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Assembly Visualization Will Save You Many Times Over

CAD

Assembly Visualization Will Save You Many Times Over

Introduced in 2012, Assembly Visualization is a commonly overlooked assembly assessment tool. The Assembly Visualization tool can help you visually convey important trends of your model, identify and correct missing information and help you quickly locate components that may be adversely affecting your assembly’s performance.

How to Access and UI

First and foremost, the Assembly Visualization tool is only available in SOLIDWORKS assembly files. You can find this tool nestled in the middle of the Evaluate tab of your Command Manager, as well as under Tools > Evaluate > Assembly Visualization. The Assembly Visualization user interface is now on the left in the Feature Manager Tree Panel in a new tab.

Figure 1. Accessing Assembly Visualization and its default display.

Once launched, the component colors in the assembly will have changed to a gradient of reds to blues. Don’t panic, these colors are temporary while the tool is active. When the Assembly Visualization tool is launched for the first time on an assembly, the default colors will be a red to blue gradient comparing each component by mass, yet the list will be sorted by File Name.

Dismiss this tool using the red ‘X’ in the top right in this new tab (next to the question mark) or by selecting the tool again on the Command Manager. Saving this assembly will save any customized Assembly Visualization columns, color and display parameters.

User Interface Mechanics

First, let’s quickly introduce some user interface elements before we combine them into making something useful for your assemblies.

Colors

Naturally, you will want to utilize different colors. Double-click a slider on the left or right, then mouse click on a slider and select Change Color. To insert an additional slider, left click on the region to the left of the color bar. To toggle the temporary AV colors on and off, left click the color bar.

Figure 2. User Interface – Colors.

The sliders will shift colors to the next slider above or below it. Dragging a slider up or down on the left will sustain that color for components as you move away or towards an adjacent slider.

To create a custom discrete color scheme, you will need to add sliders to effectively act as bookends between appropriate rows. In Figure 3, by default R1 and B2 are at the top and bottom of your list, and the rest were added manually. R2 is added to sustain the red color for the first three rows. G1 is added to establish the start of green just below R2 and above Yoke Half. Meanwhile, G2 is added to sustain the green color for three components. Right up against G2 is B1, indicating the start of blue just above Hand Rail (Formed). Since B2 is at the very end of the list, all components between B1 and B2 will be a uniform blue.

Figure 3. Example of additional sliders for manual discrete color schemes.

To automatically create a discrete color scheme for an appropriate Custom Property, right click a slider or right click the area where you would add a slider and select “Group Identical”.

Figure 4. Example of Group Identical color scheme.

Sorting and Columns

Clicking on the column header name (such as File Name, Quantity and Mass) will sort this list by ascending or descending order in the same manner as any typical column you’d find in Windows Explorer.

To change the column attribute, select the right-pointing arrow of a column header and choose “More…” and then your desired attribute from the Properties dropdown list. This list is populated from three sources: SOLIDWORKS Sustainability (the full version, not SustainabilityXpress), Mass Properties and Custom Properties.

Figure 5. Changing column attributes for sorting.

Control the Appearance of Your List

Figure 6. Customizing results.

  1. Show/Hide Value Bars: Toggle the visibility of the blue bars shading the file names in the File Name column.
  2. Flat/Nested View: Have the File Name column reflect the file names visible in either a fully collapsed Top-Level Assembly Feature Manager tree (“Nested”) or a completely itemized list of every component just like a “parts only” Bill of Materials table (“Flat”).
  3. Grouped/Ungroup: Useful in the Flat view where instances of a part file might reside in different subassemblies, so instead of seeing a Quantity column consisting of all “ones,” when you choose the Grouped view, it will group all similar configurations of a part file and list the appropriate overall Quantities.
  4. Performance Analysis: This is a Large Assembly diagnostic tool introduced in 2018, and will be explored in-depth later on in this article.

Use Cases

Changing Column Categories and Display States

The assembly can be visually sorted per any custom property, as mentioned previously. For example, the assembly can visually convey the different revisions of the subassemblies and components referenced at the top level. This example combines changing the referenced column to Revision, toggling the Flat/Nested view button to view top-level subassemblies, right clicking a slider and indicating “Group Identical,” as well as the typical RMB on a component and selecting “Change Transparency.”

Figure 7. Example 1: Combining multiple UI elements to capture revision.

Better yet, this Revision custom property is driven by workflow actions in SOLIDWORKS PDM.

Figure 8. SOLIDWORKS PDM Windows Explorer view of project files.

If the Revision Custom Property is not utilizing SOLIDWORKS PDM, the full list of the revisions can also be exported as an archive list of how the Revision property matures from concept design to production. Select the right-pointing arrow in a column header > Save As… to export the list as either an .xlsx, .xls, .txt, .csv or .pdf.

The visual settings in their current state can be captured in a Display State. Select the right-pointing arrow in a column header > Add Display State, as in Figure 9 below.

Figure 9. Menu for Add Display State and Save As.

After selecting “Add Display State,” it will appear as though nothing happened. However, the command will create a new Display State in the Configuration Tab. Feel free to continue to edit this new Display State just like any other (rename it, manually adjust colors, hide/show components, etc.). The Assembly Visualization tool will not constantly update this recently captured Display State; rather this new Display State is simply a visual snapshot in time of what the model looked like upon executing the command “Add Display State” from the Assembly Visualization menu.

As the model develops and matures through the design process, selecting “Add Display State” again will append a new Display State as the latest visual snapshot of revisions to easily compare with an older capture.

Figure 10. Display State created from command within Assembly Visualization.

Add Additional Columns, Sort Hierarchy and Editing Custom Properties

The Assembly Visualization tool allows for a total of seven columns. Since the first two (File Name and Quantity) cannot be deleted, the user is only allowed to add and customize an additional five columns.

Figure 11. Add additional columns for secondary sorting.

Figure 12. Sorted by finish, with SW-Material no longer contributing to sort.

In Figure 12, notice the SW-Material column is missing the tiny up/down sorting arrow. In order to set up a primary, secondary, tertiary, etc. sorting system, the column must be included in the sort hierarchy by right clicking on the column header and selecting “Add to Sort Hierarchy.”

Figure 13. Adding a column to sort hierarchy.

When there are multiple columns added to the sort hierarchy, the sort priority starts at the left and descends towards subsequent columns to the right (only columns which were also added to the sort hierarchy). The left-most column will be tinted and is the column driving the color scheme mapped onto the assembly in the graphics area. Dragging column headers to the left and right will adjust the primary, secondary, tertiary, etc. sort order.

Figure 14. Primary sort = SW-Material; Secondary sort = Finish.

Commonly, a Bill of Materials table can be used to identify missing custom properties for a component or subassembly. Then it is up to the user to open the file, add the custom property (maybe it’s missing!) and populate the entry field.

With the Assembly Visualization tool, updating and adding the custom properties of a file is a seamless workflow. In Figure 14, Handle Mount Locknut in row 4 does not have a value for the Custom Property “Finish”.  An even bigger plot twist is that this part file is missing the Custom Property “Finish” altogether. By simply double-clicking the empty cell and entering in a value (Figure 15), the Assembly Visualization tool will simultaneously create the Custom Property and enter in this value (Figure 16).

Figure 15. Adding and updating a custom property.

Figure 16. New Custom Property added and updated by Assembly Visualization.

Similarly, the material assigned in the component’s Feature Manager tree can be updated by selecting the right-pointing arrow at the end of that cell. If the part file has multiple bodies with dissimilar materials assigned to them, this SW-Material field will show three asterisks (***). Hover over the asterisks for a popup list of all materials referenced across the multiple bodies.

The Assembly Visualization tool cannot assign different materials to different bodies. Editing the material for a multibodied part file in this manner will assign the new material to all bodies.

Figure 17. Edit Materials in Assembly Visualization.

Investigate Your Results

In this example, the primary sorting column is adjusted to be the Surface Area custom property because there’s interest in which components require the most paint.

Figure 18. Discrepancy in expected surface area.

The results look pretty, but upon a closer look we notice the Surface Area reported for the Yoke_male component is over 250x larger than the bracket_& component. I know the Yoke_male component does not have detailed threads or is secretly a heat sink with fins, so I open both component files in their own windows and discover the documents are utilizing different units:

Figure 19. The culprit = Units.

Selecting “Options…” in the Mass Properties of the bracket_&.sldprt and updating the length to a custom setting of millimeters did not change the result in the Assembly Visualization tool. The units had to be adjusted at the part document level (Tools > Options > Document Properties > Units) or by swapping to the appropriate units in the bottom right corner of the part window:

Figure 20: Quick units swap in the status bar.

Upon applying this fix, the results of the Assembly Visualization tool automatically updated as soon as the assembly file was brought back into primary focus. The Yoke_female and crank-shaft had the same issue with units and the bracket_&.

With units finally consistent across the board, the results of the Assembly Visualization tool look far different from its initial launch and are now correct and ready for downstream reference.

Figure 21. All issues captured to show correct Assembly Visualization results.

Performance Analysis

The release of SOLIDWORKS 2018 came with an enhancement to the Assembly Visualization tool called Performance Analysis. This enhancement arrived in the form of a single button to automatically generate three columns which can help identify inefficient components. This enhancement can also be launched by selecting the right-pointing arrow in a column header, then choosing Performance Analysis.

Figure 22. Performance Analysis and Auto-Generated corresponding columns.

  • Total Graphics Triangles: All geometry in 3D space can be approximated by graphics triangles. Higher values in this column can be an indication of either excessive curvature detail or that the Image Quality slider is too close to the “High (slower)” setting. Files downloaded from external sources commonly come with excessive detail (embossed logos, threads, imported sketches with discretized segments, etc.) and will likely end up high in this sort list.
  • SW-Open Time: An indication of how long it took SOLIDWORKS to open the bits and bytes from wherever this file is stored. Working locally (like in SOLIDWORKS PDM) is ideal and will keep the values in this column to a minimum, but this column may yield significantly greater numbers for a referenced component being dragged through a busy Local Area Network (LAN) or over VPN. Once the file is open, this column isn’t of any further particular use.
  • SW-Rebuild Time: How long it takes to rebuild this component in its own window.

In the example image above, the component Handle Battery Cover is taking over 13 seconds to rebuild. It is up to the user to investigate why and exercise their engineering judgement about what can be done about this. Upon opening the part file and choosing Evaluate Tab > Performance Evaluation, it appears that a single feature is consuming 88 percent of the total rebuild time.

Troubleshooting reveals that the sketch referenced by the feature Cut-Extrude1 has a sketch entity referencing a complex edge from a non-SOLIDWORKS native imported solid. Deleting the references to the imported geometry and finding an alternative solution to fully define the sketch decreased the rebuild impact of the Cut-Extrude1 feature significantly.

Figure 23. Before and after edits of “Cut-Extrude1” feature.

An alternative engineering decision could be to create a configuration which suppresses any overly heavy features or leaves the component out of the assembly entirely.

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