# CREO.1 MODELING A BELT WHEEL

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1 CREO.1 MODELING A BELT WHEEL Figure 1: A belt wheel modeled in this exercise.

2 Learning Targets In this exercise you will learn: Using symmetry when sketching Using pattern to copy features Using RMB when selecting items Changing dimensioning schema in the sketch Changing existing features Renaming parts Used program is Creo 3.0 M / 24

3 Starting a New Model Create a new model (from Quick Access bar, pressing CTRL+N or from File New) using Part as Type and Solid as Sub-type and name it as belt_roller (Figure 2). Notice that part s (and other objects ) name can t contain an empty space, that s why _-char is used. Creating Basic Geometry Figure 2: New window choices and given name. We need to design a roller for a belt. Select Revolve ( ) from Shapes group. Hold RMB on graphical area and select Define Internal Sketch. The Sketch window opens. Select RIGHT plane as Sketch Plane, TOP as Reference (if not already selected) and Top as Orientation. Click Sketch. Creating a sketch Create Centerline () from Datum group to be an Axis of Revolution for our profile. Select two points from horizontal reference line to attach the centerline to it; MMB to close the tool. The geometry for a belt roller is symmetric, so we can use it while sketching. First, select a (symmetric) Centerline ( ) from Sketching group. Select two points from vertical reference line to attach the centerline to it; MMB to close the tool. Then sketch an open loop containing seven lines using Line ( from Sketching 3 / 24

4 group) as shown in Figure 3. Avoid equal line snapping (shows letter L in green) when sketching. Close the open loop with MMB and the tool with MMB again. We don t care about the dimension values at this state. Figure 3: Sketching lines, a moment before MMB. Several weak dimensions are automatically created. Next we use geometric constrains to clean up the sketch. Select Equal ( ) from Constrain group, select two lines (4 to 3 and 5 to 6) and click MMB. Then click MMB again to close the tool. Hide the planes ( from Graphics Toolbar) to make sketching more clear. Then select all sketched lines by selecting one point outside the lines (a) and hold LMB until all sketch lines are within created box (Figure 4). Then select Mirror ( ) from Editing group and select vertical center line as a mirror line. The sketch is mirrored. Notice, that topmost and bottommost lines are longer than before. 4 / 24

5 Figure 4: Selecting all sketched lines. Now the geometry of our sketch is ready. Next we define dimensions we want to use. In last exercise, we learned how to use Normal tool for basic dimensioning; now we learn how to use it to make a diameter dimension. Select Normal ( ) from Dimension group. Select the topmost horizontal line (1), select the axis of revolution centerline (2), the topmost line again (3) and then click MMB to make a dimension (Figure 5). Using this method and method learned in previous exercise, finish the dimensioning as shown in Figure 6. To make things easier, start dimensioning from the smallest dimension. Figure 5: Making a diameter dimension (line (1), centerline (2) and line (3) again). 5 / 24

6 Figure 6: Ready to accept sketch. When ready, accept the sketch ( or hold RMB and select OK). Now we are back in the part mode. 6 / 24

7 Finalizing the revolve Everything should be fine, accept the feature ( or MMB). Rename the feature as BASE (RMB over the feature, select Rename from the menu or select the feature and press F2). Save the model! Making a Slot for a Belt Next we need some slot for a belt, the smooth surface is not ideal for holding a belt. This slot can be modeled into a previous feature, but to make the model easy to read and change, a separate feature is a must. In general, one function per feature is a good guideline. This allows us to create a fully different kind of a slot to hold a belt in the future; we don t need to go to BASE feature and redefine it. It can be also viewed from manufacturing point of view: The BASE feature is made e.g. with casting and then the slot for the belt is made with a lathe (by removing material, of course). Select Revolve ( ), hold RMB on graphics area and select Define Internal Sketch from the menu. Sketch window opens, select Use Previous. Now we are in the sketching mode, using the same sketching and reference plane as in a previous revolve feature. Open References by holding RMB and selecting References from the menu. Remove TOP from references (we need another reference). Select the topmost edge and both sides from the previous feature as references (Figure 7). Close the References window (Close). Figure 7: References for the sketch (in turquoise). 7 / 24

8 Next we sketch geometry for our slot. Use Line ( ) to create an open loop with three lines as shown in Figure 8. End the loop with MMB and close the tool by pressing MMB again. We don t care about the dimensions values at this point. Use the Equal ( ) constraint and select lines from 1 to 2 and from 3 to 4. Close the tool when ready (MMB). Figure 8: The open profile for the sketch. A moment before pressing MMB. We need that this sketch is symmetric to FRONT plane. This can be done with two ways: using midpoint (creating a point in the middle of a horizontal line and making it consistent to FRONT) or with symmetry (making a centerline to FRONT plane and using symmetry constraint). Let s do it with a middle point. Select Point ( ) from Sketching group. Hover mouse over horizontal line until it offers a midpoint constraint (letter M, Figure 9) and select that point. Now we have a point that is always in the middle of the line. Figure 9: Snapping to midpoint constraint (M). 8 / 24

9 Next we define to the program that we want that this previously created point to be always attached to the FRONT plane. Select Coincident ( ) from Constrain group. Select that previously created point and the vertical reference line that goes through FRONT plane. Close the tool (MMB). Now we have only three dimensions. Finish the dimensioning as shown in Figure 10. Figure 10: Ready sketch. Accept the sketch ( ). We need to define an axis of revolution to our feature, because we didn t create one when sketching. Put Axis Display ( ) on, select the axis that is in the center of the previous feature (there should be only one axis). Set Remove Material ( ) option on. Rename the feature to BELT_SLOT (from Properties tab). When your model looks like in Figure 11, accept the feature ( or MMB). Remember to save the model! Figure 11: Ready to accept the revolve feature. 9 / 24

10 Redefining Existing Features Now we have a dimensional problem: the diameter of the belt contact circle doesn t exist, we only have the whole wheel diameter and the depth of the belt slot. The belt contact diameter is something that we need in our model. It is needed to e.g. calculating the gear ratio; to calculate the gear ratio we don t care about the thickness of the belt. So, let s change our feature in that way that we have the belt contact diameter in the sketch. Click the symbol on the left side of the BASE_SLOT feature, select its internal sketch (Section 1) and click RMB (Figure 12). There are two ways to edit the selected feature: Edit ( ), which allows changing the existing dimensions and Edit Definition ( ), which allows changing the sketch (or feature) definition e.g. sketching new lines, making new dimensions or changing references. Select Edit Definition ( ). Figure 12: RMB menu for internal sketch of BELT_SLOT feature. We are back in the sketching mode. Hold RMB and select References. Notice, that there are only two references (the upper surface of the first revolve feature and the FRONT plane) although as seen in Figure 7 there were four references. This is because the program removes unused references when our feature (BELT_SLOT) is ready. This keeps the sketches clean and interdependence with other features minimal. Select the axis of the previous feature as a reference (Figure 13). To select the axis, be sure that your Axis Display ( ) in Graphical Toolbar is set on. 10 / 24

11 Figure 13: New reference (axis) for the sketch. Next create a (symmetry) Centerline (, from Sketching group) to be on the previously defined reference line (axis A_1). Then select Normal ( ) from Dimension group, select the horizontal line, select the centerline, select the line again and press MMB to create a diameter dimension where your cursor is at that time. (If you select horizontal line only one time, it creates a radius dimension.) The Resolve Sketch window opens (Figure 14). This happens because our sketch is over-constrained; all the demands can t be true at the same time, the sketch has only one degree of freedom in vertical (i.e. only one dimension is needed to define the height of our sketch). The program has listed all constrains that are overlapping each other. Select the 10 mm dimension from the list and select Delete. This removes that dimension and now the height of the sketch is defined by the belt contact diameter. Select MMB to close the Normal tool. Notice that the newly created dimension is colored blue. This means that the dimension is created by the user (strong dimension), but it is not locked. Select the horizontal line, hold LMB and drag the line; you can see that the geometry moves and also the dimension value updates. To prevent this to happen, double-click the diameter dimension and give it a value of 380. Notice that the dimension is now green. When you modify a strong or weak dimension by giving it a new value, program automatically locks that dimension. (This can be done also by selecting the dimension, holding RMB and selecting Lock from the menu.) 11 / 24

12 Figure 14: Resolve Sketch window. When ready, accept the sketch ( or hold RMB and select OK). We are now back in the part mode. Notice that we didn t need to accept the revolve feature. This was because we edited the internal sketch directly. We can also change the internal sketch by selecting Edit Definition for the base feature (BELT_SLOT), selecting Placement tab and then select Edit (or hold RMB in graphical area and select Edit Internal Sketch). When the sketch is closed, the dashboard of the base feature stays active and we can change values there. Making Cuts Our wheel is too heavy; we need to make it lighter. Select Extrude ( ) from Shapes group. Hold RMB on graphics area, select Define Internal Sketch, select FRONT as a sketching plane, TOP as a reference plane and Orientation to be Top. Click Sketch. Sketching Using Arc tool with Center and Ends ( ) from Sketching group, sketch two arcs (from 1 to 2 and from 3 to 3) and then using Line ( ) connect those arcs (Figure 15). Avoid any snapping (i.e. automatic constraint adding). At this moment, we don t care about the dimensions and their values! 12 / 24

13 Figure 15: Sketched geometry. Notice the location of arc s center point. Next we use constraints to redefine the geometry. Select Perpendicular ( ) from Constraint group, select the bottommost arc (3 to 4) and select the line (1 to 3); now the arc and the line are perpendicular. Use the same method with the other straight line (2 to 4). Next, select Horizontal ( ) from Constraint tab, select point 3, point 4 and close the tool with MMB; this makes those points to be at the same horizontal line and thus makes the sketch symmetric to the vertical reference line (Figure 16). 13 / 24

14 Figure 16: Two Perpendicular and one Horizontal constraints created. We need that our cut follows the size of the wheel (i.e. BASE feature). For this reason, select References (from ribbon or from RMB menu) and add two surfaces from BASE feature as shown in Figure 17. Figure 17: Added reference surfaces. 14 / 24

15 Now it is time for dimensions. Select Normal (from ribbon or hold RMB and select Dimension). Select the upper arc, then the upper reference circle and press MMB between those two; this creates a distance dimension between those arcs. Give a value of 10. Use the same method for the lower arc and the reference circle, give also a value of 10. The Normal tool is still active. Select the one straight line, then the other one and MMB between those two; this creates an angular dimension. Give a value of 60. Close the tool with MMB. Your sketch should look like in Figure 18. The sketch is ready, accept it ( ). Figure 18: Ready to accept sketch. Making Extrusion to both sides We are back in the part mode. Notice that the sketch is made in the middle plane of our part and program offers extrusion with value # to a direction of the positive plane side (blue side is positive, red is negative) with Remove Material ( ) option on (Figure 19). 15 / 24

16 Figure 19: Default definition options for the extrude. Default definition for this extrude is not acceptable. First, we don t need any dimensions. We want that this shape is cut through the existing material. Secondly, we want that this cut cuts material to both sides (positive and negative). Select Options tab from Extrude dashboard. Here you can define extrusion types for both sides (Side 1 and Side 2). Select Through All for both sides. Now we are cutting through the material for both directions from the sketching plane (FRONT). If your model looks like in Figure 20, accept the feature. Rename the feature as CUT. 16 / 24

17 Figure 20: Ready to accept Extrude. Notice sketch outline in green. Rounds Our cut s edges are very sharp; let s put some rounds. Select Round ( ) from Engineering group. First we create rounds for the four edges of the CUT feature. Hoover the mouse over one edge as shown in Figure 21. Then right-click until all four edges of CUT feature are highlighted (Figure 22) and then select them with LMB. In general, clicking the right mouse button selects objects (edges, surfaces, planes etc.) in the area of the mouse pointer. Give a value of 10 to be as rounding dimension. 17 / 24

18 Figure 21: Hovering the mouse over one edge of CUT feature. Figure 22: All edges of the feature CUT highlighted using right-clicks, a moment before selecting them. Choose Sets tab and select *New set. Using right click(s) choose all edges as shown in Figure 23. Give a value of 3. Accept the feature (MMB). 18 / 24

19 Figure 23: Selecting edges for second Set, a moment before selecting. Now we have two different kinds of rounds within one Round feature. Sets can be used to clean up the model tree and thus making removing the rounds from model easier (e.g. exporting geometry to other programs). Remember to save your model. Some notes about Intersect When we were selecting edges for rounding, we said to program to select all edges of that feature. This selection method is called intersecting. In Exercise 1.1, we selected certain edges; if we change the geometry enough, the edges may change and thus our rounds will fail. With intersecting we are safer, because we are not referring to certain edge, but to all edges. For example, in Figure 24 the cut geometry is changed, but the Round feature and its sets are untouched. Do not change your model! 19 / 24

20 Multiplying Features Figure 24: CUT feature dramatically changed, but Round feature untouched. To get our wheel balanced, we need more of those cuts. A very bad way to add those is to change the existing sketch and add them there (program understands multiple closed loops). Also a bad way is to make entirely new cuts with the same values. The best way is to use a tool that is designed for multiple features. This tool is called Pattern (, in Editing group). There is one limitation with pattern; it can only multiple one feature, but we want pattern both CUT and Round features. We can do two separate patterns, but a better way is to group two features and then pattern them. Making groups Select the CUT feature from the model tree, hold CTRL and select the Round feature. Now you have both features selected, click RMB and select Group and Group again. Groups can be also used to clean up the model tree by grouping features of s same kind (e.g. all rounds and chamfers as one group). Making patterns Select the newly created group and select Pattern ( from Editing group or RMB and select Pattern); the Pattern dashboard opens. Next we need to define the patterning method. By default Dimension is 20 / 24

21 selected, click on that text on the left in the Pattern dashboard and select Axis from a drop-down menu. Then select the only existing axis in the model (be sure that Axis Display is set on). The program creates a rotational pattern with four instances (copied features, our group is the first instance) using 90 as increment. We want five instances that are divided equal to one rotation (360 ). To divide instances equal, select from the dashboard; the 90 value grays out and 360 lightens. Next change the amount of instances to five (5). Notice that the amount of preview circles (location estimations for the created instances) changes. Notice the vectors with numbers 1 and 2; those are patterning directions (1 director along the angle, 2 radial distance from axis). If the preview looks like in Figure 25, accept the feature. Rename the pattern as CUTS. Figure 25: Ready to accept pattern. 21 / 24

22 Using Edit The spokes look too thin and therefore we need to do something. One option is to redefine pattern and say that we only want four cuts, but then the spokes are too thick. Other option is to change the dimension of the cut (the angular one). Select previously made pattern (CUTS), RMB, select and notice that you can only change pattern s dimension(s) (e.g. amount of patterned features). Therefore, select the arrow symbol left to the pattern s name to see what belongs to pattern feature. You see that there are five groups under the feature. Select first group, RMB, select and notice that you can change all dimensions of that group (the dimensions of the cut and the dimensions of the round). Select the arrow symbol left to the first group to see what is there, select CUT feature, RMB, select and notice that you can only change the dimensions of that feature and the dimensions of the pattern where this feature belongs. Change the angular dimension from 60 to 50 by double-clicking it, giving a new value and hitting ENTER to update the geometry (Figure 26). Notice that all other patterned cuts are also updated. Move the cursor somewhere in the background, click LMB, move it again, click LMB to get out of Edit mode. Remember to save your model. Figure 26: Changed CUT feature. Changed dimension highlighted in bright green. 22 / 24

23 Adding Other Features Create a Round ( ) feature with one set (remember to hold CTRL when selecting multiple edges) and a radius of 4 as shown in Figure 27. Figure 27: Four edges rounded, notice that the geometry is symmetric. Create also a Chamfer ( ) of 4 (45 x D as a type) to eight edges shown in Figure 28. Now our part doesn t have any sharp edges. 23 / 24

24 Figure 28: Eight edges chamfered, notice that the geometry is symmetric. Changing the Name of the Part We have created a belt wheel, but it is named as belt roller; we need to change our part s name to be more corresponding with its function. A bad way to change part s name is through the operating system (Windows), because then all the older versions need to be changed also (and in assemblies you have big problems). Therefore, change the part s name only through Creo. Select File, Manage File and select Rename. Rename part as belt_wheel. Notice that all older versions of that file are also renamed. Save the model. This ends this exercise; your model should look like in Figure / 24

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