Base Support

A centered rectangle, as well as two centerlines in the x-axis and y-axis, should be drawn from the origin. A centered arc tool is used to make the right cut on the rectangle and a mirror tool is used to replicate this feature on the left side. This sketch is then extruded to the specified depth on both sides of the top plane to make the starting base of the part. The edges of the resulting base are rounded in order to enhance the quality of the part, in terms of safety and durability. Next, we extrude on the top plane once again to add the corner ellipse-shaped feature. This is done by making two circles of the same radii and connecting their sides with lines, trimming the interior curve segments. An extrusion of a certain depth is made on both sides of the top plane.

A slot is made on the previous feature by using the offset tool at a specified depth and removing material through all. Next, the left corner pocket feature and its slot are selected on the model tree and mirrored off the right plane to the right side. The bottom corner pockets and their slot features are then mirrored using the front plane to the top corners of the base. A sketch is created on the right plane; a centerline and two reference surfaces are added to make a revolved protrusion. A hole is added to the top of the conical cylinder at a specified diameter through all the material. The conical cylinder is mirrored off the front plane to the top of the base. Next, ribs are created on the outer edges of the conical cylinder using the profile rib tool and sketch on the right plane. The edge of the conical cylinder and the surface of the base are made as reference to create the diagonal line. This line extrudes towards the base and expands out according to the specified thickness of the rib. The final feature can then be mirrored off the front plane to duplicate the result.

A rib is also created between the two conical cylinders to allow for more support centrally. The same process is done for a profile rib, except the tops of the conical cylinders are used as references. Additionally, a sketch is made on the right plane and uses a centered arc to remove material off the top of the center rib at specified dimensions. Then, profile ribs are also created on the left and right sides of the center rib for more support. The first rib starts with a sketch on the front plane with references on the top surface of the center rib and the base surface. This right rib is also mirrored off the right plane to replicate the feature on both sides. A lateral hole featured is also added to the conical cylinder using the hole tool on the right plane. The top and front surface of the base are selected as references for the hole and material is removed through all the material. The result is mirrored with the front plane to the other conical cylinder, completing the “base support” model.

Basketball Rim

The part starts off with a sketch in the top plane, create a circle with a specified diameter and sweep it using a circular cross section of specified diameter. Use notepad and type the data points provided by the PDF file and name the file “rim_support.pts”. Create an offset coordinate system with the current coordinate system as a reference. Import the notepad file and draw a datum curve through all the imported points. Use the sweep feature on this datum curve using a circular cross section with a specified diameter. Create an extrusion and select the front plane as the sketching plane and draw the outline of the bracket with its specified dimensions. Use the thicken feature to add depth to the sketch and extrude on both sides.

Create an extrusion once again with the same details as the previous one, but create the outline for the inner bracket support, including two holes within the sketch. Use the hole feature to create a hole in the back of the bracket and specified location and size dimensions. Use the pattern feature on the hole in the horizontal and vertical direction to created 4 symmetrical holes. Use the rounding tool on the 4 vertical edges of the inside of the bracket and the 4 horizontal edges of the inner bracket at their respective specified values. The color of the part may be modified; otherwise the modeling of the basketball rim reached its completion.

Optimization of a Crank Shaft

Modify the mass properties, specifically the density. Determine the original center of gravity and rename it as COG on the model tree. Measure the distance between the COG and axis 7. Rename it to OFFSET. Measure the distance between the inner and outer edges where the crank and shaft intersect. Rename it to SHOULDER. Run a sensitivity analysis on the R1.35 dimension with the parameters set as the OFFSET and SHOULDER. Click compute and two graphs will be generated: Sensitivity plot of SHOULDER clearance versus radius of balance body & Sensitivity plot of OFFSET distance versus radius of balance body. Run a feasibility analysis with the parameter set as OFFSET. Make constraints for OFFSET, SHOULDER, and VOLUME COG. Use the 40-degree angle, the R1.35, and 0.1852 distance measurements as the specified dimensions.

Compute the feasibility analysis and graphs should be produced for all three parameters, in terms of their optimization limit convergences. Run an optimization analysis on minimization of the VOLUME of COG. Compute the optimization analysis and graphs should be produced for all three parameters, in terms of their optimization limit convergences.

Eccentric Mechanism

Create sub assembly called eccentric_asm with the open the eccentric part. Assemble the shaft to it with coincident constraints. Open clip2, clip1, washer2, and washer1 in order to add Component Interface to the 2 surfaces that will be used for assembly later on. Assemble clip2 to the assembly with 2 coincident constraints to the shaft part. Assemble washer2 to the assembly with 2 coincident constraints to the clip2 part. Assemble clip1 to the assembly with 2 coincident constraints to the eccentric part. Assemble washer1 to the assembly with 2 coincident constraints to the clip1 part. Run Global interferences, confirming that there are no interferences. Create the sub assembly base_asm and start with the base part. Open the bushing part and assemble it with the two smaller holes on the base part with 2 coincident constraints. Assemble the post part to the assembly with 2 coincident constraints to the farthest end hole where the bushing part was originally assembled.

Create a sub assembly called arm_asm and open the arm part. Assemble clip1 to the assembly with 2 coincident constraints to the arm part. Assemble washer1 to the assembly with 2 coincident constraints to the clip1 part. Create the total assembly called eccentric_mechanism open the base_asm sub assembly. Create a pin connection with the eccentric_asm sub assembly at the unoccupied hole with the bushing on it. Check global interference and 3 problems will arise. Measure the distance that the eccentric_asm sub assembly is driven into the base_asm. To do so, create a cut down half the mechanism to see it easier. This is found to be 0.096in. Therefore, to resolve the issue, open the shaft part and add 0.096in to all length measurements. Delete the cut feature and create a pin connection with the arm_asm sub assembly at the post part. Create a pin connection with the link part at the small add-on on the eccentric part. Create a new set to create a pin connection on the other side of the link. Assemble clip2 to the assembly with 2 coincident constraints to the groove of the post part. Assemble washer2 to the assembly with 2 coincident constraints to the clip2 part. Check the global interferences are checked and it shows that the issues were resolved.

Create a velocity servo motor created between eccentric_asm sub assembly and base_asm. Create a position graph of the mechanism motion over a 10 second period. Specify the zero reference and reconnect the bodies of the mechanism. Run a mechanism analysis and make it kinematic. Check for collision detection errors during the playback. There are no interferences and the clip can be saved as a “.pbk” file. Go to the measure button and repeat the above procedure for velocity and acceleration of the mechanism. Pick the joint between link and arm as the measuring location. Create a trace curve by selecting the eccentric_mechanism as the paper part and the edge of the small hole on the arm part as the curve endpoint.

Cam

The process starts off by creating an excel file using a series of displacement values and angle values in separate columns, followed by a third column with zeros throughout the column. This data is converted into notepad and save with the file name “cam_disp.pts”. Next, the extrude feature is used to get the hub of the cam created. The outer diameter is 2.5 in and the inner diameter is 1 in. Next, a datum graph is created and a coordinate system in put in place. From there, a spline is made at the origin followed two other points, creating a hill-looking shape. The spline is selected and then click modify to import the cam graph. First, move to the files tab and then select the coordinate system put in place. After this, you may select the import button and add the “cam_disp.pts” file that was created moments ago.

Next, we must create a second coordinate system that is directly under the first one. Set the distance between the coordinate systems to be 0.5 in, which is the thickness of the cam that will be created. In addition, remove the original coordinate system and finalize the datum graph. Next, conduct a sweep feature and select the bottom edges of the hub. Select the front half first, then press the shift button along with the back edge of the hub. Next, select the variable section option at the top, followed by the section button. Go to sketch view and draw a rectangle at the top of the sketch. Specify the height of the cam to be 0.5 in, and then create a relation in the tools tab for the width. Type in “ /* use evalgraph to determine dimension sd4 = evalgraph(“camgraph”,trajpar*360)”. After this, approve the sketch and the cam should be formed with variable displacements along the perimeter of the hub.

Next, select the surface of the cam and conduct an extrude feature to add the key slot. Create a centerline in the sketch diagonally. This will give a symmetric feature to the key slot, which will be placed right at the top of the hub’s hole. Create a square that is 0.5inx0.5in and place in midway between the hole and the hub material. Remove the material through all to obtain the key slot feature. Lastly, create a sketch on the surface of the cam and draw an arc along the cam with arbitrary dimensions. Create an extrude feature on the same surface and select the text feature. Type in your name in the text box, check the box allowing the text to be placed along the curve, and select the recently made sketch. The name can either extruded on top of the cam or engraved into the cam. Afterwards, a chamfer is made on the inner edge of the hub hole at 45 degrees and a specified value. A round is also made on all the outer edges of the model at a specified value as well. The color of the part may be modified; otherwise the modeling of the cam reached its completion.

Hammer Handle

The part starts off with a revolve feature in the front plane. A horizontal centerline is created and the top half of the provided sketch is created. The sketch is revolved 360 degrees, followed by a set of chamfers at the front, middle and back of the hammer handle base. The chamfers are made with and DxD, 45xD and 45xD, respectively. A second revolve feature is created and the front plane is used as the sketch plane. The top and left end of the thin cylinder are marked as references. A horizontal and vertical centerline is created, where the horizontal centerline coincides with the previous axis of revolution and vertical centerline is 0.472in away from the referenced left end. Sketch a rectangle with specified dimensions, which is clipped to the top reference, to create stress relief for the sweeping manufacturing process. Revolve it about the horizontal centerline and remove material.

Next, a helical sweep is created on the front plane and the remove material option is selected immediately. The same two references are made for this feature as the previous one, as well as a vertical centerline at the left end of the part. Draw a line to represent the trajectory of the sweep, starting from the centerline that is lined up with the top reference, and dimension it to 0.047in. Then, create a section proportional to an upside-down trapezoid that is symmetric with the previously made centerline and forms a 60 degrees angle. Specify the pitch to be 1/20 and accept all changes. This forms the feature of the part that screws into the hammer piece. Another helical sweep feature is created on the front plane, but near the right side of the part where the diameter is larger. References are added to the top plane and right end of the part, as well as a horizontal centerline on the axis of revolution. A horizontal line beginning 0.27in away from the right end of the part creates the trajectory of the sweep. The pitch on the feature is specified to be 2.0693in and an equilateral triangle is sketched symmetrically on the centerline as the section for the sweep. The sweep is accepted and material is removed. Preselect this feature and pattern it about the axis of revolution 12 times at an angle of 30 degrees apart from each other. Preselect this pattern and mirror it about the front plane to create the final design of the hammer handle’s grip area. The color of the part may be modified; otherwise the modeling of the hammer handle reached its completion.

3D Priting of a Card Holder

The part starts off using the revolve feature with reference to the right plane. There are two construction centerlines made in the vertical and horizontal directions of the origin. A quarter-circle is created with a vertical line, two horizontal lines, and an arc connecting the ends of the short horizontal line and the grounded, long horizontal line. The sketch is revolved 360 degrees and forms the base part of the card holder. Next, an extrude feature is created in the top plane and a circle is drawn with a specified diameter. The center of the circle is placed at a specified distance from the two centerlines to create a certain curved shape. The material at the intersection of the card holder base and the sketched circle is removed. This extrude is also mirrored about the front plane to duplicate this feature on the left side.

An extrude feature is performed in the top plane once again, where a circle is sketched at a specified diameter. The center of the circle is also specified at a certain distance away from the two initial centerlines to cut a certain shape at the bottom of the base. Once the sketch is finished, the material is removed to finish the cut. Next, the base is extruded in the right plane with a top orientation. The outer curved surface of the base is used as a reference for the sketch. Three lines are created in a chain that will form the base where the business cards will be placed at the end of the manufacturing process. After the sketch is completed, the sketch is extruded and the material is removed. Another sketch is made on the newly cut surface and the part is viewed using hidden line to see all the present lines. The bottom edge of the previous cut is used as a reference line. A horizontal line is created; its length and distance from the reference line are specified. Then, a conic arc is created that connects the two ends of the horizontal line and the tip of the arc connects to the vertical centerline with a specified arc values and height.

Another sketch is made on the top plane, where another horizontal line and conic arc are created. This sketch also has its own specified dimensions for each aspect of the sketch. After both sketches are made, two datum points are created at the tops of both arcs by selecting the arc and their respective intersecting planes. Once the datum points are made, a sketch is made on the right plane, where the datum points are used as references. An arc is used to connect the points and serves as a trajectory path for the proceeding feature. The previously sketched arc is selected and a swept blend is created. The selected sections option should be selected and the 2 previous conic arc sketches should be selected as the planes used for the swept blend. Afterwards, material is then added in between the two sketches, created a surface for the business cards to lie on for display. In the model tree, the sketches, datum points and datum curves should be hidden. At that point, various rounds are made at the top of the card holder.

The three curved cuts on the side of the model that were made earlier are selected, as well as the bottom of the card holder. At that point, the shell feature is used at a specified 3mm thickness. The shell feature is used again at a specified 0.8mm for any faces located at the bottom of the card holder to remove any excess and unnecessary material. Lastly, a series of rounds are made in sets for various curves and edges at specified values. The color of the part may be modified; otherwise the modeling of the card holder reached its completion.

Helical Extension Spring

A sketch is created that appears as half of a hexagon, where the top and bottom sides of the sketch are constrained to be equal length. After this sketch path is formed, a sweep operation is done, where a sweep cross section in the form of a circle is placed at the bottom end point of the half-hexagon sketch. After the spring is formed, you must edit definition and created variations in the pitch. Specific pitch values are assigned for the start point, the end point, up to 3in, up to 4in, up to 8in, up to 9in and up to 12in.

Afterwards, a new datum plane DTM1 is created through a 12in offset from the top plane. The newly created datum plane DTM1 is used as a sketching plane for the trajectory of the next sweep. In the sketch, a semi circle snapped on the origin of the x- and y- axis. Then, a sweep section is created through the projection of the cross sectional circle of the previous sweep. Afterwards, the front plane is selected and sketch is done to create the trajectory of the final sweep to create the hook feature. Next, a vertical line is created, followed by a semi-circle and a slightly longer vertical line at the end of the semi circle. An arc is used to connect the end of the vertical line to the origin of the sketch. After the sketch finishes, it is preselected and a sweep operation takes place. A circular cross section is created at the start of the sketch at a specified diameter and it is swept along the trajectory path.

For the bottom side of the spring, the same processes are used to create the bottom hook feature. The revolve feature is used at the bottom end of the spring. The cross section of the end of the spring is projected, the central axis of revolution inside the spring is selected in the placement tab, and the right plane is chosen as the final destination in the options tab. Then, a sweep section is created through the projection of the cross sectional circle of the previous sweep. Afterwards, the front plane is selected and sketch is done to create the trajectory of the final sweep to create the hook feature. The top plane is created as a reference for this sketch. Next, a vertical line is created, followed by a semi-circle and a slightly longer vertical line at the end of the semi circle. An arc is used to connect the end of the vertical line to the origin of the sketch. All the values are modified as a group and the radii of the arc and semi circle are constrained to be equal. After the sketch finishes, it is preselected and a sweep operation takes place.

Pen Clip

The process starts off by selecting the planar feature and defining the uniform thickness of the sheet metal. Use the right plane as a reference and add a vertical centerline to the sketch. Create a T-shaped sketch that is symmetrical to the centerline, as well as two fillets at the vertex of the T shape. Next, use the bend feature and select planar 1 in the placement tab. Right click on the part and select rolled bend on both sides. Create a vertical line right down the middle of the T shape and then create references on the two vertical lines and the one horizontal line intersecting the fillets. Set the feature to bend inward at a specified radius and thickness. Next, the unbend feature is used to return the object to its original shape.

Afterwards, the flat feature is selected and set to user defined. The bottom edge of the T shape is used to create a trapezoid sketch, which has the same thickness as the previous part. The flat feature is used once again, with the bottom edge of the trapezoid shape as the sketching reference. A cross shape is sketched that is symmetrical with the vertical centerline. Half of the cross shape in drawn and the remaining half is created through the mirror feature. After the flat surface is made, the bend back feature is used on the top section of the clip to return the original cylindrical-looking bend on the top. Next, the bend feature is used to bend the top section of the cross-shaped fat feature inwards. Make sure to specify that the outside radius option is selected, it is a 90 degrees bend and the bend line is drawn across the designated bending area. The bend feature is used again, with the same specifications as the previous bend, but with a vertical bend line at the right side of the cross shape. In addition, the bend feature is used to create the same bending feature on the left side of the cross shape. The bend feature is used to bend the remaining bottom feature of the cross shape adjacent to the recent two bends with a horizontal bend line. Lastly, the surface of the most recent bend is used as the sketching plane for the final bend. The same specifications are used as the previous bends, but the bend line is made at a specified distance from the referenced lines located at the top of the side bends. Once again, the feature is bent inwards, allowing for the formation of a box at the end of the clip. The color of the part may be modified; otherwise the modeling of the clip reached its completion.

Pump Housing

Create a datum plane through the edge of the semi-circle sweep. Next, select the extrude feature on the DTM1 sketching plane, using the right-most arc as a reference. Sketch a circle that clips to the referenced arc and extrude it as a surface. Next, use the merge tool to combine the extruded and the swept surfaces.

Next, use the extrude feature to sketch a circle on the right plane at a specified diameter and depth. Next, use the merge tool to combine the most recent extruded feature and Merge1. Use the round tool at a specified value to round the intersecting edge of Extrude2 and the swept feature. Next, use the thicken tool on Modify2 and thicken it at a specified value inside the model. In addition, select the revolve feature with the front plane as the sketching plane, with the right vertical line and the top horizontal line as references. Sketch the profile on the right side for the revolve, which consists of an arc, followed by a diagonal line, followed by a horizontal line. Make sure to add a fillet to the vertex between the diagonal and horizontal line. Revolve 360 degrees and use the thicken icon to change the direction of thickening. Do the same procedure for the left side, except that the sketch will consist of an arc and one vertical line.

Next, go to the face of the previous cylindrical extrude and project the inner circle. Also, sketch an outer circle at a specified diameter to create the outlet flange. Afterwards, create a new datum plane DTM2 intersecting the center axis and -30 degrees offset from the front plane. Create another revolve feature using DTM2 as the sketching plane and draw the sketch in a sideways L shape at the edge of the center hole of the part. Next, revolve around the axis by 300 degrees to complete the feature. Next, use the hole feature to create a hole at the beginning of the 300 degrees revolve feature using references, such as an angle of 15 degrees from DTM1 and a diameter of 8.75 on the axis A2. Select the diameter option to create the hole and make sure depth is set to “drill to next surface”. Pattern this hole around A2 with 30 degrees increments and a total of 10 holes. Lastly, go to the outlet flange feature and create a hole with the same procedure, except that the references are axis A5 with a diameter of 5 and the right plane with an angle of 45 degrees. Pattern this hole around axis A5 with 45 degrees increments and a total of 8 holes. The color of the part may be modified; otherwise the modeling of the pump housing reached its completion.

Razor Handle

The process starts off by creating a sketching and drawing a spline from the origin of the coordinate system. The spline contains 5 points, including the origin, that follow a trajectory for the razor. The second point in put under the x-axis and the final three points are above the x-axis. Datum points are then created along the trajectory using the offset option at distances equal to the spline points. The swept blend feature creates the base of the razor handle by drawing elliptical sections at each datum point on the trajectory. Use the reference option and select the trajectory curve as the reference point for all the drawings. While drawing the ellipse on each point, make sure the ellipses are consistently created on top of their center to prevent torsional stress and twisting.

Next, use the rounding feature at a specified value to smoothen the end of the razor. Use the extrude feature with the front sketching plane and select the front edge of the razor area as a reference. Draw a circle at a specified diameter and make sure the drawing snaps to the reference line; this creates the front razor piece. Select the top plane and create a new datum plane with a specified offset in order to place it above the razor handle. Select the new plane DTM1 and use the project feature while viewing the part as hidden line. Reference the central axis of the previously made razor piece and draw two vertical centerlines to its left side. Sketch two circles vertically separated on the first centerline, followed by another circle on the intersection of the horizontal line and the second centerline. Connect the three circles with arcs and delete the inner segments to create a closed sketch. Select the top surface as the reference and project down to get the sketch on the part surface. Confirm the sketch and then use the offset tool to remove a specified depth of material from the curved razor handle. Preselect the razor surface, select the offset option, use DTM1 as the reference plane, and create the sketching section by projecting the previously made sketch. The same project and offset method is used to create the name on the handle area of the part, with the exception of the text tool. The color of the part may be modified; otherwise the modeling of the razor handle reached its completion.

Chain Link

The five parts consist of roller link part, bushing part, roller part, pin link plate part, and pin part. Each part is made with the specified dimensions in the PDF file. Each part is also saved with the parameter of MATERIAL as a string variable “STEEL”. First, the roller link assembly is made and the roller link plate is the starting part. Add the bushing part to the assembly and use the coincident constraint for the outer surface of the bushing and the inner surface of the hole. Also, use a distance constraint for the top surfaces of both parts and make the value 0.005 in. Use the repeat tool to replicate the same constraints to the right hole with the bushing part. Next, add the roller part and use the coincident constraint with the inside hole of the roller and the outer surface of the bushing part. Also, use a distance constraint on the bottom surface of the roller and the top surface of the roller link plate and set the value to 0.01 in. Use the repeat tool to replicate the same constraints to the right bushing with the roller part. Add the roller link plate and use the coincident constraint with the inside hole of the roller link plate and the outside surface of the bushing. Set a distance constraint with the top surface of the bushing and the top surface of the roller link plate and set the value to be 0.005 in. Go to view manager and create a new exploded view called Exp0001 and separate the parts individually. This way, all the parts are level and have their own row for clarity. Afterwards, make sure to save the view and save the sub-assembly.

Next, create the pin link assembly and use the pin link plate as the default part. Add the pin part to the assembly and use the coincident constraint for the outer surface of the pin and the inner surface of the hole. Also, use a coincident constraint for the top surfaces of the pin link plate and the bottom surface of the pin. Use the repeat tool to replicate the same constraints to the right hole with the pin part. Edit the position of the default exploded view in Manage Views and separate the pins evenly above the pin link plate. Save the newly edited exploded view and save the assembly. Finally, create the roller chain assembly and use the roller link assembly as the default part. Add the pin link assembly and use the coincident constraint with the outer surface of the pin and the inner surface of the hole. Also, use the coincident constraint with the bottom surface of the pin link plate and the top of the roller link plate. Add in the roller link assembly and use the same constraints to connect to the right pin of the pin link assembly. Next, pre-select the pin link assembly and repeat it at the empty right hole. Add the pin link plate and constrain it at the bottom of the inner pins of the pin link assemblies. Use the repeat tool to add the same part with the same constraints to the right pin of the second pin link assembly. Go to the analysis tab and select global interference to confirm that there are no interferences causing stress to the part. Lastly, edit the default exploded view to give all parts their own row, similar to the image in the PDF file, and save the default exploded view. The color of the parts may be modified; otherwise the modeling of the roller chain assembly reached its completion.

Syrup Bottle

The process starts off by importing a NotePad file with the data for two curves. Go to get data, import, and select “bottle.ibl” as the file, then two curves are generated. Mirror the left curve about the front plane to produce a right curve. In addition, mirror the bottom curve about the top plane to produce a top curve. Next, create a sketch on the front plane and draw a vertical line at a specified value; this serves as the trajectory. Next, perform a variable section sweep and use the previous sketch as the reference, as well as all four curves while holding the control key. Sketch a section and created a centered ellipse connecting the bottom of all the curves. After the sweep is completed, the base of the bottle is created.

Next, create an extrude feature using the top surface of the bottle and sketch a circle using the project feature. Extrude it at a specified depth in order to create the top for the bottle. Create a round at the intersection of the top and the bottle at a specified value. Also, create a set of rounds at the bottom of the bottle, where the ellipse was drawn initially. Right click the black circle at the dimensions on the model and select “add radius” over the four sections of the ellipse. For each of the 4 points, enter a specified displacement and radius, allowing for a smooth surface at the bottom of the bottle. Afterwards, use the shell feature at a specified thickness and select the top surface of the bottle cap scoop out all the internal material. A helical sweep is then used to create threads on the bottle top so the cap can contain the liquid. Use the front plane as the sketching plane and select the top horizontal surface as a reference, as well as a vertical centerline drawn at a distance from the middle line. Draw a vertical line at the right side of the bottle top at a specified value to serve as the trajectory. Then, create a sketch section in the form of a triangle with a fillet on the right vertex. After the thread is created, select the newly created surfaces at the front and back of the helical sweep and smoothen them out to allow for the cap’s threads to lock in a location, containing the liquid inside. This is done by using the revolve feature and selecting the axis of revolution as the previously made centerline. Project the face of the helical sweep’s face as the sketch and rotate at 57 degrees. This is done for both sides of the helical sweep to smoothen out the ends. Lastly, we want to create the front sketch for where the bottle’s name brand would be added to market the product. Start by offsetting a datum plane off the front plane by any value, as long as it is on top of the model. Use the project feature and use DTM1 as the sketching plane. Sketch the section by creating one large circle on the top area and two equal circles spread out equally on the lower section of the model. Connect the circles with arcs and delete the inner segments to close the sketch. Finish the sketch, select the variable section sweep surface as the surface option, and pick DTM1 as the directional reference. Next, perform a sweep for the previously made sketch and draw a semi circle at a distance away from the horizontal surface and sweep it throughout the sketch as the trajectory. Afterwards, round the inner and outer surfaces at a specified value. The color of the part may be modified; otherwise the modeling of the bottle reached its completion.

Valve Cam Mechanism

Create a sub assembly called rocker_arm and insert the rocker shaft part with default constraints. Open the rocker part and assemble it to the rocker arm with coincident constraints on the axis of each part and a distance constraint on the front planes of each for 25mm. Create the assembly called valve cam and add the shaft mount part with default constraints. Create datum plane 1 offset 25mm from the front datum plane, datum plane 2 at an angle of 112° with the top plane and through the top hole’s axis, datum plane 3 offset 31mm from DTM2, datum axis AA1 between DTM1 and DTM3, datum plane 4 through the axis of the top hole and an angle of 22° from the top datum plane, and datum plane 5 offset -52mm from DTM4. Create a pin connection with the assembly and the rocker arm part, aligning its axis with that of the top hole and the back surface with that of the shaft mount’s back surface. Create a pin connection with the camshaft part, where the axis is coincident with the axis of the lower hole and the back surface is lined up with the back surface of the shaft mount.

Assemble the valve guide part by aligning its axis with AA_1 and its top datum plane is coincident with DTM5. Create a slider connection with the valve and the valve guide by aligning its axis with AA_1 and its right datum plane is coincident with DTM3. Create a cam follower connection between the camshaft part and the rocker part. Create a second cam follower connection using the Front Reference as datum point PNT0 and datum point PNT1 as Back Reference and the curve surface of the rocker part. Create a spring on the valve by selecting PNT0 on valve_guide.prt and PNT0 on valve.prt simultaneously. Use 150 as k, the spring constant. Right-click the rotation axis between camshaft and shaft mount and select apply Servo Motor. Set the value to 12000 deg/sec. Retrieve the graph for its position and keep a snapshot of the graph over a 10 second interval. Run a mechanical analysis of the position, velocity, and acceleration of the mechanism over a 0.2 second interval. This is done by creating 5 measure definitions, including valve_position, valve_velocity, valve_acceleration, spring_load, and servo_load. Retrieve a graph of the position, velocity, and acceleration of the valve cam on a graph simultaneously, as well as on separate graphs. Retrieve a graph of the spring load and servo load on separate graphs as well. Playback your analysis results with collision settings on and then save your playback as a “.pbk” file.

Control Bracket Drawing

The drawing starts off by opening the part and then creating a new drawing. Be sure to select the premade drawing format with the title block. Create a general view of the part, starting with the front view, and then projecting the right and top views from the front view. Next, create another general view, but change the trimetric option to isometric and then add the isometric view to the top right corner. Change the scale of the front, right, and top views to be 0.5. Add the auxiliary view for the top inclined edge of the front view and placed above it, while the left inclined edge of the front view is placed to its left. Present the top, front, right, and auxiliary views in the hidden line format.

Next, create two partial views at the end edges of the auxiliary views and a spline tool. They should appear on the drawing as 2-D cross sections with detailed dimensions for unseen features of the part. Adjust the section lines of the partial views to be half-spaced and 60 degrees. In the drawing properties of the detailed drawing, change values of the detail options to the specified values in the PDF file (ex: text height, arrow style, etc.). Add dimensions to all the views of the drawing through the “ show model annotations” option. Add specific dimensions to each view according to the respective PDF file. Also, be sure to add all the axis for all views to specify revolves and holes easily. Lastly, add a note to the end of the drawing that states: “NOTE: ALL FILLETS AND ROUNDS R.12 UNLESS OTHERWISE SPECIFIED MATERIAL: CAST IRON”.