The Revolve Feature and Assembly Modeling PTC
Clock Page 52 PTC
Contents Introduction... 54 The Revolve Feature... 55 Creating a revolved feature...57 Creating face details... 58 Using Text... 61 Assembling multiple components... 62 Adding components to an assembly...63 Assembling components...64 Definitions... 65 Assembling the hands...66 Mechanical movement...71 Editing constraints... 71 Finding and deleting a constraint... 72 Adding an offset Constraint...73 Variables and design rules...74 Adding a control variable...76 Creating and editing design rules.. 77 Clock Page 53 PTC
Introduction This unit is designed to introduce the Revolve Feature and techniques for assembling components. The Revolve Feature is useful for developing solids and other shapes that might be made on a lathe, such as wheels, bottles, knobs, etc. You may also use this feature to remove material. Most often you will use this feature as a part of an overall component design that uses many different Pro/DESKTOP features. Most products are made of more than one component. Ballpoint pens, for example, are made from a number of pieces such as a barrel, cap, clip, ink cartridge, etc. In just a pen cap for example, the clip and is made of steel, the rest of the cap is made of plastic. To model a ballpoint pen you would need to make each individual component part and then put them all together in the right way to make the complete pen. The power of Pro/DESKTOP is that your design models are not just pictures of the components you develop, but rather they are recipes for actually producing the component. All the geometry of your design is captured in the software and if the required equipment is available, the part can be manufactured. Of course it is possible to design something in Pro/DESKTOP that cannot be manufactured, so the more you learn about production processes the more realistic your designs will be. In this tutorial you will use the revolve feature to model a clock face. Then you will use the techniques of assembly to put together the clock face with other components that have already been developed. These other components include the clock mechanism, and the second, minute and hour clock hands. If you wish, you can make your own clock hands. You might want to look at the clock mechanism first to determine the size of the shafts that the each hand will need to fit. Clock Page 54 PTC
The Revolve Feature Overview To use the Pro/DESKTOP Revolve Feature you will need two sketches: an axis sketch and a profile sketch. These sketches must be on the same workplane. It is important to name your sketches so you can identify them in the dialogue box that appears when the Revolve Feature is selected. Start Pro/DESKTOP and open a new design. Create a new sketch called axis on the lateral workplane by right clicking on the lateral workplane in the browser window and select new sketch. View onto the workplane (Shift + W). Check to make sure that Pro/DESKTOP is set to use millimeters as the dimension units. Use the pull-down menu Tools > Options and choose Units from the tabs. Select millimeters for both model distances and paper distances. Click O.K. Create an axis sketch Draw a horizontal line about 50mm long through the origin. This must be a single straight line. Tip: You can use the snap to grid values in the main toolbar to make sure you are starting the line at (25, 0) and ending at (-25, 0) to keep the origin points in the middle of the line. Clock Page 55 PTC
Sketching a profile You will be shown how to create the main part of the face profile and then you will define the rim shape yourself. Starting the profile sketch On the Lateral workplane create another sketch called Face profile by right clicking on the lateral workplane icon in the browser window and selecting new sketch. Add the dimension constraints and alter them to the values shown in the drawing on the right. Note: The short horizontal line at the bottom of the sketch has a constraint (4mm) to set the distance from the axis line. This dimension will form the radius of the center hole diameter for the shaft of the clock mechanism to pass through. This shape is not yet a valid profile. Add some extra lines to close the shape. The actual shape is up to you. Consider using a circle or ellipse as a detail for the rim. Don t forget to snip out lines to make a valid profile. Fill a valid profile This technique makes it easy to find out if a sketch is a valid profile. Open the Line menu. Select Toggle Sketch Filled. Your profile sketch should look something like this. If it will not shade, zoom in on the places where lines intersect; check to see if there are any duplicate lines or gaps in the profile. View of profile sketch with Select Constraints tool active Clock Page 56 PTC
Creating a revolved feature Now that you have created both the axis and profile sketches in the previous steps you are now ready to generate a 3D solid using the revolve command. Revolve the clock face profile Click on the Revolve icon or use the pull-down Feature menu and select Revolve Profile The Revolve Profile dialogue box will open. Type 360 (degrees) in the angle box or grab the yellow anchor tag on the design and spin around the axis line to revolve a solid. (You must be in isometric view to do this, shift+i) Change the options to those above, making sure you select the names for the sketches you created for profile and axis. Select OK. The 3D clock face will be generated. Save your design as Clock Face.des Clock Page 57 PTC
Creating face details Duplicating hour marks Now you will add the surface features to indicate the hour positions. Later, you will add numbers using the Text Outline command. Be creative. These are a couple of examples of possible clock faces. Follow each small step but then feel free to change the sketch and regenerate the design to reflect your own ideas. Creating a new sketch and workplane for the hour marks Using the select face tool select the front face of the clock where the numbers will be placed and create a new sketch. Because you selected a new surface, a new workplane will automatically be created. Name the workplane front face and name the sketch face detail. Click on view onto workplane (Shift + W). Drawing and duplicating hour marks Draw a 25mm diameter circle on the centerline at the twelve O clock position about 75mm from the center hole (at Snap to Grid 0,75). Pro/DESKTOP has a tool for duplicating shapes on a rectangular grid or in a circular pattern around an axis origin point. Clock Page 58 PTC
If necessary, you can relocate the axis origin to the center of the clock face with the Reposition Axes command. Use the Workplane pull-down menu or right clicking anywhere in the field and select Reposition Axis. Line the cursor up to the desired spot in the center of the clock and left click. The axis origin point will snap to this new location. The axis origin should be in the center of the clock face to insure the numbers are all centered Make sure the circle you have just drawn is selected by using the select lines tool. It should be highlighted red. Pull-down the Edit menu in the main toolbar. Select Duplicate. A dialogue box will open. Select the Circular tab. Fill-in the values as shown. Select. You should now have 12 circles around the clock face. Use the Extrude Feature command to raise the clock face numbers a small distance above the workplane. Now view your clock face in Isometric (Shift + I) or Trimetric (Shift + T). You now have hour marks. Save your design file. Clock Page 59 PTC
NOTES Clock Page 60 PTC
Using Text You will now insert numbers (text) onto the clock face in the 12, 3, 6, and 9 o clock positions. Before you can do this you will need to delete the circles from certain locations. Using the design model that you have just saved. Delete the circles at the 3, 6, 9, and 12 o clock positions. Pull-down the Line menu and select Add Text Outline. This dialogue box opens. Choose a font from the list and fill-in the rest of the values as shown. Select. The numeral 12 will appear on the design, highlighted. If the number is too large (or small), delete and try another value for the height. Drag the numeral into the number twelve o clock position on the clock. Repeat the above to insert 9, 6 and 3 in the appropriate positions. Note: Any time you change something in your design that requires recalculating you must click on the Update Document icon in the main toolbar (the stoplight) Regenerate the design with the tool. Your 3D-clock face will now have extruded numerals. If you are happy with the design make sure you save your work before going on to the next step. Clock Page 61 PTC
Assembling multiple components Producing assemblies in Pro/DESKTOP Assemblies are a collection of components. The parts are assembled using constraints such as Center axes, Mate or Align. Components (Separate Pro/DESKTOP Designs) Assembly (In new Pro/DESKTOP design) When the constraints allow it, components can be made to move on screen according to mechanical principles. Starting an assembly A new design forms the basis of an assembly. Tip: All components making up an assembly should be separate individual design files saved in a specific location. To produce an assembly file you need to open a new blank design and bring the individual part files in one at a time. Start a New Design. Save it with the name assembly.des. Here are two ways to add components to an assembly. Clock Page 62 PTC
Adding components to an assembly Components can be added in one of two ways. Adding a component assembly menu Open the Assembly pull-down menu. Select Add Component. Open the folder containing your clock components. Select the file for your clock face. Select. The clock face appears, highlighted in the design window. Adding a component drag from explorer Open a small explorer window in front of Pro/DESKTOP. The explorer window should contain the file with the clock components. Drag from explorer into the new design window. Drag one of the clock hands from explorer window onto the Pro/DESKTOP design window. Practice inserting the remaining hands and the clock mechanism using both of these methods. Save your assembly model. Clock Page 63 PTC
Assembling components Assembly constraints Assembly involves selecting surfaces or edges and applying an assembly constraint to the two surfaces. These are different than dimensional constraints in that they control the position of parts relative to each other. Types of assembly constraint The following illustration shows most of the assembly constraints available in Pro/DESKTOP. Align Mate Offset Orient Center Axes Hint: To become familiar with how the different constraints function, try using different constraint commands and then use the edit > undo function erase each one until the correct constraint is obtained. Clock Page 64 PTC
Definitions The Center Axes command aligns cylindrical surfaces on two different components central to each other (like a wheel and an axel). You can align two holes, the inside of a hole and the outside of a cylinder, and two cylinders and in certain instances, you can also use arcs of circles. You cannot directly specify the direction of the alignment, but other constraints will allow you to position exactly where you wish the pats to go. The Align brings the faces of two parts onto the same plane, but not necessarily facing the way you might wish. You might need to use this command on more than one face to get the parts oriented the way you want them. The Mate command connects or mates the faces of two parts together. It s like gluing or welding the parts together Tip: The Mate and Align commands can be used to set up a tangent condition between plane/sphere, plane/cylinder, cylinder/cylinder, sphere/sphere, and cylinder/sphere feature combinations. The Offset command allows you specify a space between two parts that are mated or aligned. This constraint is used for things like spacing the axel of a car equally to the body on both sides. It can be considered to be a spacer. The Orient command lets you select edges or axes and constrain them to be parallel. Pro/DESKTOP rotates the component so that two selected edges become parallel. This command is useful for lining up a keyway or slot. The Orient command is available any time that you select two axes or straight edges. Clock Page 65 PTC
Assembling the hands When assembling two components Pro/DESKTOP will move one or both of the components. When you rotate the hands of the clock the clock should stay in place and only the hands should move. You can use the Toggle Fixed command from the constraints menu to fix the clock face to the design or use the shortcut below. Fixing the clock face Select the Select Part tool. Highlight the clock face. Right click on the clock face. Select Fix Component from the floating menu. Now that the clock face cannot move, the other components can be assembled to it. Tip: You will need to drag components close together and zoom in to make it easier to select the faces to be constrained. Assembling the mechanism Use the arrow keys on the keyboard to turn the design until you can see the back of the clock face. Use the Select Part tool to drag the clock mechanism close to the clock face. (Remember, to move a part you must select it by a click and release of the mouse button now that it is highlighted, click and hold the mouse button and drag the part to a new location.) Use the (select face) tool to select the inside surface of the hole in the clock face. Hold down the shift button to select more than one face, click and select the outside cylinder surface of the mechanism shaft. Clock Page 66 PTC
Hold down the Shift key and select the front face of the clock mechanism. You should now have the two surfaces selected. Open the pull-down Assembly menu and select Center Axes. The mechanism will move and line up with the hole of the clock face. Use the (select face) tool to select the front face of the mechanism and the back face of the clock. Once two surfaces are highlighted, the assembly options can be accessed in two ways. For this example you will use the assembly menu. Open the Assembly menu. Select the Mate option. The mechanism will move into position flush with the back of the clock. Fasten the mechanism to the clock with the nut This is another way to center and mate two parts. Using the Edge select tool, select the inside edge of hole in the nut and the outside edge of the clock mechanism spindle. Right click and choose Center axes. Note: You have now used two techniques for the Center Axes command: the Select Faces tool and the Select Edges tool. Using the Select Faces tool select the inside face of the nut and the flat clock face as shown above. Right click and choose Mate. Clock Page 67 PTC
Assemble the hour hand Drag the hour hand near to the spindle center. Highlight the edge of the hole in the hour hand and the edge of the hour drive shaft on the spindle. Right click and select Center axes. Note: The hands are designed with a curved lead in one side to enable the hand to be pushed onto the shaft during assembly. This ferrule should face outwards when assembled Select both the end surface of the large spindle and the face of the hour hand that does not have the ferrule (use Select Faces tool). Right click and select Mate from the floating menu. Clock Page 68 PTC
Assemble the minute and second hands Use the same techniques to assemble the minute hand. Use the select face tool the highlight the inside surface of the hole of the minute hand and the outside surface of the smaller spindle. From the assembly pull down menu click on Center Axes. Use the select face tool to select the front face of the correct spindle step and the face of the minute hand that does not have the ferrule on it. Click on Mate in the assembly menu, or right click in the design and select the mate command. The hand will flip over and mate the two highlighted surfaces. Save your work. Clock Page 69 PTC
When assembled correctly, the ferrule should face outwards on both hands. Bring in the second hand using the add component command. Select the inside of the hole on the second hand and the outside of the spindle it fits onto. Click on Center Axes. Use the select faces tool and select the top surface of the spindle and the bottom face of the second hand. Click on Mate and the clock is now complete. The next step will show you how to move the hands. Clock Page 70 PTC
Mechanical movement It is very easy to make things move in Pro/DESKTOP, provided, the appropriate assembly constraints are in place. Moving a hand Using, the Select Part tool click to highlight one of the hands and release the mouse button. Point directly at the highlighted hand and drag it around the clock face. The hand should rotate, as you would expect the real clock to behave. Editing constraints Principles of variables Pro/DESKTOP automatically keeps track of variables such as dimension constraints, and these can be edited to alter models. Design rules can also be created to control several constraints at once. Formulas can be entered in design rules. The next few steps will show you how to modify the clock assembly to create an exploded assembly where the separation between all components can be controlled using a single variable. Clock Page 71 PTC
Finding and deleting a constraint Pro/DESKTOP automatically keeps track of variables such as dimension constraints and these can be edited to alter models. Design rules can also be created to control several constraints. The mate constraint between the hour hand and the mechanism spindle needs to be deleted and replaced with an offset mate constraint so we can alter it. An offset of 0 (zero) is the same as a mate. But we can also change the offset to some other value and create exploded-view drawings easily. Locating a specific constraint Locating the correct constraint is easily done using the browser. In the Browser pull-down menu select Components. Using, the Select Parts tool, highlight the hour hand. With the hand highlighted right mouse click. From the floating menu select Synchronize Browser. The Browser will highlight the Hour hand item in the list (above). Click on the symbol next to Hour hand. The browser will show the assembly constraints associated with the hour hand. The Mate constraint is the one we want to delete. As a final check, right click on Mate in the browser. Click on Select Defining Geometry. The surfaces making up the mate constraint will highlight on the model. Clock Page 72 PTC
Deleting a constraint Right click on Mate in the browser and select Delete from the floating menu. The hour hand will still be constrained axially on the clock mechanism but will be free to move along the axis. An offset mate constraint will now be added. Adding an offset constraint An Offset constraint can be used to create Align or Mate conditions. We will use the Offset Mate constraint. Initially the offset constraint will be created with a distance of zero. Offset Constraint Drag the hour hand slightly away from the spindle. Select both the face of the end of the spindle and the back face of the hour hand. Right click in the design screen and select Offset The dialogue box will look something like this. Change the variable name Mate 1 to Hour offset. Leave the Offset (mm) at 0. Select. The hand will return to its assembled position. Save your work. Clock Page 73 PTC
Variables and design rules Changing design variables Pro/DESKTOP creates design variables automatically and these can be accessed through the Tools menu. Looking at variables Make sure the file saved at the end of the previous step is open in Pro/DESKTOP. Open the Tools menu and select Variables. A dialogue box will open. Variables are listed against each workplane. The browser on the left works in the same way as the one in the design window. In the example above there are no variables on the base workplane. This is because you are working in an assembly. Click on assembly.des in the top of the Browser window of the variables dialogue box. You will now see assembly variables listed. Clock Page 74 PTC
Changing variables Next to each variable is a column with the heading Value Click next to Hour offset in the Value column and change the number to 40 (mm). Click on in the upper right corner. The hour hand will move 40 mm away from the mechanism. Save your work. Change Mates of other components to Offsets Delete the mate constraint of the other clock hands, the nut and the mechanism and re-constraint each with an Offset mate. You should right-click over the mate; choose Select Defining Geometry. Right-click again and choose Delete and while the surfaces are still selected, right-click in the design window and choose Offset. Be sure to name each offset. If you forget, you can right-click over the Mate offset in the Browser, and choose Properties and re-name. Your variables list should now look something like this: Clock Page 75 PTC
Adding a control variable The variables that already exist in your clock assembly have come from the model. In order to control these variables you need to add a new one. This will be used to control the offsets between components. Add a new variable Pull-down the Tools menu and select Variables. Change the Hour offset Value back to 0. In the Variables window click on. Fill-in the following dialogue. Select. The following line will appear in the list of variables: All of the variables are now in place to control the model. Still missing, however, are the links between them. In Pro/DESKTOP these links are called Design Rules. The next step will show you how to create them. Clock Page 76 PTC
Creating and editing design rules Design rules are added to link and control variables. In this step you will create design rules linking the variable called separation and the mate offsets you created between mechanism, hands and clock face. Open the Variables dialogue box. Notice how the labels given to the mate conditions make it easier to identify what part of the model they control. Reset the Hour offset value to 0. Adding a design rule Open the Tools pull-down menu and click on Design Rules The Design Rule dialogue window opens. In the next part you need to be able to see both Variables and Design Rule windows on screen at the same time. Move the Variables and Design rule windows until they can both be seen on screen. Clock Page 77 PTC
Add a design rule Double click next to the faint check mark in the Design rule window. The entry line opens and a text cursor blinks waiting for input. Clicking on variables is the best way to build a design rule. In the Variables window click on Nut offset. An entry will appear in the design rule window. Click at the end of the new entry and type in an equals sign (=). Click on the variable Separation in the Variables window. Press Enter on the keyboard. The Design Rule will now appear in the window. Well done, you have entered your first design rule! At the moment this will not have any effect on the model. Further design rules must be added to link the Separation value to the Mate offsets. Clock Page 78 PTC
Changing the separation Changing the value of the variable Separation will now control the variable Nut offset. Click next to Separation in the Value column and change the number to 40. Click on a blank space in the window. The nut will move 40mm away from the clock face. The effect is no different from altering a variable directly. The real benefit of design rules will be obvious after the next section. First change the Separation back to zero. Adding further design rules Add these design rules using the same technique. Hint: Remember to add variables to a design rule by clicking on them in the variables window. The equal signs are the only keyboard entry. The asterisk on the other offsets acts as a multiplier that spaces out all the parts. The clock should be assembled normally. Change the value of the Separation variable to 40 (mm). The clock should now look like an exploded assembly! Experiment changing the separation variable. Try values between 0 and 80. Save your work. You can now see the power of design variables. Think of other models that would benefit from this technique. Clock Page 79 PTC
NOTES Clock Page 80 PTC