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ES1310 D17 Introduction to Computer Aided Design Laboratory Exercise #10 – Motion Studies Objectives: In this lab you will learn how to use assembly mates and Motion Studies to animate  a mechanism and simulate assembly sequences. Prep Exercises: Complete the first half of the Solidworks Animation Tutorial found under the Design Evaluation  tab. Select your own choice of color for the base component (not blue). When you have  completed the plunger animation, place a copy of the .avi file in your storage drive folder for Lab  10. Watch the Spur Gear video.  In-class Exercises:  Exercise 1: Double Slider Quick Return Linkage In this exercise, you will model a six-bar linkage using a top-down approach. The linkage is shown in  schematic form in the figure below. You will start with the Quick Return skeleton assembly that contains  a sketch with the fixed slider axis and two reference axes for the fixed pivots A and D. Note that Axis A  passes through the global origin of the assembly file and coincident with the z-axis. The sketch with the  Fixed Slider Axis is on the Front reference plane. Fixed Slider Axis Moving Slider AxisFigure 2. Double Slider Quick Return Mechanism Figure 3. Skeleton Assembly file with pivot axes and fixed slider axis, front view. Parts can be found on the storage drive under course-resources\Lab10\QR Mechanism. Inspect the  parts to understand how they were modeled (you should always do this whenever you obtain parts  from another source, so that you know what you are working with). Similar to the radial engine  assembly demonstrated in class, this mechanism has no fixed base part.  Begin with Link4 Rocker and make a coincident/concentric mate between Axis A and the axis of the hole  at the origin of the link. Mate the front reference planes of the assembly and the link, and then drag the  link to verify that the link has only one Degree of Freedom, rotation about Axis A.  Next, add the Link3 Grooved Slider by making coincident constraints between the front datum planes of  both parts, and the top datum planes of both parts. Is the slider positioned properly in the slot? How  were the parts modeled to facilitate this assembly? Verify that the assembly now has 2 DoF – the rocker  can pivot about Axis A and the slider can translate along the link in the slot.  Add Link2 Crank next – this link has a coincident/concentric constraint on the fat end with Axis D, but  you cannot mate the reference planes without causing a collision. What should you do? Notice that the  crank is behind the slider block in Figure 2. Choose suitable mates to position the crank properly at Pivot  D on the ground assembly and at Pivot C, the hole in the Grooved Slider. Drag the linkage – Link2 Crank  should be able to make a full rotation. How many DoF does your linkage have now?  Let’s add the Link6 Solid Slider next. Don’t panic over “separation syndrome” – we will connect things up  soon enough. What mates do you need to make the Solid Slider translate along a horizontal plane with  the center of the block aligned with the centerline in Sketch 1? How can you keep it from rotating about  a vertical axis? Your Solid Slider should have 2 DoF now – translation along the Fixed Axis (centerline in  the sketch) and translation in the global (assembly) z-direction. Verify that the slider can move only in  these two directions, and cannot rotate. Our linkage now has a total of three DoF – two in the Solid  Slider and one in the remaining link assembly.  Finally, add the Link5 Dyad. See if you can figure out how to mate this component to the rest of the  parts. Refer to Figure 2 to see which parts are in front or behind other parts. Drag the crank around and  verify that your mechanism has only one DoF. Expand your Mates folder and take a snapshot in  isometric view. Calculate to be sure that you do not have any interferences. While it is fun to drag the linkage around, it is more informative to animate the linkage. It’s always good  to know where you are starting from, so move the crank to a horizontal position. You can’t drag the link  to the exact position that you want, so use a parallel mate between the Top reference planes of the  Link2 Crank and the assembly. Now let’s make a Motion Study, Basic Motion, then add a Motor to the  Link2 Crank axis. Select Rotary Motor, and the edge of the hole in the fat end of Link2 Crank for the  Component/Direction. Flip the arrow if necessary to make the crank rotate counter-clockwise. Choose a  motor speed that will complete one full revolution in the desired time (your choice), and set the  endpoint of the timeline to the correct time. Run your motion study, place your assembly in a FRONT  view, and make a movie for your submissions folder. Save your assembly in your submissions folder (use  Pack and Go). Expand the Feature Manager so that the components in the Mates are all visible, then  make a screen shot with your Timeline, front view, for your report. Figure 4. Lab 10 QR Mechanism screen shot, fully assembled, in isometric view.  Figure 5. Starting the Motion AnalysisExercise 2 – Spur Gears  Watch the spur gear design video if you have not already done so. The tutorial uses a top-down design approach within the assembly file to control the placement of the  gears. The top-down skeleton consists of the sketch containing two circles, which represent the pitch  circles of the chosen gears in the assembly file. Note that these circles are constrained to be tangent in  the sketch. You should start by choosing the gear parameters including the gear ratio, diametral pitch,  pressure angle and tooth numbers. Your gear set should have your own choice of parameters, not the  identical values used in the tutorial. Don’t be sloppy like the author of the video – you should fully  constrain your top-down skeleton sketch, and use construction mode for the circles.  Terminology • In a gearset, the large gear is called the gear, and the smaller  gear is called the pinion. The minimum number of teeth on  the pinion should be 18 for a pressure angle of 20˚, or 12 for a  pressure angle of 25˚.  • The pitch circle is the imaginary circle that rolls without  slipping on the pitch circle of a mating gear. Many important  measurements are taken on and from this circle. The video  uses the pitch circle diameters of 6” and 3” to define the size  of the gears in the defining sketch; note that these circles are  tangent in the skeleton model.  • Diametral pitch is a measure of the number of teeth per inch  of diameter of the pitch circle (NOT along the circumference).  This determines the size of the teeth. For example, in the  video, the diametral pitch is 6; the gear has diameter of 6”,  resulting in 36 teeth, and the pinion has a diameter of 3”,  resulting in 18 teeth. Mating gears must have the same diametral pitch. • Pressure angle is the angle between the line of action (common normal of the tooth surface)  and the direction of the velocity of the gear (tangent to the pitch circle). Gear manufacturers use  standard pressure angles of 14.5˚, 20˚ and 25˚. All gears in the set must have the same pressure  angle. The most common is 20˚, whereas 14.5˚is essentially obsolete. Open a new assembly file and create a gearset as described in the tutorial video. Set up your skeleton  sketch on the front datum plane. Make sure that your sketch is fully constrained. You should have a keyway hole in the center so that you can observe the rotation better. Manually reposition the gears  such that the teeth mesh before trying the “Move Component” method for making the gears move. This  is interesting, but you can‘t make a video by dragging the gears, so we need to add a prescribed motion  to the model.  You are going to add a mechanical mate to simulate the desired motion. View temporary axes and  choose the axes on the gears when selecting the mate. Set the gear ratio based on your desired design. Make sure your gears are lined up properly before you assign the mate or the teeth will collide. Once  you have your mates set up, create a Basic Motion study to show the gears spinning. In the Motion  Study, set the rotational speed somewhere between 1 and 20 RPM depending on how your computer  can process the motion. Change the colors of your gears, change the view orientation, and any other  effects that will make your video interesting. Expand the Feature Manager so that the components in  the Mates are all visible, then take a screen shot of the gears in an isometric view with the mates fully  expanded and the Motion Study timeline. Save a copy of the video file of the gears spinning called  “yourusername_Lab10_gears.avi” in your storage drive Lab 10 folder. Expand Lab 10 Homework can be found in a separate file.  ES 1310 – D17  Lab 2 - Holes, Fillets, Design Tables Lab: 3 Exercises and HW Lab Goals: The goal of this lab is to continue to familiarize yourself with basic SolidWorks tools and features. You will learn to use design tables, which can be utilized to make multiple part configurations in a single part, and practice using geometric relations. Exercise 1: In this exercise you will use the slot tool,  design tables, and the pattern tool to make bars with  equally spaced holes.  Before you begin, watch the video “How to use SolidWorks design tables (parametric part modeling)”  that is on CANVAS.  1. Open a new part document and save the file as “bar.sldprt” 2. In the options menu, set the part to the ANSI drafting standard and MMGS units. 3. Based on the desired final isometric view (with the front face as shown) draw a slot on the appropriate plane using the slot tool. Make the center of the bar at the origin. 4. Make the bar height and length dimensions 20 mm and 160 mm respectively. 5. Make the bar 2 mm thick. 6. Draw a 10 mm circle on the left side of the bar at the center of the radius of curvature for the slot. 7. Use an extruded cut to make a through hole. 8. Use the linear pattern tool to add holes every 20 mm along the bar.9. Take a screen shot of an isometric view of this part with the Feature Manager fully expanded and copy that to your lab 2 submission document. 10. Create a design table so that you will be able to change the size, shape, and number of holes in  the part.  11. Take screen shots of the isometric view for the 5 hole and 3 hole configurations and copy  them to your Lab 2 submission document. Exercise 2 – Hole Wizard The hole wizard is a useful tool in SolidWorks as it includes a wide variety of built in data for standard  sizing and shapes of different types of holes used for various fasteners and slots. In this exercise you will  use a number of different types of holes to see how each of the features functions.  1) Read the SOLIDWORKS Online Help file entries under a) hole -> simple b) hole wizard -> overview c) hole wizard -> hole types Create a cube 5 inches wide by 5 inches long by 3 inches high. Using construction lines on the top face to  draw a square centered on the face spaced 2 inches apart. The center of the block in 3D space should be  at the origin.  Use the hole wizard to place the following holes on the corners of the construction line square placed  clockwise starting in the upper left hand corner.  1. Counterbore hole: ANSI inch, Hex Bolt, ½ inch diameter, close fit, End Condition: Through All,  Set Head Clearance at 0.125 inch, Near Side countersink = 1.175 inch 2. Countersink hole, ANSI Inch, flat head screw (100), 9/16th inch, Loose Fit, Blind for 2.5 inch, no  head clearance. 3. Hole: ANSI Metric, Drill Sizes, Diameter of 1.0, Blind for 1 inch 4. Straight Tapped hole, ANSI Metric, Tapped hole, M4x0.7, Blind for 1.5 inch, cosmetic threads The block material should be made from copper. Use the Mass properties tool to display the mass of the  block and the COM location.  Take a screen shot of the model in a Front view; Wire Frame display mode. Fully expand the feature  manager for the 5x5 block and all of the hole wizard features. Make sure your sketches are fully  defined, which includes the location of the holes.Exercise 3 – Dumb bell – revolve feature In this exercise you are going to create a dumb bell shape using the revolve feature and as many  geometric relationships as possible. These relationships will make our model easier to modify. Review the “Geometric Relations” document included with this lab on CANVAS before beginning. 1) Start a new IPS part file. 2) On the front plane sketch the following lines (the lines currently in blue are lines, the dashed  line in black is a construction line). You can draw a regular line and then convert it to a  construction line as shown below. 3) Use geometric relations to set the two side lengths equal to each other as well as the two  horizontal matching lines. To select both lines, click on one, then hold Ctrl while clicking on the  other. 4) Set the overall length to 8 inches using a global variable, and the inside distance between the  two end pieces to ¾ of the overall length. 5) Make sure the ends of the bar are coincident with the construction line and that the center of  the bar is at the origin. Move the construction line ends so they are coincident with the end  points of the other lines as shown. Make the outside height ¼ of the length and the inside  length 1/5 of the length. 6) Select the Revolve feature 7) Once you have selected the entities for the revolve feature, click the green check mark. Use the  construction line for the axis of revolution. Click “yes” that you would like the feature to be  automatically closed.  8) Take a screen shot of this shape in the isometric view with the feature manager fully  expanded (including the equations tab) and add it to your Lab 2 submission document. 9) Change your global variable from 8 inches to 6 inches. You can do this by modifying the overall  length in the drawing, or go to manage equations by right clicking on “Equations”. 10) Take a screen shot of the modified shape in the isometric view with the feature manager fully  expanded and add it to your Lab 2 submission document. Make sure you expand the  “Equations” portion of the feature manager. 11) Write 1-2 sentences explaining why the screenshot from step 10 does or does not look the  same as the screenshot from step 8.Homework: Based on the block you modeled in the Lab 1 HW, your model for HW in Lab 2 is shown  below:  Lab 1 Lab 2 1 16 2 15 3 14 4 13 5 12 6 11 7 10 8 9 Review HW 2 EXAMPLE PDF. Write out your strategy for creating the model of your part. Include  sketches. Assume that each small measurement line is 10 mm and the large ones are 20 mm.  Use as many geometric relationships as you can in the process of constructing your model. Take a  screen shot of your part with the Feature Managers expanded and add it to your Lab 2 - Homework submission document.  Make sure you label which block you are modeling on your assignment submission document. You can  write the part # right above or below the screenshot of the part. Modeling Strategies Solid Decomposition Geometric Constraints ES1310 INTRODUCTION TO CAD - LECTURE 2Solid PrimitivesProjection ContoursProjection ContoursProjection ContoursStep 1- Decomposition ► Study the part ► Look for primitive shapes ► Don’t forget “negative” space (cuts) ► Look for projection contours ► Look for edge features (fillets, chamfers) ► What is the basic shape before applying edge features? ► Look for “smart” features such as holes, ribs, shells ► What is the basic shape without holes? without fillets? ► Choose a (simple) base protrusion feature ► Many options  ► How would you decompose this part? (see SW parts)Step 2 – Origin and Orientation ► Choose a position for the origin ► Consider design intent ► Is there any symmetry? Put the origin on symmetry planes ► No symmetry? Place origin on a vertex of the base ► Be logical - Keep the part centered or in the positive xyz  octant ► Choose a base sketch plane ► Which view should be the front view?  ► Most descriptive contour should be the front view (most of the  time) ► How is the part used? Does it have a “natural” orientation? ► What is the orientation of the base sketch with respect to  the front view?Your Turn! Decompose these Parts Where will you put the origin? What does the base sketch look like?Step 3 – Base Sketch Geometry ► KISS principle – Keep It Super Simple ► A single loop, no intersecting line segments or arcs ► Identify geometric relationships ► Make rough sketch, approximate size ► Pay attention to automatic constraints as you sketch ► FIRST Add geometric constraints  ► THEN Add dimensions ► Sketch MUST be fully constrained (all BLACK, no BLUE)Identify the Geometric ConstraintsPartially constrained sketch after application of  geometric constraintsFully constrained sketch has 12 geometric constraints, and  only 5 dimensionsHorizontal Vertical Collinear Coradial Perpendicular Parallel Coincident Concentric Equal length Equal radius Midpoint SymmetricSummary – Modeling Strategy ► Decompose the part into simple features ► Basic extrusions, revolves and cuts ► Edge features (fillet, round, chamfer) ► Standard Pick-and-Place features (holes, shells) ► Choose Base Protrusion ► Select origin location and sketching plane ► Sketch Base Profile ► Make sketch ► Add geometric constraints ► Add dimensions ES1310 D17 Introduction to Computer Aided Design Laboratory Exercise #7 - Assemblies Objectives:  The purpose of this lab is to apply the principles of CAD assemblies discussed in lecture to an  assembly in Solidworks.  1. Practice fully constraining individual parts in an assembly.  2. Practice the use of patterns to simplify assembly modeling.  3. Modify similar parts to simplify the modeling process.  Prep Exercises: Put the following parts in a single folder named Lab 7 on your storage drive. We will be building  the Front-support assembly in chapter 3 of your text, so you will need all of the parts.  • Hex Standoff (from Lab 3 prep, pages 3-9 thru 3-15 in your text, not graded) • Triangle Plate (from Lab 3, starting on page 3-31 in your text, not graded) • Angle-13Hole (will be supplied by instructors) • Screw (will be obtained from the toolbox) Complete the Lesson 2 Assemblies Tutorial in SolidWorks You should already have the Tutor1 part from Lab 1.  In-class Exercises: Read all instructions before you begin! Exercise 1: Front-Support Bracket Assembly The Angle-13Hole part is in the ES1310 shared storage folder. To retrieve the file: • Map the drive: \\storage.wpi.edu\academics\courses\ES\ES1310\D17\ • Find the file in the course-resources\Lab 7 Assemblies 1 folder.  • Do NOT drag and drop the file. Use copy-paste to place a COPY of the file in your  working folder with the other parts that you will use to build this assembly.  Front-Support Assembly instructions are provided on pages 3-56 to 3-66 in your text.  Follow the instructions in your text up to Step 647. STOP! You don’t have a screw! Don’t  reinvent the wheel ☺ We are going to use the toolbox to obtain a standard #10-24 x 3/8” round  head machine screw. Open the Design Library tab on the right side of the screen.  Open the Toolbox. Navigate to ANSI inch > Bolts and Screws > Machine Screws1 Click on the Round Head Screw and drag the part to the hole in  the left end of the Angle-13Hole part in the assembly as shown by  the arrows above. Because this part was modeled using the Hole  Wizard, the toolbox recognizes the hole size and automatically  places a #10-32 screw in the hole, in the correct orientation. We  want a #10-24 screw, so use the pull-down menu to select the  proper size. Use the options in the Property Manager to select  0.375 length, Cross Drive Type, and Cosmetic threads.   The screw component is already present in the model, so we can  copy the component. Hold the CTRL key and drag the existing  screw to the third hole from the right end of the Angle-13Hole  part, over the standoff. The screw is copied and mated in the hole! Repeat to place the two  screws at the right end of each horizontal slot in the Angle-13Hole as shown in the image below. 2 Note that these screws are still not fully constrained. Use parallel mates to fully constrain the  screws. Expand each screw in the Feature Manager to select the desired datum plane on the  screw, then select a parallel surface on the Angle-13Hole.  Take a screen shot of your completed assembly with the Mates folder fully expanded. Make sure  that all of the components show in the Feature Manager, the names of all components are not cut  off, and that all of the components are fully constrained (no minus signs in the feature tree).  Exercise 2: Assembling the LEGO bricks You should have two LEGO brick models from Lab  5. Use the Change Appearance icon to change the  color of the bricks so that they are different colors. Do  NOT use RED. Change the color of a single peg on  each brick; in the Color property manager, choose 3 part, feature, or surface filter in the Select Geometry box to color your part selectively.  First Component: Use your own brick first as  the base of the model. Open a new assembly file  and set the units to IPS. Place your brick in the  default fixed position, with the global assembly  origin aligned with the part origin. If your part is  not correctly oriented, float the part and mate the  datum planes to achieve the desired orientation  with the top of the brick facing up, as  demonstrated in lecture.  Second Component: Duplicate your brick in the  assembly by holding down the CTRL key and  dragging the part to a different location. Place your second brick directly on top of the first brick,  aligning the back and left sides of both bricks, the top of the base brick and the bottom of  the second brick. In the assembly, change the color of the second brick. In the Appearance  manager, select At the Component Level to change only one brick’s color. 4 Interference Analysis: Select Evaluate > Interference Detection > Calculate to determine  where interferences occur. The parts will automatically be displayed in semi-transparent mode.  Highlight all of the results in the list to see the red regions in the display. 5 You can use the Section View tool, change to top view, to inspect the interferences. Drag the  orange arrow up to the level of the interferences and recalculate the interferences. Change to top  view. 6 Take a screen shot of the interferences in top view, sectioned as shown in the images below.  Interference results will vary. Notice the peg/cylinder interference in the first image, vs. the  peg/rib interference in the second image, as well as the differences from peg to peg. 7 It is possible that you will not have any interferences. Section your part and submit the  screen shot anyway.  Before the end of class, submit your .pdf or .doc file with screen shots of your Front  Support Assembly and your LEGO brick assembly, sectioned, showing interferences. 8 ES1310 Introduction to CAD – D17 Lab 3 Geometric Relations Lab Goals: In this lab you will learn to control the shape of sketches using geometric relations  (or constraints), select end conditions for basic extrusions and other features, and convert  entities for reuse in the model. These strategies capture design intent and control the geometry  of your parts without excessive or redundant dimensioning. These methods create robust,  flexible and predictable models.  Prep Exercise: Create the Hex-Standoff part on pages 3-9 thru 3-15 in your text. This part  introduces you to the sketch polygon command, constrains the orientation of the hexagon  using a horizontal relation, and uses the Hole Wizard to create a tapped thru hole. You do not  need to pass in a screenshot of this part for grading, but you will need this part for future lab  work, and you must know how to use these tools. Exercise 1: Sketch Relations Create the initial sketch shown on the left. Be messy! Make sure  that there are no green relation symbols and no black lines on your sketch. Everything should  be blue. Notice that the location of the origin is not coincident with any part of the sketch.  Take a screenshot of your Initial sketch, then get to work at constraining the sketch until you  have created the Final sketch on the right. When an entity (line, arc, vertex) is selected, the  property manager will appear at the left, showing all of the relations on that entity, and those  that can be applied. If two or more entities are selected, the property manager will present a  list of possible geometric relations that can be applied. To see a list of all relations in the model,  and count them, use the button in the middle of the sketcher toolbar. Note that  dimensions are also listed here as Distance, Radius, or Diameter Relations. Place the origin at the center of the circle. Try to use as many different types of relations as  possible. When all of the geometric relations have been applied to create the desired shape,  you should have 10 geometric relations.1 | Page Four different types of relations = Unimaginative ☹ Seven different types of relations = Excellent! ☺ The sketch should still be all blue. Now dimension the sketch until all of the entities are black.  You should need only six dimensions. If you need more than 6 dimensions, you have not  applied enough geometric relations.  Take a screenshot of your final sketch, showing all dimensions and relations and the list of  relations in the sidebar. A sample screenshot is shown on the last page of this lab. Exercise 2: Create the bearing shown in Figure 6.60.  Step 1: Begin by creating a solid cylinder as your base feature. Center the cylinder at the origin on the  top datum plane with the given dimensions. Note the placement of the origin, which we will use to  capture symmetry across the Front and Right datum planes in the part. Step 2: Create a new sketch on the top datum plane. We are going to take advantage of the existing  geometry and symmetry to make the next feature, the flange. We are going to build one side of the 2 | Page flange, put the hole in it, then mirror those two features. Let’s start by putting in the centerline. Use the  pull-down on the line command to insert a vertical centerline across the cylinder. Be sure to snap to the  edges of the cylinder using the dynamic sketch relations as shown in the figure below. Hover over the  center of the circle and drag the pointer up to the top of the circle – you should see the vertical relation  symbol in the dynamic sketcher. Pick the yellow point at the top of the circle, then the yellow point at  the bottom of the circle. The result is shown on the right.    Dynamic relations in sketcher – note cursor is at  the top of the circle and shows vertical relation  (white) and point on circle to pick (yellow  diamond). Finished centerline with vertical relation and  coincident relations on the endpoints. The  centerline should be black, indicating that it is  fully constrained. If not, add the vertical and  coincident constraints manually.  Step 3: Sketch a circle to the right of the part. Select the center of the circle and the origin and add a  horizontal relation. Do NOT dimension the circle yet. Remember the sketching strategy: sketch  geometry, add geometric relations, then dimension. 3 | Page Step 4: Draw two lines from the large circle to the small circle as shown in the figure below; watch the  dynamic sketcher and try to capture the coincident and tangent relations while sketching. Make sure  that all four endpoints of the lines are both coincident and tangent to the respective circles. To apply the  tangent relation, pick the circle and the line near the end where you want to attach to the circle to make  them tangent. Pick the endpoint of the line and the edge of the circle to make the coincident relation.  The lines are coincident at both ends but only tangent in one place. The lines are both coincident at both ends and tangent at both ends.  Step 5: We need to get rid of the inner section of the small circle using the Trim Entities tool. Select Trim  Entities from the sketcher toolbar, and select Power trim from the menu. Then swipe the cursor across  the inner segment of the small circle. The result is shown below. Close the trim command. 4 | Page Step 6: Try to swipe the right-hand side of the large circle. Ooops! It doesn’t work? Why not? The large  circle is part of the base cylinder sketch, but it is not part of this sketch for the flange. Now what? Should  you sketch another circle on top of it? NO! Use the existing geometry to capture design intent. Select  Convert Entities from the sketcher toolbar, then select the edge of the large circle (Boss-Extrude1). The  edge of the cylinder is projected into this sketch, and now, if we change the main cylinder, the flange  will change with it. Trim away the right side of the large circle. 5 | Page Step 7: Finish dimensioning the sketch. Dimension the radius of the arc. To dimension the center of the  arc, we see two dimensions on the figure 6.60 above – 48mm from the center of the main cylinder to  the center of the small hole, or 96mm between centers of the small holes. What should we do? Which  dimension is more important? For positioning the part in an assembly, the center-to-center distance  between the two holes is critical. But we do not have the left side of the sketch yet. How can we capture  that dimension? Use the centerline! Click Smart Dimension, select the centerline, select the center point  of the arc, and then place the dimension to the left of the centerline. Tah dah! The dimension measures  the center-to-center distance between the holes, which are not there yet! Make sure that all of the  sketch entities are black (sketch is fully defined). Take a screen shot of your sketch as shown below for  your lab report.  Step 8: We have the right side completed. Finish  the sketch and extrude the sketch to the correct  thickness. Make the hole on the right side of the  flange using the Hole Wizard. Pre-select the face of  the flange, select Hole Wizard, position, and put the  hole at the center of the arc. The point in the sketch  should be black. Complete the hole specification  with Type ISO Standard, Show custom sizing  14mm, End Condition Up To Next. Complete the  hole feature.  Step 9: Mirror the flange. From the Feature toolbar,  select Mirror from the Linear Pattern drop down menu. In the feature tree flyout, select the Right Plane  as the Mirror Plane, then select the Boss-Extrude-2 and Hole features to mirror. Notice the yellow image  of the mirrored geometry, so the left side will be identical to the right side flange. Always! We have 6 | Page captured symmetry at the sketch level using the centerline for dimensioning and at the part level using  the mirror command.  Step 10: Complete the part by adding a hole through the center and applying fillets to the edges, as  specified on Figure 6.60 above. Turn off the tangent edge display using the main menu bar Options ->  System Options -> Part/Assembly tangent edge display -> Removed. Do NOT attempt to make the 6mm  set screw hole. Submit a screenshot of your finished part, with feature manager fully expanded.  Flex your part! Change the center-to-center flange hole distance. Change the diameter of the center  cylinder. Rebuild the part using the Rebuild (stoplight) icon in the main menu toolbar.  Exercise 3: Model your assigned part from the figures on the next page. Place the global origin and use centerlines to capture symmetry where appropriate. Use construction lines in the sketch to control geometry. Use the Hole Wizard for ALL holes. Use only the dimensions shown on the drawing – do NO  MATH. Submit a screen shot of your most complex profile sketch, fully defined (all black) showing all  relations in the sidebar. Submit a screenshot of your finished part in default isometric view showing  the fully expanded feature manager and the location of the global origin. Part Last Name Figure 11.68 Slotted Bell Crank A – K Figure 11.64 Feeder Guide L – Z

How were the parts modeled to facilitate this assembly?

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7 | Page Use symmetry – only one 55mm  dimension  needed8 | Page Lab 3 Homework: 3 Parts  HW Part 1: Build your assigned part from the figures below. Use robust modeling strategies to select  your base feature and place it relative to the global origin. Use the Hole Wizard for all holes. Use fillet or chamfer features where appropriate. Use only the dimensions shown on the drawing. Do NO MATH! Do not duplicate dimensions - reuse existing geometry, use patterns, or use equations to capture design  intent. Submit two screenshots as described in Exercise 3 above (complex sketch and finished part). Part Last Name Figure 5.77 Slotted Guide A – C Figure 5.78 Pivot Guide D – K Figure 6.39 Offset Trip L - Q Figure 5.71 Mounting Bracket R – Z

What mates do you need to make the Solid Slider translate along a horizontal plane with the center of the block aligned with the centerline in Sketch 1?

How many DoF does your linkage have now?

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9 | Page Figure 5.78 Pivot Guide: Notice the duplicated  dimensions 12mm and  16mm as shown by the red  circles. They should be used  only ONCE in your model.  Notice that 16 + 2*12 = 40, so if you use symmetry  relations, you should need  only one of the two smaller  dimensions. Figure 6.39 Offset  Trip: Large hole is through all, small  hole should be  through next. 10 | Page Figure 5.71 Mounting Bracket : Do  not repeat R15 (shown 3 times) and  40mm dimensions – use equal or  symmetry constraints and equations  as necessary to maintain design  intent. Use equations to make hole  diameter and slot width stay equal.  Part 2: Build the Differential Spider shown in the figure below. Use symmetry and patterns to avoid  using both half-width and full-width dimensions (use one or the other). Do not repeat dimensions. Submit two screenshots as described in Exercise 3 above (complex sketch and finished part). Part 3: Build the Triangle plate in your text, starting on page 3-31. Continue through page 3-3-37 step  307. STOP! Do NOT cut circles. Continue to build the part using the Hole Wizard to place holes in the  positions shown at the bottom of page 3-38, step 338. Fully constrain the hole position sketch using only  the dimensions shown and geometric relations based on the centerline sketch. You should need only  points (no construction lines) in the hole placement sketch. Make one thru all hole feature so that all six holes have the same diameter. Rename the hole diameter for future use in equations. Continue with  steps 344 – 423 to make the slots. You do not need to submit this part, but you will need it for future  labs. You must build your own part, as it will be checked later.11 | Page Sample screenshot for Lab 3 Complex sketch with relations:12 | Page ES 1310 – C17  D 17 Lab 1 – Introduction to SolidWorks  Lab: 4 Exercises  3Lab Goals: The goal of this lab is to familiarize yourself with basic SolidWorks tools and features. You will  work on multiple planes using multiple drawing and feature tools.  Note: An example of how your homework should be submitted is shown below. Remember, all labs  other than this lab are due at the end of the lab period and the lab homework is due before the next lab  begins. These are two different submissions. This lab will be due at Midnight on the day of your lab 1  section. Exercise 1: SolidWorks “Lesson 1: Parts”  1) Open SolidWorks and open a new document.  2) Click Tutorials  3) Select Tutorials  4) Click “Lesson 1: Parts” 5) The SolidWorks window will shrink to the left side of your screen while the tutorial pane opens  on the right side of the screen.  6) Go to options and set the drafting standard to the ANSI standard. 7) Use the controls at the bottom of the tutorial in the side pane to advance through the tutorial  exercise.  8) Continue through the tutorial until you have completed the “Creating the Shell” operation.  9) Take a screen shot of your part in an isometric view with the Feature Manager fully expanded  (all the “+” buttons expanded). Paste the screen shot into a word document that you will be  submitting for this lab. Feature  Manager fully  expanded Notes:  1) You should not have any (-) symbols next to your sketches. If you have (-) signs, it means that  your sketch is under defined and you must edit that drawings to fully define the sketch.  2) If you cannot find a particular tool in the SolidWorks window, you can click on the icon in the  tutorial window, and the location in the SolidWorks window will be highlighted.  3) There are many ways to draw shapes. Feel free to experiment and use the other drawing tools  to make your shapes.    Exercise 2: Drawing on different planes  In this exercise you will be making the same shape on different planes to evaluate the differences in  working on different planes. The final shape is shown here ---------------------------⮴ Open a new part document and change the dimensions to IPS for inches.  [Tools-> Options->Document Properties->Units]  Start on the Top Plane:  2  3  1  4 1) Draw a rectangle centered at the origin (There are many ways to draw rectangles in the  rectangle drawing menu. One allows you to pick the center point of the rectangle) You may use  the numbers on the figure above to follow the order of the buttons to make the rectangle.  2) When dimensioning, create a global variable called “length” equal to 5 inches. (see below and  watch the video associated with this lab for more detail)  3) Dimension the rectangle with a height equal to “length” and a base equal to 2 * “length” (see  below)  4) Extrude the shape to make a brick with a depth of 0.5 * “length”  5) Draw a circle in the center of the top of the brick with a diameter equal to 0.5 * “length”  a. Make sure you fully define the circle at the center of the brick so there is no (-) next to  the sketch  6) Using the circle profile, cut a cylinder half way through the brick ( 0.25 x “length”)  7) Expand the Feature Manager  8) Put the shape in an isometric view with (Display “Shaded with Edges”) (see below)  9) Take a screenshot of the block in the isometric view with the feature managers fully expanded  and add it to your Lab submission document.  10) For the second orientation, start on the front plane and repeat the modeling process.  Alternatively, you can find the “edit sketch plane” command and use this to modify your model. 11) Take a screenshot of this second block in the isometric view with the feature managers fully  expanded and add it to your Lab submission document.  STEP 2 STEP 3  STEP 8   NOTE: You can change equations by right clicking on Equations and selecting “Manage Equations”. If you  want to change dimensions of a given entity within a sketch, you can modify the equation for that name.  (i.e. = “test” *2 ) Exercise 3: Create the part shown -----------------------------------------------------⮴  1) Start a new part file  2) Change the file to ANSI and MMGS  3) Draw a rectangle (75 mm x 50 mm) (think about what plane to start on)  Use a different global variable for each dimension.  4) Extrude the rectangle to a thickness of ½ the block depth (25 mm). Dimension this length using  the global variable created for the 50 mm dimension from step 3.  5) On the front face draw a triangle such that the length of one side is ¼ that of the long  rectangular length and ½ the thickness of the block.  6) Extruded cut the triangular shape 1/3 of the way through the block depth  7) Add 8 mm fillets to the other three corners of the block  8) In the opposite top corner, cut a cylinder through the block. The circle used to draw the cylinder  has a diameter of 1/10 the width of the block (i.e. 5 mm) and is located at the center of the  radius for the fillet. Once you have the circle tool selected, if you are “normal to” the face, when  the mouse gets close to where the center of the circle will be, a small circle with center marks  will appear at the center of the fillet radius. 9) Change the block material to Alloy Steel (Click on the “Materials” label in the feature tree to  change the material)  10) Put the shape in an isometric view with (Display “Shaded with Edges”)  11) Fully Expand the Feature Manager  12) Take a screenshot and add it to your Lab submission document  Homework Exercise 4: Draw your assigned block from the image below. (Block will be assigned in lab)  Assume each small line mark gap is 0.25 inch, the large line mark gaps are 0.5 inch and all holes  are through holes.  Submit this exercise as a screen shot of the isometric views with the feature managers fully  expanded to show that all of the sketches are fully defined. Be sure to state which block you  modeled. Sketch the three principle views (front, top and right) of your object on 1/4" graph paper. Align the views correctly. You can download graph paper at http://www.printfreegraphpaper.com/ Include a scan of your sketch with your screen shot.ES1310 Introduction to CAD – D17 Lab 5 Reverse Engineering Lab Goals: In this lab you will practice decomposing objects and devising modeling strategies  for feature-based parts, use engineering tools to take measurements and reverse engineer a  part, practice multi-view sketching and begin learning about dimensioning. Prep Exercise: DO THIS BEFORE LAB.  Watch the video on using your calipers. Alternative video. Study the LEGO bricks in the photo above. Select a standard rectangular LEGO brick with 4, 6 or 8  dots. Devise a modeling strategy by decomposing the geometry of the brick into primitive and profile  features. Outline your modeling strategy using sketches to identify each feature. Create a multi-view  sketch of your brick (front, top, right and bottom views), including hidden lines and centerlines. Try to  keep your sketches approximately to scale (you may choose a larger scale for clarity, try 2x or 4x) and be  sure to properly align your views. You can print out graph paper online from this link. Bring TWO copies of your multi-view sketch and modeling strategy to lab. Put your student ID number  (not your name) on all pages. The remainder of the lab exercises must be completed during the lab  period. Instructions will be provided in the lab.  BRING YOUR CALIPERS TO LAB. Lab Activities Select a standard rectangular LEGO brick from the collection available in the lab, or bring your  own. Your brick must have at least four pegs on the top (2 x n) and be standard height. (Students who want a greater challenge may choose a non-rectangular brick with permission of  the instructor.) Step 1: Measurements Refer to the video on using calipers. Make sure that your calipers are zeroed before making any  measurements. Measure all of the features on your LEGO block to three decimal places, in inches.  Consider your modeling strategy and the dimensions that you would need to model the part in  SolidWorks. Record the dimensions of your block on BOTH copies of your multi-view drawing. Every  feature should have dimensions of position and location. If you are unable to make a specific  measurement because of limitations in the capabilities of the tools (your calipers), you may estimate the value, but you should note on your sketch that this dimension is an estimate. If you need to calculate a  value based on other measurements, note any calculations on your sketch.  Record the overall length, width, height, wall thickness and peg diameter of your block on the  spreadsheet on the podium computer.  Step 2: Modeling Give one copy of your dimensioned sketch and modeling strategy to the instructor (paper copy). Build  your part using your modeling strategy. Record any missing dimensions that you needed to measure to  complete your model. Note any problems with the modeling strategy that arise.  What to submit: • a screen shot of your model with the feature tree fully expanded, including a bottom isometric  view and the default view • scan of your modeling process sketches, with notes on corrections • scan of your multi-view drawing, with notes on missing dimensions and calculations   Lab 5 Homework  You will receive a copy of a classmate’s sketches. This brick should be a different size from your brick.  Attempt to model the part in SolidWorks using the modeling strategy and dimensions provided by your  classmate. Note any dimensions that you needed during the modeling process that were not previously  recorded with an asterisk, and estimate values if necessary. Note any questions or problems with the  modeling strategy on the sheet. Provide comments and suggestions about the modeling strategy as  feedback for your classmate.  Submit the same items as above. Include a paragraph or two comparing your modeling strategy with  that of your classmate, and explain any challenges or difficulties that you encountered in building the  model from the given instructions and dimensions.  Return the paper copies of the multi-view sketches and modeling strategy to the instructor at the  beginning of the next lab. ES1310 Introduction to CAD – D17 Lab #4 Objectives: Create models using the following Features: Revolved  Base, Shell, Linear Pattern, Fillet, Extruded Base, Extruded Cut,  Hole Wizard, Chamfer, Rib, Revolved Cut, Circular Pattern,  Reference Planes and Reference Axes. Rename a feature or sketch for clarity. Slowly click the  feature or sketch name twice and enter the new name when  the old one is highlighted. Item 1: Create the illustrated model.  Copy and open the model from the provided Lab folder. Utilize the model only as an example. Create your own  model.  Utilize the Rollback bar tool to obtain sketch (planes and  dimensions) and feature information. Start on the Front Plane.  Create an ANSI - MMGS model. Use SOLIDWORKS Help if needed during the lab exercise. Copyright Planchard 2016 Use the Edit Sketch and Edit Feature tool to understand how  the model was created.  Use the Edit Sketch Plane tool to understand the sketch plane  for the sketch in the FeatureManager.  There are no STEP-BY-STEP procedures for this model.  Apply Material to the model. Think about the steps you need to create and dimension each  sketch and feature.  Check your model against the one that you downloaded with  the Mass Properties tool.  Submit the model in an Isometric view; Shaded With Edges  display mode. Display a fully expanded FeatureManager. No  Tangent edges. All sketches must be fully  defined as illustrated.  Display the Mass properties  and the Center of Mass  point on the part.Copyright Planchard 2016 Item 2: Create the Rib Model part. Create the below model from the provided  information. The Base Sketch of this model is the Top Plane. Apply  Material (6061 Alloy) to the model as illustrated in the  FeatureManager. Include the total mass and volume properties of the  model. Submit the model in an Isometric view; Shaded With Edges display  mode. Display a fully expanded FeatureManager. All sketches must  be fully defined. Do not display the origin, tangent edges or geometric relations in the  final model. Use the origin, tangent edges or geometric relations only  during the modeling period. ANSI standard states, “Dimensioning to hidden lines should be  avoided wherever possible. However, sometimes it is necessary  as below. (Sketch 4), for the  Rib feature!Copyright Planchard 2016 Item 3: View Chapter 8 in the SOLIDWORKS Tutorial book, page 8-11 Perform Mass-Volume tutorial 8-5. Include the overall mass and volume properties of the  part.  Use the SOLIDWORKS Online Tutorials for help. Submit the model in an Isometric view; Shaded With  Edges display mode with a fully expanded  FeatureManager. All sketches must be fully defined. Display the mass of the  model.Copyright Planchard 2016 Lab Homework:  Item 1 Create an Ice Cream Cone model. View the  Homework section in Chapter 5 - Traditional Ice  cream cone in the SOLIDWORKS Tutorial book,  page 5-55. Think about where you would start? There are no step-by-step instructions in this  section.  Create all sketches and features for this model.  There are many different ways to create this model. Include Revolve, Extrude, and Rib features. Submit the model in an Isometric view; Shaded With  Edges display mode with a fully expanded  FeatureManager. Copyright Planchard 2016 Item 2: Create the Wheel part in your textbook (pages 5-24 to 5-38) and set the material to 1060  Aluminum Alloy.  Submit a screenshot of your finished part in default isometric view showing the fully  expanded feature manager and the mass properties.Copyright Planchard 2016 Parent-Child Relationships, Datum Features2Parent-Child Relationship • Each new feature (child) is dependent upon referenced  existing features (parents) • The default datum planes and coordinate system are  original features (Adam and Eve) • All references used in the creation of a feature come  from a parent feature ▫ Datum planes used for sketching and orientation of sketch plane ▫ Surfaces and edges used for placement of features ▫ Anything else that is “picked” during the creation of a new  feature 3Parent-Child Relationship • Modeling strategies ▫ keep tree as flat as possible ▫ minimize number of dependents ▫ use datums for sketcher references ▫ use algebraic relations instead of parent-child • Parent features may not be deleted or  suppressed until children are re-routed ▫ i.e. NO orphans! Reference Planes and  Axes (Datums) • Solid protrusion 2  referenced to top face of  block 1 • Cylindrical boss 4  referenced to wedge face,  edges • Axis of hole 7 referenced  to axis of boss56Datum Features • Point • Axis • Plane • Coordinate System Using Datums How would  you model  this part?Using Datums • How would  you model this  part?Using Datums • How would  you model this  part?
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