It's just like the other one, but...

“Just like the other one, but with a few changes”, that’s what I became used to hearing my boss say all the time when talking about our next assignment. “The super-heater for boiler 2 is very similar to the one for boiler 1, only the following is different…”, or “This boiler is exactly like the one we serviced in Cosamaloapan, but…”, or my favorite one, “I would like to see the same arrangement of tubes, but bent at different angles. I want to compare. We could even reposition the dome…”.  I guess what I needed back then (besides SolidWorks) was the ability to create different configurations of the same thing, so my boss could knock himself off asking for changes!

Configurations are simply variations of the same model in which dimensions are changed, features suppressed, colors and other properties changed. All this inside one same document! Configurations can be created manually or through the use of a design table. You can create configurations for parts and also for assemblies.

My first experience with configurations was that simple model created in one of the SolidWorks tutorials. The one that didn’t turn out all that great the first time because my sketch was underdefined, remember? That particular example illustrated the use of configurations and design tables to change the dimensions of the model. In the configuration manager you can see four configurations that were created using the design table. You can also see the model, with its original dimensions, that appears as the “default” configuration.

All the configurations share the same features, but their dimensions are different. Take a look at configuration number 4, for instance.

A design table is used as an aid in driving the dimensions for the different configurations. This is especially useful when you have several configurations!

Configurations and design tables can also drive other things about a model, such as the number of instances in a pattern, colors, and even what features (or components in the case of an assembly configuration), get suppressed.

Well, I just had to experiment with this, so I created a little model of my own and several configurations for it,  by means of suppressing features in some of them. You can tell by the model of choice that I was probably thinking about updating my wardrobe. My husband, on the other hand, still hopes I was actually thinking about starting Spring cleaning early this year.

Anyway, this is my default configuration for the model. It’s the one I created first and all the features in this default configuration are shared by all the other ones. Notice how there are features that have been suppressed in this configuration and appear in gray. It means that they are not solved for this particular configuration, but they still are part of the feature manager design tree because they are solved in other configurations of the same part.

Creating a new configuration manually is really simple. All you have to do is go to the configuration manager and RMB click the name of the part. In the menu that opens, choose “Add Configuration”. This opens the Add Configuration dialog box, where you can assign a name to your configuration, add a description and comments to it, decide in which way it will be displayed in the bill of materials (under the document name, configuration name or any other you decide), and even assign a specific color that will apply to that configuration only. You can also create derived configurations under each configuration, by RMB clicking the name of the configuration and following the same procedure. The configurations created in this fashion display a little cubic symbol next to their name, while the ones created or managed by means of a design table display an excel symbol. 

Once you created the new configuration (and make sure it’s still the active configuration) you can begin making changes to that configuration in particular. The new features you add to it will only apply to that configuration and will be suppressed for the rest, unless you specify otherwise whenever given the option. Take a look at the dialog box for Cut-Extrude 1, for instance. At the bottom, there’s the option of choosing what configurations it will apply to. In my case, I chose only this one.

When a configuration is active, the symbol on the side of its name is displayed in color and the name of the model reflects the configuration in use. Notice in the following image that  “New Configuration” and the derived configuration “hanger –style 2 red” were created manually, while the rest of the configurations are managed through a design table.

In the above example, “New configuration” is the active configuration and this is what you would see in the feature manager. Notice how some of the features that were suppressed for the Default configuration are now unsuppressed, but Sweep 2, Dome 2 and Mirror 1 remain suppressed for this configuration.

This is the feature manager for the configuration “hanger with hooks”. For this configuration in particular, Sweep 2, Dome 2 and Mirror 1 are unsuppressed.

You can manually assign a material to your model and decide which configurations it will apply to. Unfortunately,   I don’t think you can drive materials through the use of a design table. That would be really helpful!

After having created a few configurations manually, I decided to add a design table to my part. You have a few options when first adding a design table. You can create one from scratch, allow SolidWorks to create one for you, listing all the configurations (if any) that you have created so far and all the parameters in your model that could be driven by the design table, or you can use an existing one (Excel document), if you have it. 

I chose auto-create and also chose to allow for any changes in my model (new configurations, new features, etc.) to be reflected as updates to the design table. This is what my design table looks like. Notice how in this design table I’m not driving dimensions but what features are suppressed and unsuppressed in each configuration in my model.

I’m still learning about what other things can be driven using a design table and what other creative uses they may have. So far, I think I’m getting the hang of part configurations. Assembly configurations are a different story, though.

Comments

[Devon T. Sowell]

Hello Gabi-

Good job on the Configurations.

However, I don't recommend Configurations for Custom Parts; off the shelf Parts like Nuts and Bolts, no problem.

Here are three simple reasons, there a a few more too;

Part Files with mutiple Configurations have large File Sizes. When used in Assemblies/Drawings, performance is not good.

Configuration Names; these remind me of AutoCAD "Layer" Names. To the person that creates them, they have meaning, to another User, they usually are very confusing.

Finally, the problem I've seen at many of my Clients is this; In a Drawing, and it's Views, How do you know "which" Configuration is Displayed and then, Is it the correct Configuration? How do you know? One of my Clients had an exsiting Assembly, each Component Part had mutiple Configurations,, the top Level Assembly had over 60 different configurations, each with a "vague" name. the Creator of this Assembly no longer worked there. No one knew which Configuration was the correct one!

Devon

[Devon T. Sowell]

I like to do this;

One file, with one Part Number, with one Drawing. Same with Assemblies too. This will reduce confusion and increase confidence.

Cheers,
Devon

[Gabi]

Hi Devon,

Hey, thanks for the comments! I can see your point about the file size and the confusion created over the names of configurations. I guess the names could be somehow documented, but it was interesting to see that, just like you said, when you create a drawing out of a part configuration, the name displayed is the one of the model, but nowhere in there says what configuration was used. Interesting...

[Devon T. Sowell]

I meant to say this;

"One Configuration, One file, with one Part Number, with one Drawing. Same with Assemblies too. This will reduce confusion and increase confidence.

Devon

[Jerry Steiger]

Gabi,

Devon brought up some very good points. For just those reasons I have often converted multiple configurations of a part into multiple parts when it no longer seemed to be worth the pain to stick with one part. But I still have a number of parts with multiple configurations, because it seems to be less pain to deal with the configurations than it is to deal with having multilple parts that need to keep most of their features in sync. As an example, if your coat hanger was made with interchangable inserts in a single mold, I would be highly inclined to keep it as multiple configurations.

Jerry Steiger

[Rod Uding]

I agree with Devon on the One Config, One File, One Part Number Scheme. In our office we have problems with files that have multiple configs like bar stock. If I need to add on to it and someone else is using it. I have to have them exit it or add the part I need to the config.

We do try to keep the configs if used to the least number possible if we do use them.

[Gabi]

Hmmm... This is a very interesting point, Rod! I don't have others working with me, so I don't get to experience the kind of troubles you have found with configurations. I would've never thought of that! So, I'm beginning to wonder, what is the real purpose of the configurations? I mean, if they cause confusion and bloat the file size and reduce performance, and cause all kinds of troubles when working as a team, why is it that SW was given the ability to create files with multiple configurations in the first place? Is there a way around all these issues?