First of all, model the component according to the dimensions shown below. Finally save the model as Flange-cutaway.

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1 Configurations In the following tutorial we will look at using configurations. Configurations may also be used to create different versions of a component for display purposes. Configuration may also be used to create different variations of the component itself. In this section we will create a cutaway version of a component and a full version of the component. First of all, model the component according to the dimensions shown below. Finally save the model as Flange-cutaway. Save a second copy of the component as Flange-Variants using the Save as copy option for use later. 1

2 Creating display configurations Having created the model, now create an extruded cut to form the cutaway feature; then suppress this feature. You are now ready to create your first configuration. To create a configuration select the configurations tab at the top of the feature manager. With the component in its full state, right click on the Default configuration and select Add Derived Configuration When prompted add Full as the configuration name then choose accept. Full is now the currently active configuration. Next save a new configuration called cutaway by again right clicking on the Default configuration and selecting Add Derived Configuration This time type Cutaway as the configuration name. Cutaway is now the current configuration. Any changes we make now will apply to this configuration only. Next, un-suppress the cutaway feature. (Changes apply to the currently active configuration only). You now have two configurations. We can now alternate between configurations by right clicking and selecting Show Configurations. Alternately we can double click on the configuration required. 2

3 Displaying different configurations in draft mode Having created different configuration of a component we can now display different configuration of the component simultaneously in draft mode. When inserting a view into a drawing we can select which configuration we want to display. First of all create a new blank draft document. We will now insert an ISO view. In order to create an isometric view of the Full configuration select model view from the view layout toolbar. Next browse and select the relevant model and choose the next button In the reference configuration section, choose the Full configuration and select Isometric as the orientation. Repeat the process again this time selecting the cutaway configuration. Complete the drawing by creating a plan, elevation and sectional end view of the full component. Save drawing as Flange-cutaway.slddrw. 3

4 Using configuration to create product variants We will now use configurations created by a Design table to create a number of product variants. First of all open the component called Flange-Variants saved earlier. In this exercise we will create a number of versions/configurations: Version Tube ID Tube OD Flange OD PCD No Holes Thickness Light Medium Heavy The existing model corresponds to the smallest of the 3 variants shown above. All variants have a common internal diameter of 30mm. Dimensions are such that they cannot readily be defined using equations. We will now create the other variants, medium and heavy using a design table. Creating configurations using Design tables Where a small number of variants are required it is sufficient to manually adjust each dimension or parameter and save each configuration in turn. However where several variants / configuration are required it is useful to create a design table. To create a design table choose Insert Tables Design table For the source use the Auto-Create option. If prompted to select dimensions to add to the design table select all then OK. The table which appears contains all critical dimension and any other relevant parameters. 4

5 To add other variants simply add the variant name and all relevant dimensions. For the light version add the name light as shown and copy all values from the default line (since the light variant corresponds to the current or default size). To create the other variants. Simple type the name of the variant (this will become the configuration name) then type in each new dimension / parameter value. The D2@ syntax for naming dimensions does not make them particularly recognizable however you should recognize each dimension and what it does from its default value. N.B. As each of you may have a slightly different approach to model your component the table will more than likely be different from that above. To exit the design table just click in the Solid Works graphics area. On exiting the design table you will be presented with the message. The design table generated the following configurations. Select OK to continue. This will generate the three configurations as shown. Note also the presence of a new category of Tables containing the Design Table just created. All modifications to the design table are carried out by right clicking on this feature and selecting edit table. 5

6 This results in the three configurations shown below. As can be seen, the holes on the medium and heavy configurations are quite close to the edge. We will now modify the design table to place the holes more centrally on the flange portion of the component. To do this, change the PCD to 90 and 100 on the medium and heavy components respectively. To do so right click on the Design table and choose Edit table. This will open the table in the graphics area as seen earlier. (Alternately you may edit the table in a new window. This will open the table stand alone in Excel) Exit the design table. This will modify the configurations as required. Finally create draft views of each configuration in a single sheet. NB. If you accidently exit the design table (e.g. if you select a point outside the table) you can open it again for editing by right clicking on the design table and choosing Edit table. 6

7 Assignment In the following assignment you will create a number of hand-wheels. Each hand-wheel is similar in general design but different in terms of overall dimensions and number of spokes. Below are the critical dimensions. Version Hub Dia Hub Thk Wheel Diameter Rim Diam Spoke Dia No. Spokes Small Medium Large V-Large Sizes and numbers of spokes are such that they cannot be readily be related by equations. Fillet radius = 2mm Assignment Model the basic wheel then using configuration and or design tables create the four versions as configuration within a single part documents. Create a draft containing an isometric view of each configuration. 7