CAD Craft

A resource to CAD Craft specialists, and a showcase of my work — in both material and virtual worlds

Part 2: Configurations & Modular Design

Following on our discussion in Part 1, I used a Gear Assembly to show the creation of size configurations for the Gear. In Fig. 1 below, you can see in the Configurations Tab that there are currently two configurations: the Default, and Medium. (I’m using screen shots because some of the feedback I received expressed concerns that the video went too quickly.)

 

Gear Wheel configuration tab #1

Gear Wheel configuration tab #1

 

In Fig. 2, I am creating a third configuration, Large. Note at the bottom there are two check boxes, the first of which Suppress Features, is very important. It provides a setting so that any features I create for this configuration are automatically suppressed in the other configurations, instead of me having to do it manually. You can also designate acolor for each configuration, which makes it simpler to recognize different configurations at the assembly level, which is particularly handy when the difference(s) between configurations is not immediately obvious. This applies at the part & assembly or subassembly level.

 

Gear Wheel configuration tab #2

Figure 2: Gear Wheel configuration tab #2

 

Fig. 3, the sketch for the primary extrusion of the wheel disk is open, showing me modifying the diameter dimension. You will note that on the dimension dialog, there is a tab selected, opening a flyout allowing me to specify which configuration this diameter is to apply to.

 

Gear Wheel configuration tab #3

Figure 3: Gear Wheel configuration tab #3

 

In Fig. 4, you can see the new Gear configuration inserted into the assembly, showing the color and contrast in sizes.

  

Gear Drive assy with one large & one small gear

Figure 4: Gear Drive assy with one large & one small gear

 

In Fig. 5, if you look at the first instance of Gear in the Component List, you will see the configuration shows up inside (). The number inside <> designates the number of instances of that part in the assembly.

 

Selection of Component Properties in flyout

Figure 5: Selection of Component Properties in flyout

 

In Fig. 6, the Component Properties dialog is open, showing the selected configuration.

 

Component Properties dialog box showing configuration selection

Figure 6: Component Properties dialog box showing configuration selection

 

This shows the basic implementation of creating and using configurations at the part & assembly level in SolidWorks. Basic ‘engineering best practices’ speak to  certain strategies & tactics — the vison/perspective needed to creatively solve design challenges, and the steps to implement that vision. In prior posts I have spoken to the pre-design stage of contemplating the design, machining/fabrication & assembly challenge(s), as crucial to the planning process.  This important phase can go a long way in streamlining and quickening your design process. For instance, recognizing the impact of the differences between additive fabrication approaches like 3D printing, and regular reductive processes like machining, such as a lathe can be critical to certain steps needed by one and not the other. This phase of contemplation is one of the seed stages of the development of your craft as a CAD master.

This applies here in the context of how a given part is created. In the case of the gear teeth, you can see there is a tapered cut on each side of the disk. When I first created the gear, before I added the configurations for this demonstration, I had simply dimensioned the sketch from the origin, as shown below in Fig. 7.

 

Gear sweep cut sketch detail

Figure 7: Gear sweep cut sketch detail

 

In this sketch, you can see the top line along the edge of the tooth shows black, as fully defined. Instead of dimensioning it to the origin/center line below, I simply selected the edge, and converted it to a line in the sketch, which makes it’s relation “On Edge”. The advantage of this is now, no matter how I vary the diameter of the gear, the sketch will move with it, and I will get no error messages. This is far easier than the alternative of inserting new dimensions for every configuration. This is where the foresight mentioned above begins to pay dividends.

Part 3 I will further discuss how this all fits into the modular design concept.

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