Product Modelling in Solid Works In the following exercise you will use solid works to construct the computer mouse shown opposite. In this exercise you will use a number of advanced features to achieve the complex shape shown. You will also reference the surfaces of other components in order to shape the component being modelled.

Modelling the top surface. The part has a contoured top surface. Before modelling any ‘Solid’ geometry we will first construct this top surface. This surface will be created as a lofted construction surface passing through 3 arcs. First you will construct 3 planes, the 3 arcs will be constructed, one on each plane, then finally a lofted construction surface will be constructed between these arcs. Using the front plane as the basis, construct 3 parallel planes to the left and right at the distances specified • Plane 1: 50mm to the left • Plane 2: 30mm to the right • Plane 3: 80mm to the right On each plane draw arcs as follows

On plane 1 construct an arc of radius 72mm with its centre on the vertical plane and 70mm below the horizontal plane or origin. Ensure the arc extends approximately 40mm to the left and right.

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On plane 2 and draw an arc of radius 45mm with a centre 20mm below the horizontal plane. (again extending 40mm to left and right) Finally on plane 3: draw an arc with a radius of 60mm whose centre is 50mm below the horizontal plane. Create a lofted construction surface through these curves. This surface will later be used to define the upper extent of the mouse boundary.

Creating the master shape. In the next step you will create the overall outline of the mouse, extrude it downward to form the base and upward to form the top. First of all working on the top plane create the sketch shown opposite to define the perimeter of the mouse. Once complete select extrude. For direction 1 specify the ‘Up To Surface’ option and select the lofted construction surface already created. In addition activate the draft option and specify and angle of 5 degrees.

For direction 2, specify blind, a distance of 5mm and a draft angle of 8 degrees.

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Add a 3mm fillet to the bottom edge and a 5mm fillet to the top curved edge. This is the master which defines the overall shape of the mouse. Save the part as MASTER.SLDPRT rename the part under the name master.

Splitting the mouse New we will split the mouse into two separate parts, base and top. We will then continue to add further design detail to complete both components. Working on the right hand plane, create a sketch, and draw a line level with the split line (or convert entities). Stretch the end points of this line past both ends of the mouse. Finally create an extruded construction surface, again ensuring that the construction surfaces stretches past the edges of the mouse in all directions. Select Insert Features Split from the pull down menu. . With the Trim Tools section highlighted select the extruded surface just created. Then select the [Cut Part] button. Selecting this button results in two unnamed items appearing under Resulting Bodies. You will also notice both items labelled on screen as shown opposite. C lick on each in turn and specify the name base or top. The remaining path and file extension will be completed by solid works. The parts will be saved in the same location as the original model. Finally choose [Save all Bodies] followed by accept to create two separate but related part files.

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Modelling base detail You will now add further design detail to the base. This will include: • Hollowing out to a uniform wall thickness of 2mm. • Adding a lip detail around the component edges. • Add bosses and counterbored screw holes to facilitate the screws which will be used to hold the mouse together.

Shelling First of all shell or thin wall the base. Specify a thickness of 2mm and select the top (split surface) as the opening or ‘face to remove’.

Modelling lip detail Next we will add a lip detail around the edge. The purpose of this is to help locate both halves. Another purpose is to ensure that should a gap develop due to warpage it will not be possible to see through the gap. This lip will be achieved by sweeping rectangular (cross section) around the inside edge (path/ drive curve). under Options to Select ensure the path (and resulting lip follows as the way round. To do this construct a reference plane normal to the inside edge using the normal to curve feature. Then create a sketch 1mm wide by 1.5mm high. This sketch should lie between the inside and the middle of the wall thickness. Finally select the swept extrusion create the lip.

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Modelling bosses and screw holes Next create the bosses. These will be created by selecting the inside bottom surface and creating 3 sketches according to the dimensions shown. Use appropriate sketch relations or construction geometry to ensure that the circles are fully defined. On completing of the sketch extrude upwards by 8mm.

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Drafting bosses To facilitate easy removal from the injection moulding tool all vertical faces must have a taper or draft applied to them. Therefore it is necessary to draft to bosses. In this case we will apply a draft of 3 degrees to all the bosses. form the features toolbar (or To draft the bosses select the draft tool select insert features draft) For the type of draft select Neutral Plane. Specify a draft angle of 3 degrees. For the neutral plane, select the top face and for the faces to draft select the side walls. Repeat for all three bosses and finish with 1mm fillets at the base.

Adding counter bores Finally add holes to accommodate the screws which will hold the mouse together. As the screws will be inserted from below counterbored holes will be required to accommodate the head of the screw. The screw which will be used will be a M4 by 12 panhead screw (ISO 7045). This will be created later using the toolbox. To accommodate the M4 panhead screw counterbores will be inserted from below. Working from the underside, create 3 counterbored holes. N.B. Remember to select the face first before selecting the hole wizard command. Specify the standard, type etc shown opposite.

Ensure that each hole is located centrally with respect to each boss by applying the appropriate relations. If it seems that you cannot select a specific edge in order to apply a relation to, you may that by rotating the view you may be able to select it from the other side. The boss with clipping applied looks as shown below left. The completed base looks as shown on the right.

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Modelling Top detail You will now add further design detail to TOP.SLDPRT. This will include: • Hollowing out to a uniform wall thickness of 2mm. • Adding a lip detail around the component edges. • Adding the bosses and threaded screw holes to receive the screws already mentioned. • Adding cutouts to accommodate the mouse buttons. Some of these details will be added now prior to assembly. Other detail will be added later after assembly enabling us to pick up on feature of other components. Open the part called TOP. SLDPRT. N.B. For clarity images will be shown with clipping plane active.

Shelling Next using the shell command hollow out the part to a uniform wall thickness of 2mm.

Adding lip detail In the next step you will add the lip detail. However as material was added when creating the lip on the base material will need to be taken away for this lip. This will therefore be done using a swept cut. Otherwise the procedure is the same. N.B. Because of the inside wall you will need to make a slightly larger cross section sketch to ensure that all is removed.

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Adding the cutouts for the buttons Working on the top plane, create the sketch shown opposite for the button cut-outs. For the curved lines which follow the outer shape use the offset command to offset the outermost edge inwards by 5mm. Add remaining vertical lines and dimension as appropriate. Add the horizontal line and dimension so that it is 40mm from the origin or front plane. Finally trim as required to produce 3 discrete contours. When complete create an extrude cut using the through all option. Finally fillet all remaining sharp corner specifying a radius of 3mm. For the remaining detail we will need the help of the base. For this reason we will need to assemble the mouse before we can model the next feature.

Draft edges of holes Again we need to draft vertical edges. In this case we want to maintain the lower of the whole while draft the vertical faces outward. For this we need to use the ‘Parting line’ option. For the angle specify and angle of 3 degrees. For the direction of pull select the top plane. For parting lines select the lower edge of the button openings. With fact propagation set to tangent should this will select the lower edge of the entire opening. Repeat for the other two holes.

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Assembling the mouse Create a new assembly and insert the base component locating it at the origin (by choosing accept). Next insert the top component. As there are not enough flat surfaces to use for assembly purposes, we will use reference planes instead. To assemble: • Mate the top part Front plane with the assembly Front plane. • Mate the top part Right plane with the assembly Right plane. • Mate the top part Top plane with the assembly Top plane.

Creating an empty part within the Assy You are now ready to model the buttons. Rather than modelling separately and then inserting into the assembly, this will be designed in position or ‘in place’. This will allow us to utilise the edges of existing geometry. In this case the to hole cutouts. To design in place: • Select: Insert Component New part… • Select the front plane in the assembly to position this new part within the assembly. Right click on the randomly named new part in the feature manager and select Rename Part. • Specify the name BUTTONS. It is possible for the geometric information defining the buttons to be held within the assembly or to exist as a stand alone part file (which is usually the case). To create a stand alone ‘Buttons’ part file right click on the component and select: • Save Part (in External File) In the dialog which appears select the buttons File and select ‘Same As Assembly’ followed by OK. This will save the BUTTONS.SLDPRT in the same folder as the other components.

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Creating the button geometry In order to create the button geometry you must first open the BUTTON part within the assembly. This is achieved by selecting the component in question, and then selecting the ‘Edit Part’ Icon shown. Selecting the top plane open a new sketch and view normal to. Then using the CTRL key select all of the edges of one of the button openings, then select convert entities to convert in lines in the current sketch. N.B. Ensure that you select the lower rather than the upper edge. You may need to rotate the view to ensure that you get the correct edge. Repeat again for the remaining two holes. Once the sketch is complete, orientate the assembly as shown below and then select feature extrude. Change the default end condition for Blind to Offset from Surface. (This will allow you to create the buttons a specified distance above a specified surface). To specify the reference surface, activate the box and select the top surface of the mouse. In the next specify an offset distance of 1.00mm. As this offset may be above or below the surface. You may need to select to reverse the offset.

The surface buttons should now look as shown protruding 1mm above the surrounding surface.

You will now create a rim around the buttons to prevent them pushing though the opening in the TOP component. To do this we will offset the button edges outward and then extrude upward until they touch the underside of the top component.

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While still in button editing mode, select the top plane and start a sketch. Viewing vertically downwards offset the edges of the buttons outwards by 1mm. When complete, issue the extrude command. This time select the ‘up to surface’ option. To select the surface, right mouse click on the top surface of the main part, choose ‘select other’ and pick the underside surface. The buttons should now look as shown.

Finishing the buttons We will now finish the buttons in stand alone mode. Return to assembly by clicking the assembly item at the top of the feature manager and choose ‘Edit Assembly’. Next open the buttons in stand alone mode using open part.

Working on the top plane, create a sketch and draw a rectangle around the buttons. Then create an extruded cut up to 3mm below the ledge using the offset from surface option.

Shelling the buttons. The buttons are still quite bulky and would therefore take some time to cool after injection moulding. It is there necessary to thinwall or shell the components. Shelling will also reduce the quantity of material required. Shell the buttons using a wall thickness of 2mm. You can only shell one solid body at a time. As the buttons consists of three separate solid bodies you will need to shell one button at a time. Add a 3 degree draft to the upper vertical surface on the button and finish with a 0.5mm fillet to remove the sharp edge.

Top component details Return to the top component and add bosses and screw holes to match with those in the base.

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