Car Wheel

Draw a sketch using arcs and straight lines to form the profile of the car wheel. Use revolve tool to create the base of the car wheel part. Use the offset entities tool on the left-most arc and draw two vertical rectangles, connecting each end. Use the revolving cut tool to remove material and then mirror this feature about the top plane. Use splines and vertical lines on the front plane to create curved exterior of the center of the car wheel, which requires the revolve tool. Create a new plane coincident with the inner circular edge of the car wheel and then convert the entities of the circle to this plane. Create a sketch that implements an original design of a wheel rim. Create an extruded cut of the single design. Use the pattern tool to create 16 of these features. Create a plane 6.5in offset from the top plane. Use hole wizard to create a counter bored legacy hole in the remaining region of the wheel rim. Use the circular pattern tool to repeat the hole around the central axis five times. Create a circle sketch at the center for the logo of the car brand, which is a through all extruded cut. Create another extruded cut for the hole for the hubcap-sitting region. Use the rollback tool to suppress the hole features and create a circular flat surface on the inside of the car rim. Resume the hole features to implement them into this new extruded base. Make appropriate rounds to all edges of the car rim.

Create the tire part by making a sketch of the cross section of the tire with all the specified dimensions and values. Revolve the most recent sketch to create the tire foundation. Add fillets to the edges of the tires where they are necessary. Create a plane 14in above the tire and use the offset surface tool at a distance of 0 in to replicate the desired surface and hide Fillet 3. On the newly created plane, sketch the original design of the tire tracks. In this case, a zigzag type of tire has been selected. Create a split line curve to project the zigzag sketch onto the desired surface. Resume Fillet 3 and then thicken the desired cut at 0.1 in. Pattern this design about the tire axis 20 times and then mirror the pattern about the right plane.

Create hub cap part by drawing the desired sketch for the wheel hubcap part and adjust for the diameter of your design. Use the revolve tool to create the hubcap base. Use the same procedure as above for offsetting sketches onto surfaces in order to add your initials to the top surface of the hubcap. Make appropriate rounds and chamfers to the edges of the hubcap. Use various mating techniques to assemble the above three parts to create the car wheel assembly.

Landing Gear Assembly

The assembly starts off with the insertion of the strut part. Add the piston part and then mate the outer surface of the top of the piston with the inner surface of the strut with the concentric constraint. Add the wheel hub part and mate its inner top face to the bottom face of the piston with the coincident constraint. Add a concentric constraint to the circular edges of the previously selected surfaces in order to fully constrain the parts. Use a coincident constraint to line up the front plane of the strut and the wheel hub. Add the shaft part and mate its outer surface with the inner hole surface of the wheel hub with the concentric constraint. Use the coincident constraint to align the right plane of the shaft and the front plane of the wheel hub.

Add the upper sway link part and use the coincident constraint to mate the inner hole edge of the upper sway link with the circular edge of the lower left hole of the strut. Add the lower sway link and add the same constraint as above, except between the wheel hub and the lower sway link. Use the coincident constraint to combine the outer right hole of the lower sway link to the inner right hole of the upper sway link. Install the Solid works Toolbox manager and use this to add the necessary screws to connect the assembly. Select the “Heavy Hex Flange – ANSI B18.2.3.9M” screw and select M14 as the size and 100mm as the length. Use the concentric constraint to mate the outer surface of the body of the screw with the inner surface of the holes of the upper sway link. Add a coincident constraint with the bottom surface of the screw head and the top surface of the upper sway link to fully constrain it. Repeat the same procedure for the other two screws.

Go to the design library to add the nuts for each screw. Select the “Hex Flange Nut – ANSI B18.2.4.4M” nut and use M14 as the size. Use the same two constraints as with the screw and the landing gear assembly parts in order to fully constrain the parts. Shorten the length of the screws to insure material cost is minimized. Next, calculate the interference detection, ignoring the first three interferences, and try to resolve the final interference for the upper sway link. Open this part and modify the dimension of cut out depth from 25 mm to 30 mm, which should resolve the interference. Open the hex screw part and the hex nut part and save these parts to the landing gear assembly folder. Lastly, created an exploded view of the part by moving all the parts individually. Start by moving the strut vertically above the assembly and moving the wheel hub & shaft vertically below the assembly. Move the shaft out of the wheel hub and then move Upper Sway Link, bolt and nut located on the right upward and then to the left. Repeat the same procedure for the Lower Sway Link. After the exploded view is finished, create an animation for it that shows how the assembly would be put together.

Support Bracket

The part starts off with a base flange on the top plane, consisting of a 3-mm thick sheet metal part with a rectangular sketch with a semi-circle cut and a small hole at the bottom left area. Next, create an edge flange off the bottom edge of the original base flange, using the bend outside option. Use the unfold option to return the part to its original shape with the bend marks. Create an extended cut in the shape of a triangle on the edge flange. Then, create another base flange on the right side of the sheet metal in the shape of a boot. Create an extended cut on the top surface of the sheet metal in the shape of a boot as well, which consists of a circle and two vertical lines. Next, create an extended cut that consists of a center point arc slot using the center of the previous circle’s sketch as a reference. Now, rebend the original base flange and then create an outer edge flange at the right edge sticking out of the sheet metal. Use the hole wizard on this part to create a specific drill hole in the location shown on the PDF file. Create yet another outer edge flange on the vertical edge under the newly made edge flange, extending until the end vertex of the previous feature. Create a corner relief at the joining of these two recent features to prevent any stress-related failures. Add a few fillets to some sharp edges and then mirror the body about the far right face of the support bracket. Lastly, flatten the part to see the outline or the part and how it would be cut out, and then unflatten the part to get the final product.

Jansen Mechanism

Start by inserting the frame part and set it at the origin. Insert the crank part and mate the hole less end of the crank with the middle hole of the frame. Insert the upper ternary link and mate using a coincident constraint between circular edges of lower right hole of upper ternary link and left hole of frame. Insert the upper coupler and mate coincident between circular edges of the left hole of upper coupler and top hole of upper ternary link. Insert the lower ternary link and mate using a coincident constraint between circular edges of upper left hole of lower ternary link and the remaining hole of the upper coupler. Insert the short lower coupler and mate it to the remaining holes of both the u[per and lower ternary links. Insert the long lower coupler and use mate coincident to assemble long lower coupler to short lower coupler and upper coupler links. Repeat the same procedure to assemble the right side of the mechanism. Note that the right side of mechanism is located on the rear side of crank and frame.

Go into Solidworks Motion and enter the MotionStudy1 tab. Change the animation option to motion analysis. Go into mate and pick assembly Right Plane and Top Plane of the crank. Accept parallel constraint so that the crank is in upright position. Add a motor to the front face of the crank and enter its speed as 60 rpm. Set its frames per second to be 100. Drag the rotary motor simulation key to 10 seconds and calculate the motion study. Set the type of result to Displacement/Velocity/Acceleration à Trace Path. Repeat the same procedure to plot trace curve on the lower hole of right lower ternary link. Retrieve the plot of the x-component for the linear displacement, linear velocity, and linear acceleration plots. Also, retrieve the y-component and z-component of the linear displacement plot.

Housing Cover Drawing

The drawing starts off by opening the part and creating a drawing from the part using the CUSTOM-B-ANSI-INCH template. Start with the top view as the first view and place it at the top left of the drawing sheet. Add a sectional view to the top view at the bottom of it in order to create the front view. Create a projected view of this sectional view in order to create the right view, as well as an auxiliary view at incline located at the top right of the view. Make all of these views with the option Hidden Lines Removed. Add a shaded version of the isometric view at the top right of the drawing sheet. Make a spline around the centerpiece of the auxiliary view and select the crop view option to keep only the view within the spline boundary. Pick the top, auxiliary, and right view, then right-click and select tangent edge, then tangent edges removed. Adjust the options for the lines for all views as described in the respective PDF file and add centerlines for all appropriate views.

Select the model items option and add default dimensions to the entire model and eliminate any duplicates. Use combinations of drag, SHIFT, and CTRL keys in order to move and hide any dimensions for all views. For certain dimensions, such as hole diameter, there must certain specifications added, such as DRILL or THRU – EQUAL SPACED. The smart dimensions option is also used to add any missing dimensions. The hole callout tool is used to provide more detailed information of holes, such as small, patterned holes around a surface. Add surface finish checkmarks to three surfaces on the sectional view of the top view. Go to the auxiliary view of the section view and change the angles of the coordinates of the three holes to 0 degrees so they coincide with the sectional view’s axis. Create a dimension to tell the distance between the centers of the two holes. Next, create an auxiliary sectional view of the original auxiliary view towards the top of the drawing sheet. Use the spline tool crop view tool once again to capture only the bottom of the view, and then drag the 0.3125 dimensions to the newly created view. Add in a note box for the 1 diameter drill hole and say “THESE HOLES FOR INSPECTION, ADJUSTMENT & LUBRICATION”. Insert a new branch at the intersection point of the arrow corner and pass it through the 1.75 diameter core hole. Add another note with no arrows at the lower left corner of the drawing sheet and say “FILLETS & ROUNDS R.125”. Lastly, add the drawing date to the title block of the drawing sheet, making sure that any fonts are adjusted so all components of the title block fit into their appropriate slots.