Documenting Part Configurations in a Drawing

This video shows you one way to document a number of different part configurations on the same drawing, using Custom Properties to capture the dimensions that change across the configurations, and a BOM in a drawing to display those dimensions.

Assembly rebuild times and AssemblyXpert

This video illustrates how to use SolidWorks AssemblyXpert and Assembly Visualization tools to analyse rebuild times in your assembly.

AssemblyXpert analyses performance of assemblies and suggests possible actions you can take to improve performance. It also provides you with information about your assembly.

The AssemblyXpert is available in any assembly file and can be accessed from Tools >> AssemblyXpert, or from the Evaluate Command Manager tab.

It performs a number of diagnostic tests in the background, and will present options to correct any issues if they are present (click on the names to view detailed descriptions from the SolidWorks Web Help):

• Display Speed
  
  • Is the display speed too slow during dynamic operations such as moving components or rotating views?

• In-Context Part Performance
  
  • Does evaluating a component during rebuild take too long?

• In-Context Circular References
  
  • Do any components have circular references?

• In-Context Relationship Performance
  
  • Are any components rebuilt multiple times when the assembly is rebuilt?

• In-Context Relationship Conflicts
  
  • Does a sub-assembly component have an in-context relationship to a component that has more than one configuration in the current assembly?

• Components Far from Origin
  
  • Are any components significantly far from the assembly origin?

• Verification on Rebuild
  
  • Is Verification on rebuild turned
    

It also shows:

• How many components in the assembly have been saved to the latest SolidWorks format

• The number of components in resolved, lightweight, Speedpak or suppressed states

• How many mates are evaluated in this level of assembly

• Rebuild time of the full assembly

• Information regarding the structure of the assembly including:
  
  • Total number of parts
  • Number of unique parts
    
  • Maximum depth (how many levels of sub-assemblies there are)
    
  • Number of bodies

The rebuild time of the assembly is a new feature in SolidWorks 2011. Clicking on the glasses icon will show the rebuild time for the assembly, broken down into sub-assembly rebuild time. Part rebuild times, in-context relationships between parts, and mates all contribute to the rebuild times shown. You can use these times to optimise those features that contribute most, such as reorganising mates.

Also notice that the top level assembly is included last in the list, as the mates in this assembly need to be re-evaluated after all of the sub-assemblies have been rebuilt. This ensures any changes from the rebuilds are accounted for in the top-level mates.

You can use these rebuild times to benchmark computer performance. Each computer will rebuild a given assembly at a different speed, so you can use a typical assembly that you work with to evaluate computer performance relative to each other. Make sure you are using the same performance options to ensure comparable results.

You can also use the information regarding the number of parts to work out how complex an assembly is. I would consider an assembly with 200 to 500 parts or more a “large assembly”. The uncertainty is based on the complexity of the parts (are they made of simple extrudes, or complex surfaces?) and/or whether those parts have multiple bodies. Check the number of bodies in the assembly to see if some parts contain a large number of bodies – for example large weldment parts, or assemblies that have been saved as a part will both be counted as one part, but contain many bodies. You can use these factors to help determine the “Large assembly mode” threshold.

Configuring the SolidWorks Toolbox

The SolidWorks Toolbox is a database of commonly used fasteners and parts, available if you have SolidWorks Professional or Premium. You can customise the Toolbox with your own part numbers, descriptions and other fields you may wish to show on a Bill Of Materials.

This video shows you how to customise the Toolbox to reflect the fasteners you use in your designs, and how to quickly add a large number of properties to those parts using Microsoft Excel.

The Toolbox runs off a database which contains all of the available sizes and dimensions for each part it contains. When you select a certain component for the first time in SolidWorks, it generates that particular configuration or part based on the dimensions contained in the database. If you wish to change the size of an existing Toolbox component, and the new size has not been used before, you need to RMB on the part (on-screen or in the Feature Tree) and select “Edit Toolbox Definition”. This will open the same original Toolbox Property Manager box, and generate the new config when you press OK.

Alternatively, from the Toolbox Configuration window, from the same button where you export settings to Excel, you can choose to "Create configurations" to generate all configurations for the component. This means you can use the ordinary method of changing configs in the assembly. But be careful using this – I did it on the bolt in the video with 198 configs and the result was a 25Mb part file. If you choose to do this, make sure you remove unnecessary bolt sizes and lengths first - you can always add them back in later.

SolidWorks Pack and Go overview

File >> Pack and Go collects all referenced files (parts, drawings, sub-assemblies) from your assembly and drawing files. It's a great way to duplicate a project if you need to make changes to the design, or move files between computers - you can even create a zip file directly from the dialog box.

You can also use Pack and Go to rename individual files and their destinations (by double-clicking in the respective fields), or you can use the Select/Replace... button to make bulk or batch changes to all of your files - e.g. replacing a specific text string such as a Job number from every single file with a new one.

Pack and Go will create the new files while maintaining file references between all of your part, assembly and drawings, even if names and folder structures have changed.