Sports Deodorant Bottle tutorial. For Pro ENGINEER WILDFIRE 3.0 Schools Advanced Edition

Transcription

1 Sports Deodorant Bottle tutorial For Pro ENGINEER WILDFIRE 3.0 Schools Advanced Edition

2 Written by Mike Brown Copyright 2006, Parametric Technology Corporation (PTC) All rights reserved under copyright laws of the United Kingdom, United States and other countries. PTC, the PTC Logo, Pro/ENGINEER, Pro/DESKTOP, Wildfire, Windchill, and all PTC product names and logos are trademarks or registered trademarks of PTC and/or its subsidiaries in the United States and in other countries. Conditions of use Copying and use of these materials is authorised only in the schools, colleges and universities of teachers who are authorised to teach Pro/ENGINEER in the classroom. All other use is prohibited unless written permission is obtained from the copyright holder Acknowledgements Ian Pilkington, Andrew Deighton, Paul Sagar PTC 2 of 52

3 Table of Contents 1.0 Introduction Pre-requisites Abbreviations and terminology used within this tutorial Teacher s notes Installation and setup Pro/ENGINEER functionality addressed in this tutorial Science / Mathematical areas addressed in this tutorial D&T subject areas addressed in this tutorial Project Briefing Product background Product Design Solid Modelling The Ball The Collar The Cap The Bottle Design Analysis and Optimisation Calculating the volume of liquid Creating the Packaging % extra FREE...50 Appendix A...52 PTC 3 of 52

4 1.0 Introduction The Sports Deodorant bottle tutorial provides Students with an understanding of the product design process involved in the creation of a new personal hygiene product aimed at the sports/athletic market. During these tutorials Users will learn how to create parts and assemblies within, and explore the D&T, Mathematic and Scientific activities that are involved in the product design process This Tutorial and Teacher Resource has been produced by PTC and in support of the PTC Design & Technology in Schools programme. 1.1 Pre-requisites Schools Advanced Edition or University Plus Edition or Student Edition This tutorial contains screen and menu images taken from the Schools Advanced Edition so Users using other Pro/ENGINEER Editions may notice some slight differences. This tutorial has also been based on the use of Pro/ENGINEER start parts & templates supplied as part of the PTC D&T programme. While this tutorial can be used with other Pro/ENGINEER start parts there may be changes required in terms of view orientation, datum plane and coordinate system references etc. This tutorial requires an intermediate level of experience in Pro/ENGINEER Wildfire. PTC 4 of 52

5 1.2 Abbreviations and terminology used within this tutorial Ctrl LHMB MMB Pro/E.prt.asm RHMB The keyboard Control button (used in Pro/ENGINEER for multiple selection). Left-Hand Mouse Button Middle Mouse Button Pro/ENGINEER File extension for Pro/ENGINEER parts File extension for Pro/ENGINEER assemblies Right-Hand Mouse Button 2.0 Teacher s notes The aim of the tutorial is to provide students with an interesting project that supports the Design & Technology curriculum and demonstrates additional mathematical and scientific principles in an applied manner. Teachers and Students should have a good level of experience in modelling with Pro/ENGINEER in order to complete this tutorial. 2.2 Installation and setup These Installation notes have been complied based on a directory structure used as part of the PTC D&T programme, the UK CAD in Schools initiative and the deployment of Pro/ENGINEER. Users not part of this programme can still use this tutorial but may need to adapt either their Pro/E configuration files or the directory structure used in the tutorial. This tutorial is supplied with two bitmap images. These images should be placed in the Working Directory or in a centrally accessible directory. PTC 5 of 52

6 2.3 Pro/ENGINEER functionality addressed in this tutorial. Sketching o 2D geometry creation & modification o Geometric & dimensional constraints o Datum Plane and Axis creation Modelling o Revolve o Shell o Extrude o Variable Section Sweep o Helical sweep o Solidify o Part parameters o Relations o Goal driven Design Optimisation o Material assignment o Parametric modifications o Style Feature (Interactive Surface Design) Curve creation, analysis & modification Surface creation o Sheetmetal Creation of walls Unfold / development of 3D Sheetmetal component Assemblies o Assembly constraints o Design in context o Assembly Design Optimisation 2.4 Science / Mathematical areas addressed in this tutorial Biology Volume Nets (flat pattern development) 2.5 D&T subject areas addressed in this tutorial The Product Design Process o The inter-dependent relationships between components o Product Marketing affects on Product Design. CAD o Parametric feature based solid-modelling PTC 6 of 52

7 3.0 Project Briefing The Beauty and Style division of a Global Pharmaceutical company has identified the need for a more stylised offering of its roll-on deodorant product to address the needs of the sports and athletic oriented consumer. The new product needs to have a distinctive shape that fits securely into the hand in an ergonomic manner. To keep production costs down the new bottle has to use existing components such as the screw-cap and the roll-on applicator. 3.1 Product background What s the difference between Anti-perspirant and Deodorant? Anti-perspirants reduce wetness by plugging the sweat glands with miniscule amounts of aluminium salts that stay in place for around 3 to 4 days before being flushed out. Aluminium salts also act as anti-bacterials to stop any sweat that escapes your apocrine glands* from being turned into a nasty smell by the bacteria on your skin. The most effective anti-perspirants only block about 60% of sweat, they re really only designed for reducing underarm sweat and should never be applied all over your body as you may overheat if too many sweat glands are blocked. Deodorants are all about smelling nice. They include both a fragrance and an alcohol (ethanol) that kills BO-generation** bacteria, although it s only effective for about 12 hours. Deodorant won t stop you sweating but it will make you smell nicer. *Apocrine glands are formed from the same structure as the hair follicle and are found in different parts of the body including the armpits. **Body Odour is produced by micro-organisms (germs) that grow in particularly moist areas of the skin, such as the armpit. They produce BO by digesting the natural oils found on the skin but need water (sweat) to do so. 3.2 Product Design Before you design the new stylised bottle the roll-on applicator and screw cap will be modelled; these components will define the shape and size of the bottle top. The bottle will have an ergonomic and distinctive shape but must be designed to hold 50ml of Deodorant. PTC 7 of 52

8 4.0 Solid Modelling Start Pro/ENGINEER Wildfire and create a new directory i.e. deodorant bottle within the Folder Navigator. Set this new directory as the working directory; select the directory folder with the LHMB and then click the RHMB and select Set Working Directory. 4.1 The Ball In this section you will create the ball used in the roll-on applicator of the deodorant bottle. Create a new part called BALL. Click File>New and in the dialog that appears ensure Part is selected and then enter BALL. (Pro/ENGINEER will create a file BALL.prt) Create a new sketch and, following the prompt, Datum plane. ; select the FRONT To enter the sketcher select Sketch in the menu, Pro/ENGINEER automatically references the other datum planes and creates required reference geometry. If your sketch is not automatically oriented normal to the screen you can click View onto sketch. Select Create Circle and with the cursor positioned over the intersection of the two reference/construction lines click the LHMB; this will locate the circle centre. Now move the cursor out to define the radius and click the LHMB to create the circle. You can use the MMB to exit the create circle command. Change the dimensional constraint to 35.5mm; double click the dimension value and enter 35.5 then hit the return key to enter the value. PTC 8 of 52

9 Select Create Line and using the LHMB select at the points marked X 1 and X 2. Use the MMB to finish the insert line command. Select Dynamic Trim and remove the lefthand side of the circle. Next insert a Centreline along the vertical construction line. Finish and exit the sketch by clicking. Now select Revolve Feature and select the newly created sketch. Pro/ENGINEER will preview the feature; click the MMB to accept or the green tick in the Dashboard. The ball used in the roll-on applicator is made from acrylic and is hollow. To create a hollow ball select Shell Tool. Enter a thickness value of 2mm. Click the MMB to accept or the green tick in the Dashboard. Now Save this part using File>Save, or click Save File. PTC 9 of 52

10 4.2 The Collar In this section you will create the Collar which holds the BALL in the neck of the bottle. Create a new part called COLLAR. Create a new sketch on the FRONT datum plane. Insert a circle with its centre located at the intersection of the two references lines with a diameter of 35.5mm. This circle represents the outer diameter of the BALL and is to be used for construction purposes. From the RHMB menu select Construction, this will change the circle geometry from a solid line to dashed. Make sure you have the circle selected before opening up the RHMB menu. Insert another circle centred at the same location and drag the diameter so it s just a little large than the construction circle. Instead of defining the size of this new circle by its diameter it will be defined by an offset from the construction circle. Select Create Dimension and select the two circles at the points marked X 1 and X 2 with the LHMB. Position the dimension at the point marked X 3 using the MMB, Pro/ENGINEER will open a small dialogue asking you if this should be a Vertical or Horizontal dimension, Select Horizontal followed by Accept. Change the value to 2mm. This is not the final value but will allow easier construction/visibility of additional geometry. PTC 10 of 52

11 Now insert a line starting on the outer circle extending outwards. Use the LHMB to select the start point on the outer circle and ensure the normal symbol is displayed before using the LHMB to locate the end of the new line. Next insert another circle concentric with the existing circles and select the end of the newly created line to define the circle s diameter Use Dynamic Trim to remove the unwanted sections of circles Dimension the radial line and add a dimension from the horizontal reference line to the upper end of the line as shown, then change the values to those shown. Next create the geometry shown below. Ensure the line from the outer circle is tangent to circle and at an angle (which should be changed to 3 ). Use the Dynamic Trim to remove geometry. Insert a Centreline along the vertical reference line that passes through the centre of the circles. Now insert a chord line around the position shown. Then insert a radial line from the centre of the circle to the mid point of the chord line, an M symbol will appear to indicate the mid point. Chord line PTC 11 of 52

12 Select Sketcher Constraint and in the Constraint Menu select the Perpendicular constraint the radial line.. Now select the chord line and Change the radial line into Construction and use Dynamic Trim to remove the geometry not required as shown. To finish the profile add a vertical line from the end of the chord line and a horizontal line to close the profile as shown. Add the dimensions shown below and change the values to those shown. Finish and exit the sketch by clicking. Now select Revolve Feature and select the newly created sketch. Pro/ENGINEER will preview the feature; click the MMB to accept or the green tick in the Dashboard. PTC 12 of 52

13 Create a New Sketch and use the previous Datum Plane (i.e. FRONT). Once in the Sketch go to Top Toolbar and select Sketch>References and select outer straight edge of the new revolve to create construction/reference geometry in the current sketch. Insert a Centreline along the vertical reference line Sketch the closed profile shown and add the relevant dimensions. Note the 41.5mm dimension is a diameter and is created by selecting the Centreline, the profile geometry and the Centreline again, all with the LHMB, and then placing the dimension with the MBM. Finish and exit the sketch by clicking. Now select Revolve Feature and select the newly created sketch. Pro/ENGINEER will preview the feature; click the MMB to accept or the green tick in the Dashboard. Create another New Sketch on the FRONT datum plane. Select the bottom face of the newly created revolve and the tapered face of the main revolved feature for Sketch References, then sketch and dimension the profile shown. Insert a Centreline as before. Finish and exit the sketch by clicking. PTC 13 of 52

14 Now select Revolve Feature and select the newly created sketch. Pro/ENGINEER will preview the feature; click the MMB to accept or the green tick in the Dashboard. The Collar is now finished. 4.3 The Cap In this section you will create the screw Cap for the bottle. Create a new part called CAP. Create a new sketch on the FRONT datum plane. Insert a Centreline along the vertical construction line and then sketch the open profile show, (one vertical line and one horizontal line). Insert and Elliptical Fillet,, and change the dimensions to those shown. Finish and exit the sketch by clicking. Now select Revolve Feature and select the newly created sketch. As this is an open profile Pro/ENGINEER will assume you want to create a Surface so make sure you select As a Solid in the Dashboard. Pro/ENGINEER will now automatically assume a THIN feature, enter 2mm for the thickness. PTC 14 of 52

15 Pro/ENGINEER will preview the feature; click the MMB to accept or the green tick in the Dashboard.. The next task is to model the screw thread. To obtain the required thread form complete with run-in will require the creation of some surface geometry. Select the two faces of the CAP shown; keep selecting over one of the faces until Pro/ENGINEER s selection filter identifies the face then use the Ctrl key to select the other face. Use Copy (Ctrl C) then Paste (Ctrl V) to create copies of just these two faces. Use the MMB to complete the copy command. This command is referred to as Copy Geom. From the top Toolbar select Insert>Helical Sweep>Surface, this will open a Helical Sweep menu and a Menu Manager. In the Attributes menu select Done to accept the default settings of Constant, Thru Axis and Right Handed. The next menu that will appear is for setting up a Sketch Plane, select the FRONT datum plane. You will then be asked if this is the required viewing direction onto the Plane, select OK. You will then need to identify an orientation for the Sketch Plane, select TOP in the Menu Manager and then select the TOP Datum Plane in either graphics window or the Model Tree. Pro/ENGINEER will then place you in the Sketcher. During this modelling activity it is easier to work with the model displayed in hidden line mode, select Hidden Line. PTC 15 of 52

16 At this stage in the Helical Sweep feature Pro/ENGINEER needs and axis of rotation and a sweep direction vector (this specifies both direction and length of the sweep. From the top Toolbar select Sketch>References and select one of the vertical inner walls of the CAP. Insert a Line along this reference line starting 4mm up from the base of the CAP extending up 15mm. Insert a Centreline along the reference line on the axis of the CAP. To accept this geometry and progress to the next step click accept sketch. Pro/ENGINEER will now prompt for a Pitch value, enter 4mm, either select the green tick or hit return to enter the value. You will now be placed back in the sketcher to create the profile section. Sketch a simple straight line running along the horizontal reference line (the one 4mm up from the base of the CAP), ensuring it intersects the inside face of the CAP. To accept this geometry and progress to the next step click accept sketch. You have now defined all the geometry and references required to create to Helical Sweep, click OK in the Helical Sweep Menu. The next step is to use the helically swept surface and the previously copied surfaces to generate a path along which to sweep the thread profile. In the Model Tree select the Copy feature and the Surface feature, (use the Ctrl key for multiple select) From the top Toolbar select Intersect. This will create a helical spline; to see this more clearly select the newly created helical Surface in the Model Tree and from the RHMB select Hide. PTC 16 of 52

17 The next step is to create the thread by sweeping a profile along the helical spline. Select Variable Section Sweep Feature and select the helical spline, either directly by the geometry or in the model tree by selecting the Intersect feature. Make sure the Create Surface option is selected in the Dashboard. Pro/ENGINEER will display the selected spline as the Path for the sweep. The T= 0.00 indicators refer to the Tangent ends of the sweep. The default is 0.00 indicating the sweep will start and end at the ends of the path. In this case we want the thread to extend tangentially at both the start and the end of the thread. Double click the T = 0.00 indicators and enter a value of 9mm for both of them. Next select Sketch Section. Pro/ENGINEER will reorient the view and create some reference geometry. Sketch an open profile as shown with the indicated dimensions. To accept this geometry and progress to the next step click accept sketch. Pro/ENGINEER now has sufficient information to create a helical sweep; however, as this part of the CAP has a 3 taper the sweep actually twists with each revolution. To create the required thread we need to tell Pro/ENGINEER to reference the sweep from another piece of geometry. In the Variable Section Sweep Dashboard select Options and in the menu that appears select Constant section. Now select References. In the menu that appears select Normal To Trajectory and change this to Normal To Projection. Pro/ENGINEER will now prompt for a selection, select the Datum Axis in the graphics window (make sure you have Datum Axes visible ) Click the MMB to accept or the green tick in the Dashboard.. PTC 17 of 52

18 The thread geometry created now has the required run-in but it s still just a surface. Select the Var Sect Sweep in the Model Tree and from the top Toolbar select Edit>Solidify. Pro/ENGINEER will indicate which side of the swept surface it intends to make part of the solid, click the MMB to accept and finish the command. The next step is to add material to help seat the ball applicator. Create a New Sketch on the FRONT Datum Plane and select the inside curved face and vertical face of the CAP as a Sketch References. Sketch the geometry shown with the dimensions and values indicated. Don t forget to add a Centreline. Accept the sketch and exit the Sketcher. Now select the Revolve Feature icon and select the newly created sketch. The final feature on the CAP is a small extrusion which keeps the BALL pressed down in the COLLAR to ensure a seal is maintained and now liquid escapes. Create a New Sketch on the top inside flat face of the CAP and sketch a Circle 10mm in Diameter with its centre located at the intersection of the two default sketch reference lines. Finish and exit the Sketch. Create an Extrude Feature 3mm down with a Thin option and a thickness of 1mm on the outside of the circle. PTC 18 of 52

19 4.3 The Bottle In this section you will create the actual bottle part of the Deodorant Bottle. While the Bottle will have a freeform shape the top of the bottle and its neck must mate up with the CAP and COLLAR components. As part of the Product Design process a Designer has drawn a couple of concepts for the shape of the bottle (scan right.bmp & scan front.bmp). These images will be used to help define the Pro/ENGINEER geometry See Appendix A Create a new part called BOTTLE. Create a New Datum Plane offset from the TOP Datum Plane by 70mm, this will help in sizing the bottle and in future modifications. Rename this Datum Plane to BOTTLE_HEIGHT Select the Style Tool icon. Pro/ENGINEER will change the menu down the right-hand side of the screen and display an addition set of icons under the top Toolbar. Pro/ENGINEER will also change the Datum Plane display; a grid is displayed on the active Datum Plane. Click the Set Active Datum Plane icon and select the RIGHT Datum Plane. Select Styling from the top Toolbar and from the drop-down menu select Trace Sketch PTC 19 of 52

20 Pro/ENGINEER will open the Trace Sketch menu; Select RIGHT. This will open up another menu; navigate to the directory where you placed the two scanned images, scan right.bmp & scan front.bmp, during the tutorial set-up and select scan right.bmp. Change your view orientation to look directly onto the RIGHT Datum Plane. Pro/ENGINEER has inserted the bitmap image on the RIGHT datum plane. The image has a number of graphical handles that allow you to manipulate the image: o o o o The large blue cross allows you to rotate the image around its intersection. The green horizontal and vertical lines allow you fit the image to a required size by dragging the green circles. The grey box is another graphical handle that scales the image. The H & V in the bottom left-hand corner of the image denote the Horizontal and Vertical axes of the image (these are not related to the part and are only used to manipulate the image). Using the green circles drag the green lines so that the top one intersects the centre of the base of the CAP and the bottom green line touches the bottom of the bottle. In the Trace Sketch menu enter a value of 70mm and click Fit. Pro/ENGINEER will scale the image so that the distance between these two lines is 70mm. Drag the image so that the centre of the bottle lines up with the FRONT Datum Plane and the upper green line lies on B OTTLE_HEIGHT Datum Plane. Then Click OK in the Trace Sketch menu. PTC 20 of 52

21 Click the Set Active Datum Plane icon and select the FRONT Datum Plane. In the Trace Sketch menu select the Add option and select the FRONT Datum Plane. Change the view orientation to look directly onto the FRONT Datum Plane. The image will have come in on its side. Select the Properties in the Trace Sketch menu and Rotate the image 90º Using the graphical handles scale the image to the required size. To obtain the correct size re-orient the view as you scale to compare the image size to the previously scaled image. This will take a little trail and error until it looks correct. The placement of the Concept design sketches is now complete. Finish and Exit current Style Feature. The Concept design has the CAP angled; to incorporate this aspect of the design a new Datum Plane will be created. Create a New Axis at the intersection of the FRONT and BOTTLE_HEIGHT Datum Planes. PTC 21 of 52

22 Next create a New Datum Plane selecting first the new Axis (A_1) and then, with the Ctrl button held down, select the BOTTLE_HEIGHT Datum Plane; this new Datum Plane should be angled so that it linesup with the angled top of the bottle image (roughly at 157º). Reorient the view to look directly onto the RIGHT Datum Plane to help set the angle for this new Datum Plane. Name this new Datum Plane ANGLED_TOP. Now create another New Datum Plane, again selecting the Axis, then select the ANGLED_TOP Datum Plane, the new Datum Plane wants to be normal to ANGLED_TOP so in the Datum Plane menu select Normal, then OK. Name this new Datum Plane TOP_NORMAL. File/Save the part The Concept designs provide an idea of what the new bottle should look like but it must also be designed to fit the existing CAP and COLLAR. The next step is to assemble these existing components with the Concept designs. Create a New Assembly called DEODORANT_BOTTLE Using Add Component add in the bottle (BOTTLE.PRT). In the Assemble Component dashboard select Automatic and from the pulldown menu select Default. Accept and exit the assemble component command PTC 22 of 52

23 The next step is to assemble in the CAP. As we will only need the datum planes within the BOTTLE.PRT select all the assembly Datum Planes and Coordinate System and hide them, (ASM_RIGHT, ASM_FRONT, ASM_TOP, ASM_DEF_CSYS) Using Add Component add the screw cap (CAP.PRT). The CAP will be assembled using Datum Planes; o The TOP Datum Plane in CAP.PRT should be Aligned to ANGLED_TOP in BOTTLE.PRT; Select the Mate option for the distance/offset. o The RIGHT Datum Plane in CAP.PRT should be Aligned to the RIGHT Datum Plane in BOTTLE.PRT; again select the Mate option for the offset distance. o The FRONT Datum Plane in CAP.PRT should be Aligned to TOP_NORMAL in BOTTLE.PRT; Select the Mate option for the offset. Accept and exit the assemble component command If the CAP part has the helical swept surface visible just expand the CAP part in the model tree (by clicking the small plus symbol ), select the Surface and from the RHMB select Hide. On closer inspection it the Trace Sketches may now appear not to be aligned with the accurately positioned CAP. To position the Trace Sketches more accurately select the BOTTLE.PRT in the model tree and from the RHMB menu select Activate. You are now in the BOTTLE.PRT which is indicated by a small green diamond next to the part in the model tree. PTC 23 of 52

24 Expand the BOTTLE.PRT tree by clicking the small plus symbol. Now select the Style Feature and from the RHMB menu select Edit Definition. This will place you back in the Style Feature command. From the top Toolbar select Styling>Trace Sketch and in the Trace Sketch menu select Right: scan right.bmp Click and hold down the LHMB to drag the image to align more accurately with the CAP. When you re happy finish and Exit current Style Feature. The next step is to create some sketch geometry for the base of the bottle. It may be easier to do this in BOTTLE.PRT outside of the Assembly; from the top Toolbar Select Window and in the Drop-Down menu that appears select BOTTLE.PRT. Create a New Sketch on the TOP Datum Plane. To help in sketching the bottom of the bottle, re-orient the view slightly so you can see the two scanned images (you may also need to zoom in) At this stage you will be creating simple rectangles to indicate the rough size of the bottle bottom; the actual shape will be defined later. PTC 24 of 52

25 Insert two adjoining rectangles to form bounding boxes for the right-hand half of bottle bottom and add/modify the dimensions to align the rectangle to the Trace Sketch images. Accept the sketch and exit the Sketcher. The next step is to repeat this process where the Concept design shows the bottle waist. First a new Datum Plane needs to be created. Create a New Datum Plane and offset it from BOTTLE_HEIGHT by 19mm. Name this Datum Plane WAIST. Create a New Sketch on the WAIST Datum Plane. Again sketch two rectangles to form the bounding geometry for the waist of the bottle and add/modify the dimensions to align the rectangle to the Trace Sketch images. Accept the sketch and exit the Sketcher. The next step is to create geometry that defines the top of the bottle. As per the Concept design the bottle top and the cap are the same diameter. Create a New Sketch on the ANGLE_TOP Datum Plane. To fully locate the Sketch Pro/ENGINEER will ask you to select References; Select the RIGHT and TOP_NORMAL Datum Planes; Close the References menu. PTC 25 of 52

26 Sketch a circle 48mm diameter centred at the intersection of the two reference lines. Use Dynamic Trim to remove of the left-hand side of circle so you re left with a semi-circle on the left. Accept the sketch and exit the Sketcher. The next step is to create the freeform curves to define the contours of the bottle based on the Concept sketch images and the bounding geometry. A few of the Datum Planes not required for the construction of the curves have been hidden from some of the images used in this section of the tutorial. Select the Style Tool icon to enter the Style environment. The first curve to be created will define one half of the bottle bottom. Click the Set Active Datum Plane icon and select the TOP Datum Plane. Select the Create Curves icon. IMPORTANT Note: In the Style Curve Dashboard make sure Planar is selected Using the LHMB create curve points and create a curve similar to the one shown. PTC 26 of 52

27 The next step is to edit this curve to refine its shape and ensure it matches-up to the bounding box geometry. Click the Edit Curves icon and select the first curve. You can select and move existing points, add new points and delete unwanted points to help smooth out the curve to a pleasing form. To make the points on the curve directly reference existing geometry hold down the Shift key when moving a point; As you move the point close to a piece of geometry you will see it snap to it, this curve point is now linked to the geometry. Make sure the curve snaps to the relevant ends of the bounding box geometry (as shown below). Link points You can also control the tangency of the curve end points. Select one of the curve end points and you ll notice a green line appear, this controls the tangency of the curve. The longer the green line the more effect the tangency condition has on the curve. The curve needs to be Normal at its ends; Select the green Tangency line with the LHMB and from RHMB pull-down menu select Normal, and select the RIGHT Datum Plane, repeat this for the other end of the curve. PTC 27 of 52

28 At this point you may have a curve that looks good or one that has bumps. When creating Style Curves it is often required to have what is called a Smooth curve where the rate of change of curvature is gradual. Pro/ENGINEER has a number of curve and surface analysis tools to help you create a Smooth curve and/or surface. From the top Toolbar select Analysis>Geometry>Curvature. In the menu that appears select the Definition Tab and change the Scale to 10 and Quality to 20. If your curve is not already selected, select it. This graphical display shows the rate of change of curvature. To obtain a Smooth curve this graphical display should show gradual changes. Once again click the Edit Curves icon and select the curve. With the LHMB select each of the points (but not the end points) and drag them around until you achieve a pleasing curve that also has a gradual rate of change of curvature. PTC 28 of 52

29 To turn off the Curvature Analysis graphical display go to the top Toolbar and Analysis>Hide All. The next step is to create similar curves on the WAIST Datum Plane at the neck of the bottle. Click the Set Active Datum Plane icon and select the WAIST Datum Plane. Using Create Curves define the curve at the bottle waist and Edit Curves to modify the curve to directly reference the bounding boxes and make the curve end points Normal to the RIGHT Datum Plane. Once again you can use Curvature Analysis to ensure you have a Smooth curve. Another important requirement for these curves is the Minimum Radius of Curvature ; later on the bottle will be shelled to make it hollow and the Minimum Radius of Curvature needs to be larger than the shell thickness. For example: If the wall thickness was to be 2mm the Minimum Radius of Curvature would have to be higher that 2mm i.e. 3mm. From the top Toolbar click Analysis>Geometry>Radius, and once the menu has appeared select the curve. The value needs to be greater than 1.5mm The next Style Curves to be created will form the side contours of the bottle. Click the Set Active Datum Plane icon and select the RIGHT Datum Plane. Using the LHMB click at points along the scanned image curve and Pro/ENGINEER will start to create a curve through these points. PTC 29 of 52

30 Select the Create Curves icon again to start the next curve. The next step is to edit these curves to refine their shape (Smooth) and ensure they match-up to the existing bottle geometry. Edit Curves to make the curve ends directly reference the bounding box at the bottom and the CAP geometry at the top. Also have one point along the curve reference the curves at the waist. The curve end points also need to be Normal to the relevant Datum Planes. The next step is to create the other curve to define the shape of the side of the bottle. Click the Set Active Datum Plane icon and select the FRONT Datum Plane. Select the Create Curves icon. IMPORTANT: In the Style Curve Dashboard make sure Planar is selected. Using the LHMB click at points along the scanned image curve and Pro/ENGINEER will start to create a curve through these points. Once again the next step is to edit this curves to refine its shape and ensure it match-up to the existing bottle geometry etc. PTC 30 of 52

31 When you re satisfied with this curve you should have created 5 Style Curves in total. Each Style Curve should be directly linked to other curves at its end and also linked to the waits curve. Failure to ensure each curve is linked to other curves and/or bounding box geometry will result in feature failure when the bottle is modified. Style Curve 03 CAP curve Style Curve 02 Style Curve 04 Style Curve 05 Style curve 01 The next step is to create surfaces based on these curves. To make it easier to see the curves and surfaces you can hide the Trace Sketch images by going to the top Toolbar View>Display Settings>Model Display and un-checking the Trace Sketch box followed by OK. Click Create Surfaces from boundary Curves and using the LHMB select the first curve, then holding down the Ctrl key select the 4 curves which form the enclosed boundary. PTC 31 of 52

32 Then from the RHMB menu select Internal Collector and select the sectional geometry at the neck of the bottle. To accept this surface select the green tick on the far right of the Dashboard. The Style surface is now finished, click Exit Style Feature. PTC 32 of 52

33 To create the other side of the bottle select the newly created surface click the Mirror Tool icon the select the RIGHT Datum Plane followed by the MMB to accept. Now select both sides of the bottle and click the Merge Tool icon to join the two halves of the bottle; MMB to accept. The next step is to close the top and bottom of the bottle by creating two surface patches and trimming them to the shape of the bottle openings. Create a New Sketch on the TOP Datum Plane and sketch two lines, one on either side of the bottle bottom opening. The length and separation of the lines is not critical, they should be of sufficient size and distance apart to allow for any reasonable future changes in bottle shape and size. Finish and exit the sketch by clicking. Next click the Boundary Blend Tool icon and select both lines (hold down the Ctrl key for multiple selection); MMB to accept. To trim the new surface to the bottle click the Merge Tool icon and select both the surface and the bottle; the yellow arrow that appears indicates which part of the surface will be kept. Repeat this process to close off the top of the bottle. Create the required sketch on the ANGLED_TOP Datum Plane and select the RIGHT and TOP_NORMAL Datum Planes for references. PTC 33 of 52

34 When you have created all the required surfaces the bottle can be turned into a solid using the Solidify command Using the LHMB select part of the bottle, then move the cursor slightly and select the geometry again, the entire bottle should now be highlighted, from the top Toolbar select Edit>Solidify; MMB to accept. Add a 3mm radius round to the bottom edge of the bottle. The main body of the bottle is now complete. If you open up the DEODORANT_BOTTLE.ASM the final bottle is starting to take shape. The next step is to model the bottle top or neck, this is the bit into which the COLLAR fits and the CAP screws on to. This part of the bottle will be modelled based on the geometry of both the CAP and the COLLAR. First create a New Axis in BOTTLE.PRT. Click Create Datum Axis then select the RIGHT Datum Plane then holding down the Ctrl Key select TOP_NORMAL Datum Plane. Open up DEODORANT_BOTTLE.ASM and click Add Component and select COLLAR.PRT. The assembly references are: o The Axis of COLLAR.PRT and the newly create Axis in BOTTLE.PRT o The RIGHT Datum Plane in BOTTLE.PRT and the RIGHT Datum Plane in CAP.PRT with an Align-Mate o And the top angled face of BOTTLE.PRT is Mated to the bottom face of CAP.PRT with an Mate-Offset of 2mm. PTC 34 of 52

35 Select the BOTTLE.PRT in the model tree and from the RHMB menu select Activate. You are now in the BOTTLE.PRT which is indicated by a small green diamond next to the part in the model tree. Create a New Sketch on the top angled face of the bottle. The Sketcher will require you to specify some reference geometry to accurately position the Sketch, select the RIGHT and TOP_NORMAL Datum Planes. Click Create an Entity from an Edge and select the bottom edges of the lip on COLLAR.PRT, this will drop two arcs onto the sketch. Finish and exit the sketch by clicking. Click Extrude Feature and from the Dashboard select the Extrude to Selected Point option. Select the bottom face of the lip on COLLAR.PRT Create a Round Feature of radius 0.25mm along the edge of the new feature and the bottle. Open BOTTLE.PRT and create a Shell Feature of 1.25mm and select the top face of the bottle to open it up. PTC 35 of 52

36 The next step is to model the ridge that will retain the COLLAR.PRT in the throat of the bottle. Go back to the DEODORANT_BOTTLE.ASM and Activate BOTTLE.PRT. Change the view orientation to look onto the RIGHT Datum Plane and change the view visibility to Hidden Line. Zoom in so you can see the ridge feature on COLLAR.PRT and Create a New Sketch on the RIGHT Datum Plane. Add additional sketch references of the inside face of the bottle throat, the angled face of the ridge and the A_2 axis in BOTTLE.PRT. Create an Arc as shown and make it Tangent to the angled reference line of the COLLAR ridge. Dimension the ends of the arc and change the value to 2.5mm. Add a Centreline on the reference geometry created from the A_2 Axis Finish and exit the sketch by clicking. Create a Revolve Feature making sure you select Solid the feature. in the Dashboard. MMB to accept The final modelling step for the bottle is to create the screw thread. This thread will use the same techniques used for the creation of the screw thread on the CAP. Open BOTTLE.PRT Using Insert>Helical Sweep>Protrusion create a Constant, Thru Axis, Right Handed helical sweep around the bottle top with the Sweep direction starting 3mm from the opening of the bottle top for a length of 4.25mm. Don t forget to insert a Centreline. Sketch on the RIGHT Datum Plane and use DTM2 to define Top and DTM3 for a reference. Select the outer face of the bottle top as a Sketch>Reference. The Swp Profile starts 3mm from the top of the bottle and is 4.25mm long. PTC 36 of 52

37 Don t forget to insert a Centreline for the sweep. The Pitch is 4mm Sketch the thread section as shown. Click accept to exit the sketch. Click OK in the Protrusion: Helical Sweep menu to create the feature. To create the thread run-in click Round Feature and in the Dashboard click Sets and in the pop-up menu that appears change Circular to D1 x D2 Conic. Select the edge of the new thread and enter values of 5mm x 1mm with a Rho value of 0.1. The Rho (ρ) is the 17 th letter in the Greek alphabet and in this case refers to the radius of curvature, i.e. how flat or curved the round will be. The bottle is now complete. To complete the DEODORANT_BOTTLE.ASM add the BALL.PRT into the COLLAR. Don t forget to save all your files. PTC 37 of 52

38 5.0 Design Analysis and Optimisation This Deodorant Bottle is required to hold 50ml of deodorant liquid. During the modelling of the bottle you ve used estimated values for various dimensions. The first analysis we need to do is find out exactly how much liquid the bottle can hold. 5.1 Calculating the volume of liquid The first step is to define the fill-level of the bottle. Open up BOTTLE.PRT In the Model Tree move the Insert Here to above the Shell feature, this will suppress all features created after the Insert Here position so you should have a solid bottle. Create a New Datum Plane, giving it a name of FILL_LEVEL. Select BOTTLE_HEIGHT and offset the new Datum Plane 12mm below. From the top Toolbar click Analysis>Model>One-Sided Volume. In the menu that appears select Feature and then select the FILL_LEVEL Datum Plane. Make sure the yellow arrow points down and click to accept. This will create an Analysis Feature in the Model Tree This calculated volume is of the solid bottle below the FILL_LEVEL Datum Plane. To calculate the internal volume of the bottle below the FILL_LEVEL; i.e. the actual volume of deodorant, the first volume (VOLUME_1) needs to have the volume of the bottle mterial subtracted.. PTC 38 of 52

39 Move the Insert Here to below the Shell feature. Repeat the volume analysis process, again using One-Sided Volume. Make sure you have selected Feature, Pro/ENGINEER will create the Analysis Feature in the Model Tree,. The next step is to create an Analysis Feature. In the menu that appears select Relation for the Type of Analysis Feature (do this step first), then enter a name for the Analysis of FLUID_VOLUME (hit the Return key to enter this name). Click the Next button at the bottom of the dialogue box, this will open up the Relations menu. This relation will make fluid_volume_calculation = VOLUME_1 VOLUME_2. a) In the Relations section of the menu type fluid_volume_calculation then enter an equals symbol =. b) To bring in the VOLUME_1 feature click Insert from the Relations menu Toolbar and from the two options in the pulldown select from list c) In the next menu that appears (Select Parameter) click the word Part and from the listed options select Feature. This will close the Select Parameter menu and prompt you to select the required feature; Select VOLUME_1 from the Model Tree. As soon as you select this feature the Select Parameter menu will re-appear with the ONE_SIDED_VOL highlighted. PTC 39 of 52

40 d) At the bottom of this menu select Insert Selected. This will enter the ONE_SIDED_VOL into the Relation and take you back to the Relations menu. e) Enter a minus symbol - and repeat steps b, c &d for VOLUME_2. This will produce the required Relation; Fluid_volume_calculation = ONE_SIDE_VOL:FID_790 ONE_SIDE_VOL:FID_791 (FID refers to the Feature ID). Click Ok to accept this Relation and exit the menu and then click to accept the creation of the ANALYSIS feature. Now that an Analysis Feature has been created Pro/ENGINEER can perform an Optimisation based on this Feature. From the Pro/ENGINEER top Toolbar select Analysis>Feasibility/Optimisation. In the Goal section set it to Maximize and from the adjacent pull-down menu select FLUID_VOLUME_CALCULATION In the Design Constraints section click Add and again select FLUID_VOLUME_CALCULATION and make it = entering a value of 50,000 (50,000mm 3 which is 50ml), then click OK. In the Design Variables section click Add Dimension and then in the graphics window select the FILL_LEVEL Datum Plane. This will display the dimension used to create the Datum Plane, select this dimension and enter a Minimum value of 5 and a Maximum of 12. PTC 40 of 52

41 In the Model Tree move the Insert Here indicator to the bottom of the Model Tree to complete the modelling operations. To start the Design Optimisation click Compute. Pro/ENGINEER will now go through many iterations of a trail and error sequence; it will change the offset value of the FILL_LEVEL Datum Plane, calculate the VOLUME_1 and VOLUME_2 perform the equation to workout the FLUID_VOLUME and check this against the required value of 50ml. this process will be repeated many times until it achieves the required result and then display a graph showing the convergence path. Based on the results the current bottle can hold the required 50ml if the FILL_LEVEL is 6.58mm below BOTTLE_HEIGHT. This is acceptable so click Close and Confirm to accept the new computed value for FILL_LEVEL. Don t forget to Save your files. PTC 41 of 52

42 6.0 Creating the Packaging To help differentiate the Sports Deodorant from the normal product it will be sold in a box. The box will be designed with reference to the bottle to ensure that should any modifications be made to the bottle size the box will also change. The box will be made out of cardboard but in terms of Pro/ENGINEER the functionality used to create the box is also used to create sheet-metal components. There are a couple of ways to create a the box; a) Create the box as a solid and then turn it into a sheet-metal box b) Build the box up using sheet-metal components i.e. flat-walls etc. In this case the box will be created by building the box with sheet-metal components. Open the DEODORANT_BOTTLE.ASM As the box part doesn t yet exist Pro/ENGINEER can create a new part while also adding it to an assembly. Click Create Component in Assembly Mode, select Part and Sheetmetal, give it the name BOX, making sure you use the correct start part (i.e. the sheet-metal start part), and position it in the assembly using the Default assembly constraint. To ensure the BOX.PRT is the correct size the box geometry will directly reference the relevant parts of DEODORANT_BOTTLE.ASM. In the Model Tree Activate BOX.PRT Create a New Sketch on the RIGHT Datum Plane and select the indicated edges as Sketch References. These edges form the extremities of the bottle and the BOX size will be determined based on these edges. Sketch 3 lines; 2 vertical up each side of the bottle and one across the top, and change these to Construction lines. Make each line Tangent to the relevant Reference lines/edges. PTC 42 of 52

43 The BOX will need to be slightly larger than the Deodorant Bottle. Sketch a Rectangle that is larger than the Construction lines and dimension it so that each side of the Rectangle is offset as shown (1mm below the bottom, 2mm above the top and 1.5mm each side). Finish and Exit this Sketch. Create a New Datum Plane and select the lefthand vertical line of the just-sketched rectangle, hold down the Ctrl key and select the RIGHT Datum Plane, in the Datum Plane menu select click the word Offset and select Normal from the pull-down list; OK to create the plane. Create a New Sketch on this new Datum Plane. Change the view orientation so you can see the previously create sketch, then from the top Toolbar select Sketch>References select the end of the sketch line to create a point, repeat this for the line at the bottom of the bottle. Dimension the rectangle to be 1.5mm either side of the CAP and add a dimension and change it to 0.0mm for the top and bottom. Finish and Exit this Sketch. The first step in creating a sheet-metal component is to create what is called an unattached free wall. Click Create Unattached Free Wall and then select the second sketched rectangle. Pro/ENGINEER will preview the wall feature and prompt you for a thickness in the Dashboard. Enter a value of 0.5mm and also Flip Direction so that the thickness is on the outside. Click to accept creation. PTC 43 of 52

44 The next step is to create the lid of the box. Click Create Flat Wall and select the inside edge of the previously created unattached wall. Pro/ENGINEER will preview a default wall. Position the cursor over the preview and from the RHMB Menu select Flip Thickness. From the RHMB Menu now select Edit Shape and enter a value of in order to bring the sides of the wall in, (you must enter negative 0.5mm to ensure the offset is in ). Don t forget to enter the -0.5mm for both sides of the wall. In the Dashboard click Relief and in the sub-menu that appears select Rectangular and enter a value of 1.0mm where it initially says Up to Bend. This will create what s called a corner relief. The use of corner relief will become apparent as the BOX model evolves. the BOX lid the correct length. The next step is to make In the Dashboard click Shape and in the submenu that appears select Sketch, in the Sketch menu select Sketch. This will place you in the now familiar Sketcher. You will notice a dimension controlling the length of the wall, select and Delete this dimension. PTC 44 of 52

45 From the top Toolbar select Sketch>References and select the very end of the sketch line which was created to define the top of the BOX. This will create a point in the current sketch. Add a dimension between this point and the edge of the wall and change it s value to Accept and exit the Sketch and click the MMB or to create the BOX top. The next step is to create step is to add the lid flap, the tab that will tuck into the box to hold the lid closed. Click Create Flat Wall and select the lower edge of the box. In the Dashboard change Rectangle to Trapezoid and via Edit Shape set the length of the flap to 15mm. to accept the new wall. The bottom of the box is identical to the top so rather than go through the wall creation steps again Pro/ENGINEER can copy and paste the walls. PTC 45 of 52

46 In the Model Tree select the two walls that make up the lid and from the RHMB select Group. With the new Group still selected, use Ctrl C to copy; then select the bottom inside edge of the box and then Ctrl P. Pro/ENGINEER will preview the new wall (only the first wall in the group will be visible), position the cursor over the preview and from the RHMB menu select Flip Thickness followed by MMB to accept. The next step is to create the first side-wall of the box. Click Create Flat Wall and select the inside edge of the first wall. Pro/ENGINEER will immediately preview the new wall, From the RHMB Menu select Flip Thickness, then from Dashboard select Edit Shape and enter a value of 0.5mm, (no minus this time), to extend the side of the wall, (don t forget to do this for both sides). Next click Relief in the Dashboard and select Rectangular, (the default settings of Up to Bend and are required) The next step is to define the length of the wall by referencing existing geometry. In the Dashboard click Shape and in the sub-menu that appears select Sketch, in the Sketch menu select Sketch. You will notice a dimension controlling the length of the wall, select and Delete this dimension. Next add a new dimension between the edge of the wall and the sketch which was created to define the size of the box. Change this dimension to 0.00mm. Accept and Exit the Sketch. Most times this sketching process will flip the thickness, so to create the required newly defined wall select Flip Thickness once again from the RHMB menu. Click the green tick to create the wall. The next wall to be created is the front of the box. PTC 46 of 52

47 Click Create Flat Wall and select the inside edge of the newly created side wall, from the RHMB menu Flip Thickness and from the Dashboard click Shape and enter values of - 0.5mm, (negative 0.5mm), to bring the sides of the new wall in, then select the Relief option and change the type of Relief to Rectangular. Once again the length of the new wall needs to reference existing geometry. Go back to Shape and select Sketch, once inside the sketch delete the existing length dimension and add a new one between the edge of the new wall and the edge of the back wall and change its value to 0.0mm. Again you may need to perform Flip Thickness to ensure the wall is created outside. Accept and exit the sketch new Wall. and accept the Note: To allow the correct creation of future walls the corners of the newly created front wall, at both the top and bottom of the box, should be as shown in the enlarged image. To create the final box wall click Create Flat Wall and select the inside edge of the previously created wall. In the Shape menu change the offsets to 0.5mm and in the Relief menu select Rectangular. Back in the Shape menu select Sketch, once in the Sketcher delete the dimension controlling the length of the wall and again create a dimension to existing geometry and set the value to 0.0mm. (If you ever flip the viewing direction of the Sketch Pro/ENGINEER may also change the wall offset from 0.5mm to 0.5mm, if this happens just edit the dimensions in the Sketcher to ensure the offsets go in the correct direction). Accept the Sketch and Accept the wall creation. The next step is to create the tab which will be used to glue the previously create wall to the back wall of the box. Click Create Flat Wall and select the inside edge of the previously created wall. In the Shape menu change the offsets to - 0.5mm (negative 0.5mm) and the length to 12mm, in the Relief menu select Rectangular and then Accept the wall creation. The final task is to create the flaps on the side walls of the box, both top and bottom. PTC 47 of 52

48 Click Create Flat Wall and select the inside edge of the top part of the first side wall. Change the Shape from Rectangular to Trapezoid and in the Shape submenu set the length to 20mm. Accept the wall creation. To create the other 3 flaps select this newly created wall in the Model Tree and use Ctrl C & Ctrl P to Copy and Paste the flap onto each of the corresponding edges. When the box is finished don t forget to save the file. One of the benefits of using the Pro/ENGINEER Sheetmetal functionality is the flatten capability. Sheetmetal components are produced from flat sheets of material that are subsequently bent or formed into their required final shape. Pro/ENGINEER enables the Engineer/Designed to model the finished shape and then develop the shape into flat form ready for cutting etc. Click Create Flat Pattern, Pro/ENGINEER will then prompt you to select a Flat Plane or Edge. Select the face of the first wall created (the back of the box); Pro/ENGINEER will immediately flatten/develop the box. PTC 48 of 52

49 To allow you to produce the physical box using the flat pattern Create a new File, this time specifying Drawing with a name of BOX_DEVELOPMENT, Click OK. In the next menu select Empty with format and select A3_FORMAT followed by OK. Pro/ENGINEER will create a new empty drawing. From the RHMB menu select Insert General View and with the LHMB click in the centre of the drawing. In the Drawing View menu and in View Type change the Model view name to FRONT followed by Apply. Change the Categories to View Display and for Display Style select No Hidden, again followed by Apply. You can now Close this menu. At the bottom of the Pro/ENGINEER graphics window you will see some grey text which provides additional information about the drawing.. Using the LHMB double click SCALE: and enter a value of 1, hit the return key to enter this value. You will then see the drawing view change to full size (scale 1:1). Drag the view so that it is positioned freely within the drawing boarder. To help with manufacture Pro/ENGINEER can also display the Fold Lines ; these are lines where the flat pattern is to be folded. Click Show / Erase select Axis followed by Show All. You can now print out this drawing, cut-out the developed shape, and fold it up into the box. and in the menu that appears PTC 49 of 52

50 7.0 10% extra FREE As part of the product launch the marketing team has decided to produce an introductory offer which will provide an additional 10% for FREE. As the current Deodorant Bottle and packaging has been designed to hold 50ml the fluid capacity of the bottle needs to be increased to 55ml. Due to the complex organic shape of the bottle it s almost impossible to define how much to change certain dimensions to achieve a fluid volume of 55ml. However Pro/ENGINEER can use the previously created Analysis feature to modify the bottle to hold the required volume. This time the Feasibility Analysis will be run in the Assembly. This is required as the changes that will occur will affect a number of different components; the height of the BOTTLE, the position of the CAP, BALL & COLLAR and the size of the BOX. Open/Activate the DEODORANT_BOTTLE.ASM. Create ANALYSIS Feature. Set the Type to Relation and click Next. In the Relations menu type volume = then from menu Toolbar select Insert then change Look In from Assembly to Feature. From the Model Tree expand BOTTLE.PRT and select the FLUID_VOLUME analysis feature followed by OK and then this new assembly relation. to accept the creation of The next step is to set up the Design Optimisation. From the top Toolbar select Analysis>Feasibility/Optimisation. Pro/ENGINEER should have populated the Goal section with VOLUME:ANALYSIS1, change the Goal type to Maximise Abs Val. In the Design Constraints section; click Add and change to Set and enter a value of followed by OK. Click Cancel to close the Design Constraint menu. In the Design Variables section click Add Dimension and then select the BOTTLE_HEIGHT Datum Plane in the Model Tree. This will display the dimension in the graphics window, select this dimension. Enter a Max value of 90mm. PTC 50 of 52

51 To start the Design Optimisation click Compute. (If you want to see the effects of the design changes change the view orientation to FRONT and change the display to wire-frame Compute). before you select Pro/ENGINEER will perform the Design Optimisation, display a graph showing the convergence and modify all the affected components in the assembly. When you click Close Pro/ENGINEER will prompt you to confirm whether or not you wish to keep the changes. Select Confirm. The modelling and design optimisation of the Deodorant Bottle is now complete. Save your files. PTC 51 of 52