From hand sketch to adaptive assembly with Solidworks

This blog is translated from German with DeepL.

In development work, we repeatedly encounter the situation where boundary conditions change and yet work continues in parallel and individual parts have to be detailed. This article describes the concrete task of transferring a hand sketch – using the example of a computer mouse – into the CAD environment. For the further processing of the individual parts Solidworks offers the command “Split”. Using a basic model, the individual parts can be split off and further processed in detail. The derived individual parts remain dependent on the basic model. In the basic model, the hand sketches are inserted as sketches and can be exchanged if necessary.

Figure 1: from the sketch to the “mouse

Importing the hand sketches as an image file

The option “Insert sketch image” must usually be activated separately and is not listed among the normal sketch commands by default. This function can be found via the menu “Tools/Sketch/Sketch image” (see Fig. 2).

Figure 2

For the hand sketch, the basic dimensions are sketched as an outline. After insertion, the sketch can be freely scaled, rotated or moved so that the part structure can be sensibly designed. The inserted hand sketch is then traced with suitable splines (equation or polynomial controlled curves) and defined sketch curves (see Figure 3).

Figure 3

Structure of the basic body

In this example, the aim is to build up the entire outer shell with bounding surfaces. The hand sketches in side and ground plan serve this purpose. The geometry is completely defined so that later adjustment and documentation can be done without problems. The picture on the left shows the upper bounding surface defined by 6 sketches, all of which can be modified individually (see Fig. 4).

The image on the right shows the finished outer shell with the cut surfaces (orange and blue) for splitting off (see Fig. 5).

Figure 4                                                                                                                                                                                               Figure 5

Split off parts

The command is located under “Insert/Features/Split”.  Because in this example the body is divided into several parts (lower shell, upper shell, right mouse button, left mouse button) the command is applied several times. If all three cut surfaces are selected in one step, the body is completely split by default, in this example into 8 individual bodies (see Fig. 6).

The split-off parts are associative to the basic body and are saved as new parts. However, they can be processed individually for further detailing. Subsequent operations such as, in this example, injection-molded design, fasteners, etc. can now be introduced.

The resulting parts are then assembled to form the complete assembly. The origin of the split-off parts corresponds to that of the basic body. This means that even complex bodies can be easily linked together and their position in the assembly can be easily controlled.

Figure 6


If the situation arises that, for example, the dimensions or the separation of the parts must be changed due to design changes or the customer’s wishes, these adjustments are made in the basic body.

Adjustments to the basic body are passed on 1:1 to the derived parts. For example, the unfavorable separation in the recessed grip can easily be corrected later or during the development of the individual parts (see Figs. 7 to 9).

Enjoy trying out this useful and interesting function!

Figure 7

Figure 8

Figure 9

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