Configurations – What Are They Good For? Here’s a Few Things
SOLIDWORKS users may have been able to avoid using Configurations in the twenty or so years it has been around, but the often-overlooked ability may actually serve a purpose. Let’s take a look at Configurations with an open mind to get a complete understanding and look for benefits, both real and perceived.
Here is what Configuration is according to the SOLIDWORKS Help:
“Configurations allow you to create multiple variations of a part or assembly model within a single document. Configurations provide a convenient way to develop and manage families of models with different dimensions, components or other parameters.”
Essentially, configurations act as files within a file. Configurations are usually made of parts and assemblies that have significant commonalities. For those that have taken the SOLIDWORKS Essentials training, the Pin part, with its long and short configurations, is a simple example of this commonality. While the pin part may vary in length and perhaps diameter, it is still basically a cylinder.
We could create individual parts for each possible size of the pin, but this can be time-consuming and very tedious. Tracking and organizing all those individual pins can also be challenging especially if your organization is not using some sort of data management software. (By the way, organizing files in Windows Explorer folders, with some master list somewhere that lays out the structure of the Windows Explorer folder is not data management. That form of organizing files is an anachronistic behemoth that is just waiting to self-implode.)
And that pretty much sums up configurations. They work best with common parts because configurations make it easier to create new variations and make organizing these files simpler. It must be noted that modern data management software can also simplify the creation and organization of common parts without the need for configurations. More on this later.
Now that we know what a configuration is, let’s look at the mechanics of configurations. Configurations can be accessed from the top of the SOLIDWORKS Feature Manager in an open SOLIDWORKS part or assembly. By default, Configurations are located under the third tab.
Configuration Tab of Feature Manager.
Every single part or assembly will contain one configuration, aptly named the ‘default’ configuration. Additional configurations can be created in several ways, including the creation of some features. For example, inserting a Weldment feature will result in two configurations: one a parent, the other the child configuration, which is also known as a “derived configuration.”
At its most basic, each configuration can be created manually from the right-mouse menu.
Manually creating a configuration.
Creating each and every configuration manually is laborious and unnecessary. Toiling through the creation of dozens or perhaps hundreds of configurations would be a merciless grind. Luckily, SOLIDWORKS realized this early on and allowed the use of Microsoft Excel to streamline the process.
Spreadsheets, with their ability to cross-reference rows and columns, can significantly reduce the onerous task of creating multiple configurations. Mind you, entering reams of configurations can still be quite mind-numbing, suitable only to those who enjoy data entry.
These purpose-built Excel Spreadsheets are called design tables. Design tables work by entering the proposed configurations in column A. Subsequent columns define what will be controlled by the proposed configuration. Where the cells of the proposed configuration intersect the cells of the configurable items, we add values. Using the pin part again as an example, where the ‘long pin’ configuration intersects with the ‘length’ column, we can specify the physical length of the Pin.
We would likely not create a design table for a couple of configurations that contain only a couple of configurable items, but we do it here to provide an easily understood example. Design tables are at their best when a SOLIDWORKS component contains several configurations and/or several configurable items.
More than just dimensions can be structured with configurations. Below is a list of all the available configurable items as recorded in SOLIDWORKS Help:
Base Parts in Configurations
You can control the configuration of a base part with a design table. This is available in part documents only.
Color Parameter in Configurations
The design table can include a column for configuration-specific colors. The value is a 32-bit integer that specifies RGB (red, green, blue). If you do not specify a value, zero (black) is used.
Comment in Configurations
The Configuration Properties PropertyManager has a Comment box, where you can enter information about the configuration.
You can specify which configuration of a component is used in various configurations of an assembly.
Component Part Number in Configurations
When you create configurations with a design table, the software automatically sets options in the Configuration Properties PropertyManager.
Cosmetic Threads in Configurations
You can configure callouts for cosmetic threads.
Derived Configurations in Design Tables
You can control derived configurations in a design table.
Description in Configurations
The Configuration Properties PropertyManager has a Description box, where you can enter a description of the configuration.
Display States in Configurations
You can create multiple display states for each configuration of an assembly or part.
End Conditions in Configurations
You can change the end condition of extruded features in specified configurations.
Expand in BOM in Configurations
You can control how the assembly is listed in a BOM, when this configuration is used as a subassembly.
External Sketch Relations in Configurations
You can set different external sketch relations in specified configurations.
Shortcuts for Suppressing Items in Design Tables
The string values suppressed and unsuppressed are valid values for selected design table columns. You can use shortcuts for these string values in design tables.
Fixed or Floating Position in Configurations
You can configure whether the position of a component is fixed or floating in an assembly.
Global Variables in Configurations
You can configure global variables.
Hole Sizes in Configurations
In the Hole Specification PropertyManager, you can configure the size of Hole Wizard holes by clicking Configurations and selecting This Configuration, All configurations or Specify Configurations.
Lighting in Configurations
You can suppress and unsuppress (turn off and on) lights in configurations.
Mass Properties in Configurations
You can configure values that you assign for mass, center of mass and moments of inertia in parts and assemblies.
Materials in Configurations
You can configure materials for parts and for bodies of multibody parts.
Scale Features in Configurations
You can configure the X, Y and Z scale factors.
Sketch Dimensions in Configurations
You can control the driving state of sketch dimensions in specified configurations to control the behavior of your model.
The plane on which a sketch lies is configurable through the Sketch Plane PropertyManager. You can place a single sketch on different planes in different configurations.
Sketch Relations in Configurations
You can control the suppression state of sketch relations per configuration.
Split Parts in Configurations
You can control the configuration of a split part with a design table. This is available in part documents only.
User Notes in Design Tables
The design table can include additional columns or rows for information only (notes, intermediate calculations and so on).
The use of design tables does require Microsoft Excel. Not every SOLIDWORKS user can be expected to have Excel, however, so SOLIDWORKS introduced Modify Configurations. Modify Configurations consists of four branches. Each branch is available by right-clicking on a related object as follows:
- Configure Feature – right-clicking a feature.
- Configure Dimension – right-clicking a dimension.
- Configure Component – right-clicking a component in an assembly.
- Configure Material – right-clicking a material in the Feature Manager. Materials can also be configured from the material dialog box.
In the Modify Configuration dialog box, the item to be configured will be displayed in a table similar to an Excel spreadsheet. Additional configurable items (i.e., a dimension) can be added by double-clicking on the item in the modelling area. The items to be configured are displayed along the top row of Modify Configuration dialog box. The configurations to be generated are entered and displayed down the left column. Potential configurations can also be renamed and deleted by right-clicking on the configuration.
Modify Configuration dialog box.
Modify Configuration can be used to only create configurations, but the configurations can be saved in a table view for future access.
Save table view.
While Modify Configuration does in make design tables unnecessary in many ways, it does not completely replace them. Some SOLIDWORKS add-ins, such as Routing, rely on design tables. Also, design tables can be shared and/or referenced between multiple SOLIDWORKS documents.
Another utility that requires design tables is the SOLIDWORKS Configuration Publisher. The Configuration Publisher makes it possible to access a configuration by selecting from predefined parameters.
Configure Component dialog box.
At the beginning of this article, we mentioned that it is often faster and easier to add configurations than it is to model a new part from scratch. We looked at the pin part from the Essentials course as an example of how we can vary the size of a part by using configurations. A pin is a relatively simple part. With more complex parts, there is greater potential for time savings through the use of configurations.
Based on what we have looked at so far, we may be tempted to say that configurations should be used universally for components that share some commonality. But like everything else in CAD, there are always compromises and shortcomings.
Configurations can cause bloating of files. Each configuration needs to store information on how it differs from the other configurations, and all of it is stored in the SOLIDWORKS file. The more configurations, the bigger file. The bigger the file, the more time it takes to load or rebuild it. If you have a fastener with thirty configurations used a hundred times in an assembly, that is 30 x 100 things that have to be reloaded and rebuilt every time. This will impact performance.
There is a tool to shrink those bloated configuration components. In SOLIDWORKS System Options, you can choose to purge cached configuration data in the Performance section.
SOLIDWORKS system options.
This will purge a fair chunk of the cached configuration information. But this, too, comes at a cost. When switching between configurations, all of the configuration information that was stripped away must be rebuilt when switching configurations. You can have better performance with opening files or on switching between configurations—but you can’t have both.
Since configurations can make creating similar parts easier, many designers use configurations to design whole groups of parts. The problem with this strategy is that these groups of parts are not individual files. If you have assemblies or drawings that reference these different configurations that are all contained in a single file, which assembly or drawing does that file belong to? This use of configurations can make managing your data difficult. While this approach may save time in the near term, it can be much more costly in the long run. As I tell my SOLIDWORKS Essentials students, short-term gain can lead to long-term pain.
Besides, tools such as SOLIDWORKS’ Pack & Go, or SOLIDWORKS PDM’s Copy Tree, make it easy to create new similar parts. Most importantly, these are separate files that can be unambiguously referenced by an assembly or drawing.
I follow a simple rule when determining if individual files are required. If the form fit or function differs, then a separate file is needed. To simplify that even further, if there is a different part number, it’s a new file.
A perceived and misguided advantage of configurations harbored by some is that configurations facilitate data management. These people state that instead of having thousands of parts, a company can have much fewer parts with several configurations. This theory is often held by those that consider Windows Explorer as a data management tool. However, Windows Explorer lacks the functionality to truly organize a company’s design data. Since most companies’ design data is their lifeline, should it really be entrusted to such a basic tool?
With SOLIDWORKS Workgroup being available since the early 2000s, why would a company choose to be bogged down with an unwieldy Windows Explorer folder structure? While Workgroup was clunky, it still beat having to create configurations to tame the data monster. What’s more, Workgroup had decent search capabilities, access control, automated revisions and rudimentary lifecycles. These are things that are not part of a Windows Explorer environment.
With SOLIDWORKS PDM, SOLIDWORKS users have access to a more powerful data management tool. Like SOLIDWORKS Workgroup, each seat of SOLIDWORKS Professional and Premium ships with a seat of PDM Standard. This means that many companies already have a decent data management tool just waiting to be deployed.
At this point, you may be wondering if configurations have any use at all. In the right environment and used for the right application, configurations can still be a useful tool. Configurations lend themselves best to library or common components, that are not revision controlled. These are often purchased components such as fasteners. Ballooning file size is still something that needs to be managed, but with the application the SOLIDWORKS System Opens options discussed earlier, file bloating can be diminished.
In summary, do not let this article persuade or dissuade you from using configurations. Think of it as thorough look and an informed opinion, if anything. Its up to you to do your homework. See if configurations work for you in your particular situation, whether they are an advantage or an impediment.
Learn more with the eBook Gain Competitive Advantage with Product Data Management.
About the Author
Joe Medeiros is an Elite Applications Consultant at TRIMECH, a premier SOLIDWORKS reseller, servicing customers throughout North America, offering SOLIDWORKS customers expertise in implementing and using SOLIDWORKS solutions.
Joe has been involved in many aspects of the SOLIDWORKS product family since 1996 and as an award-winning blogger, he regularly writes about SOLIDWORKS solutions.