# Product Modelling in Solid Works

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1 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 then 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. 19/03/2013 1

2 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. To do this, activate the Surfaces toolbar and then select lofted surface. This surface will later be used to define the upper top profile of the mouse. 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. (the horizontal 60mm dimension is the dimension to corners prior to application of the 1mm fillets) 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. 19/03/2013 2

3 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. Select both check boxes to indicate that you wish to keep both halves. You are now ready to save these solid bodies as separate parts. To do so expand the solid bodies folder. Now, right click on the solid body representing the base and choose insert into new part Specify the name base.sldprt. Repeat again for the top part specifying the name top.sldprt. This creates two stand alone parts which are linked back to the original master model. 19/03/2013 3

4 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 counter-bored 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). Select under Options to ensure the path (and resulting lip) follows all the way around. 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 Swept Extrusion the lip detail. to create 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. 19/03/2013 4

5 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. To draft the bosses select the draft tool form the features toolbar (or 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 heads of the screw. The screw which will be used will be M4 Panhead screws (ISO 7045). This will be created later using the toolbox. To accommodate the M4 pan-head 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. 19/03/2013 5

7 Adding the cut-outs for the buttons Working on the top plane, create the sketch shown opposite for the button cutouts. 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 corners with a radius of 3mm. Draft edges of holes Again we need to draft vertical edges. In this case we want to maintain the lower of the hole while drafting 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 face propagation set to tangent Solid Works will select the lower edge of the entire opening. Choose accept to apply the tangent. Repeat for the other two holes. 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. 19/03/2013 7

8 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, again choosing accept. This will insert the components at the origin will all degrees of freedom constrained. This will be denoted by the letter (f) beside the component in the feature manager. Save the assembly as mouse.sldasm. 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. 19/03/2013 8

9 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. N.B. Should you find difficulty with this approach an alternative approach is suggested on the next page. 19/03/2013 9

10 Alternative approach Using the offset from surface option has been a recurring problem, whereby SolidWorks will not offset upwards despite repeated attempts to do so. Should you find that this is the case you may perform the action in two steps: Extruding up to surface Offset the surface an additional 1 millimetre. To do this select, Face, Move from the Insert menu. Under the move face menu select Offset and specify a distance of 1mm. This will offset the selected surface by the specified amount stretching all attached face to maintain the integrity of the solid model. Creating the button rim You will now create a rim around the buttons to prevent them pushing though the opening in the TOP housing. To do this we will offset the button edges outward and then extrude upward until they touch the underside of the top component. While still in button editing mode, select the top plane and start a sketch. Viewing vertically downwards (normal to plane) 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. 19/03/

11 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 therefore 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. Adding the screws To complete the mouse add three M4 x 12 Pan Head screws (ISO 7045). These will be created using the Solid Works Toolbox. To define the screws select: ISO, Bolts and screws Cross recessed screws Finally save in the current/working folder. 19/03/

12 Finish and Drafting Mouse Finally, draft the mouse creating the following: Orthographic views plan, elevation and end views. Section views and detail views Regular Isometric and exploded Isometric views Balloon references and parts list. Ensure that the standard IT-Sligo template is used for these drawings. Shown below are illustrations of each view types Orthographic views: Plan, Elevation and End views. Sections Section views should be used to show internal detail more clearly. Detail views: Create detail views of areas with small detail. E.g. seating area between buttons and top. the split line/lip detail the screw hole detail Detail views are created using: Pictorial views: Isometric and exploded views. 19/03/

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