Show Analysis tools icon () in the bottom right corner of the interface, then select Curve/surface analysis to open the dialog box. (You can also RMB-click on a sketch or part and select Curve/surface analysis):

   

2. Select the curve or surface you wish to examine.

3. Use the slider at the bottom of the dialog to adjust the magnitude of the combs, use the check boxes to choose whether or not to show curvature combs, inflection points, minimum radius, U curves, V curves, whether or not to have the combs extend across the face.

   

   Example of what a sketch curve looks like with Show curvature combs and Show minimum radius selected in the dialog box. When sketch inflection points are present, they appear as black 'bow ties'.

   

   Image example of what a sketch curve looks like with only Show curvature combs selected in the dialog box.

   Curvature combs are evaluated at evenly spaced isolines, not necessarily at the control points, and are used for evaluating the resultant shape of a curve/surface up to Flow (G3) continuity.

4. Click and drag a curve to adjust the curvature, if necessary. The combs update dynamically while you drag.

5. To visualize U-curves and/or V-curves, select either or both of those check boxes, for example:

   

6. Optional.  Increase or decrease the number of U or V curves from 2 to 64. The default is 8 for each.

7. Select Control point grids to show the location of the control points on the underlying bSpline curves that define the surface (or curve). The number and distribution of the control points provides important information about the underlying math defining the shape.

   Dense clusters of control points indicate potential problem areas, and can be deleterious to the surface quality. In short, control point grid is used to understand the underlying mathematical definition of the surface/curve,

8. When finished, close the Curvature dialog; click .

With the slider towards left of center:

With the slider closer to center:

Showing curvature during feature creation

You can also show the curvature combs for a feature in-process, for example, during an extrude:

1. With the feature dialog open, right-click in the graphics area and select Show curvature to open the Show curvature dialog:

   

2. Select a curve for the feature:

   

3. You can show the curvature for the selected edge used to create the new feature (uncheck Show for previewed edges), or select Show for previewed edges to see the curvature combs for the edge of the new feature being created:

   

You can also show curvature combs, inflection points, and the minimum radius by selecting the boxes to the left of those options in the Show curvature dialog box, shown below:

Example of a feature with Show for previewed edges, Show curvature combs, Show inflection points, and Show minimum radius selected in the Show curvature dialog box.

Display the dihedral angle of selected edges in Part Studios.

Shortcut: Shift+d

When in sketch mode, or while editing a sketch, you can use the shortcut Shift+d to automatically open the Dihedral analysis dialog. Shift+d acts as a toggle: opening and closing the dialog while selections persist.

Any changes to selections persist for the next time you invoke the tool. If you make a pre-selection before opening the tool, the tool opens with just that selection, clearing any other selections made previously.

1. In a Part Studio, click the Show Analysis tools icon () in the bottom right corner of the interface.

2. From the menu, select Dihedral analysis to open the dialog box:

   

3. Select an edge or edges to show the dihedral angle.

4. Select your preferred unit of measurement.

   • Max - When an edge (or edges) is selected, the maximum dihedral angle is displayed.

   • Min - When an edge (or edges) is selected, the minimum dihedral angle is displayed.

5. Optionally, select Enable threshold display to activate the customizable high and low threshold fields.

6. Optionally, use the Scale slider to adjust the length of the dihedral combs.

   

The image above shows an example of an edge on an entity in the graphics area with the Dihedral analysis tool applied.

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, click the Show analysis tools menu in the bottom right corner of the interface.
2. From the menu, select Interference detection to open the dialog box.
3. 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 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.

Zebra stripes represents the reflection of a striped room on the current model, faces, or surfaces in a Part Studio or Assembly. This allows you to see whether or not the curvature across edges is aligned and continuous.

1. Click the Show Analysis tools icon () in the bottom right corner of the interface.

2. From the menu, select Zebra stripes to open the dialog box:

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

• Flip stripes - Reverses the 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 visualization	Default curvature: 35 stripes
10 stripes	35 stripes; flipped

When you accept the Zebra stripes dialog (click the check mark), the dialog closes and the stripes remain. To turn the zebra stripes off, select Zebra stripes from the Show analysis tools menu again and click the X in the dialog. (Selecting Color map from the Curvature visualization menu also turns off the zebra stripes.)

Curvature color map enables deeper investigation of curvature by applying a gradient of color of your choosing onto a face or surface in a Part Studio. You can adjust the scale of the color gradient and choose from different types of color maps to gain the best visual representation to discern surface continuity and transition between edges.

1. Click the Show Analysis tools icon () in the bottom right corner of the interface. From the menu, select Curvature color map:

   This applies a color map to the faces and surfaces in the graphics area, using a color gradient to show curvature across a scale:

Options for visualizing curvature with a color map include:

• Setting colors for the map. Click the dropdown menu to select a color scheme that best suits your needs and visualization preferences:

  • Viridis - A scale of deep purple to light green

  • Blue -> Red - A scale of blue to red

  • Plasma - A scale of deep blue to light yellow

  • Rainbow - A scale of colors of the rainbow

• Selecting a graph for the map. Click the dropdown menu to select a specific graph:

  • Gaussian - Bases the color assignments on the product of the maximum and minimum radii at a given point. The curvature is displayed as the inverse of the radius.

  • Mean - Bases the color assignments on the mean of the maximum and minimum radii at a given point.

  • Max radius - Bases the color assignments on the maximum radius value at a given point.

  • Min radius - Bases the color assignments on the minimum radius value at a given point.

You can relocate the color map to any location in the graphics area to improve viewing of model and map. Hover over the graph until you see a cross-hair for mouse pointer. Click and drag the graph to a new location. For some locations, the graph reorients to a vertical position. The Colors and Curvature dropdowns remain at the top of the graphics area, regardless of where the graph is located.

Tips

When there is no curvature of the surface or face, Onshape doesn't assign any values to the color map scale since there are no calculations of radii. The color map is still visible and you can still select from maps and colors. No curvature color is applied if there are no values calculated. The model remains the same color before any curvature analysis tools were opened.

You can change the scale by clicking and dragging the end points of the scale closer to eachother. The points on the scale recalculate and the colors are refreshed on the faces and surfaces according to the new scale. You can also click on a value and type into the field to adjust the scale. Make sure to click the small refresh icon.

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 in a Part Studio.

1. Click the Show Analysis tools icon () in the bottom right corner of the graphics area. From the menu, select Draft analysis to open the dialog box and color legend. In the dialog box, indicate the Mold split direction by selecting a plane, face, or edge.

   

2. Specify the minimum draft angle.
3. Select entities to check.
4. Optionally turn off the indication of red undercut faces using the Show undercut regions check box.

Notice the draft analysis color legend at the top of the interface.

• Faces in blue indicate they meet the specified minimum angle for the draft.
• Faces in yellow indicate they are too steep (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 can edit the part to correct the drafts and see the immediate result of your actions. You can also use section views to view places on the model that might otherwise be difficult to see.

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.

Use Thickness analysis to measure how much material is distributed throughout each region of a part.

Currently only native Onshape parts and mesh model types are supported.

Steps

In a Part Studio that contains at least one part:

1. Click the Show Analysis tools icon () in the bottom right corner of the graphics area. From the menu, select Thickness analysis to open the dialog box:

   

2. Select a part (or parts) to analyze.

   Onshape instantly begins to compute the thickness analysis request. The progress spinner in the bottom left of the graphics area provides an update on the status of the analysis: 

   • Preparing thickness analysis - Geometry is discretized and processed for analysis

   • Processing thickness analysis - High performance cloud instances are provisioned

   • Calculating thickness - Thickness analysis computation begins

   • Refining thickness analysis - Initial results are available and higher fidelity results continue to process

   • Postprocessing thickness analysis - Final results are processing and will soon be available

3. Click the green check mark to accept your selection and close the dialog box. The thickness analysis tool stays active. When the initial thickness analysis results are available, the color bar opens in the graphics area: 

   

   Selected parts automatically render. The color bar maps field values to the colors displayed along the surface of your part (or parts).

4. To change the color scheme, select a palette from the Colors dropdown.

5. To change the color bar's range, select either the lower or upper bound value and type in a new number. Use the refresh button to reset the bound to the lowest/highest value within the measured field.

   Alternatively, click and drag the tick mark above either the lower or upper bound value and drag it to a new position along the legend. Reposition the color bar entirely by hovering your cursor until it becomes active, then click and drag the legend to a new position on your screen.

   Unless manually adjusted, the legend's bounds may automatically adjust to new limits while intermediate thickness analysis results are refined. Once manually adjusted, intermediate updates will not cause the upper or lower bounds to change. However, the far-most values along the color bar may update as new information becomes available.

   The legend shows unique colors for field values outside of the user-defined bounds. Check the Dim colors scale option to create a 3-color view and quickly assess regions outside of your target range.
   
   

6. Select the preferred field from the Method dropdown menu: 

   • Rolling ball

   • Rolling ball gradient (%)

   • Ray

   • Ray gradient (%)

   You can continue to work in the Part Studio normally while using Thickness analysis. The thickness evaluation will automatically update as you make edits.

7. To edit the Thickness analysis, click the Show Analysis tools icon () in the bottom right of the graphics area and select Edit thickness analysis from the menu.

8. To turn Thickness analysis off, click the Show Analysis tools icon () and select Turn thickness analysis off.

Rolling ball thickness method

The rolling ball thickness method calculates the size of the largest sphere that can be inscribed within a part at each point along the part's surface.

The sphere is tangent to the point of inspection and at least one other point upon the part (though it may be tangent to more than one part) and is thus said to roll along the part's interior while simultaneously changing size. The thickness measured is reported as the diameter of the inscribed sphere.

Tips

• The rolling ball thickness method provides a thickness measurement defined by localized, non-trivial geometric relations at more than one point within the region of interest.

• The rolling ball thickness distribution is guaranteed to be continuous across all regions of any solid part.

Ray thickness method

The ray thickness method calculates the distance traveled along a straight line path through the interior of a part.

At each point along the part's surface, a ray is projected normal to that surface, terminating upon first intersection at another point along the part. The length of the line segment between those two points is the ray thickness.

Tips

• A line projected normal to one point along the surface of a part has no guarantee of any geometric relation to the surface at its second point.

• The ray thickness distribution is seldom continuous across the entire part. It will contain sharp discontinuities, most obviously near sharp corners.

Thickness gradient (ray method or rolling ball method)

The thickness gradient measures how quickly the thickness of a part changes as one moves along the part's surface. The value itself is the ratio (A/B) of the following terms: 

1. The maximum amount that thickness could grow or shrink as one moves (nominally and instantaneously) in any direction from one point along the surface of the part, measured in units of length.

2. The nominally instantaneous geodesic distance traveled along said direction, measured in the same units of length.

The ratio is non-dimensional, non-negative, and presented as a percentage (%) out of convention.