Understanding solid works interface
https://drive.google.com/drive/folders/1lV17ZQmfVFj_ArXCBEWRltislyilASsg?usp=sharing
https://drive.google.com/drive/folders/1lV17ZQmfVFj_ArXCBEWRltislyilASsg?usp=sharing
1) Transmission belt-
2) Kick stand
3) Front Fender
4) Rear Fender
Transmission belt-Front plane is selected, the As sketched line option is selected and plotted from one point at origin and the line is made horizontal with origin. The mouse in hovered to second point and a tangency arc is created. At the endpoint of arc another line is created which is extended till a point which is not vertical to the origin. Another arc is created with one of the end point as origin. It is then made tangent by box selection from right to left. Dimension is set for the drawing. The outside entity of the belt is selected by the offset entity.(the reverse is not selected and chain options are selected) as the entity has to be outside. The sketch is boss extruded with a blind end condition and the distance dimension is set.Fillet is applied to the sketch,by selecting an edge ( constant size fillet). The faces and edges where fillets have to be assigned are selected from auto option. Symmetric and circular fillet parameters are set and are applied. The appearance for the sketch is set by selecting the appearance from task pane. The appearance is set as matte rubber for entire part.
Kickstand-The right plane is named as mid plane. A new sketch is made on front plane and an ellipse is made. It is skewed and dimensions are given so that even if the ellipse is rotated the dimensions do not change.( once proper orientation are obtained). The far end points of ellipse are made horizontal. The next sketch is made on mid plane. A spline is sketched ( standard) with one point origin and other on left side of plane.Vertical and horizontal dimensions of spline are set.The spline handles are made horizontal and dragged to set curvature. A reference plane normal to spline is sketched. An ellipse is sketched by tilting the spline and putting a pierce relation so that ellipse is intersecting with spline. The right end point of ellipse is made horizontal to origin and dimension are set for the same. The sketch is lofted ( by selecting lofted boss base) by selecting a suitable point inorder to get a proper loft. A center line spline is selected to make the loft follow the profile. Dome is created at larger ellipse face which is an elliptical dome, same is done for other face. A cut out is made at larger end of ellipse. A rectangle ( center point rectangle –mid point is selected). The dimensions are set for rectangle.An extrude cut is made with through all both. A flat spot is made at end of kickstand. A line with a mid point is made,which is made horizontal and the mid point made vertical with origin. Split tool is chosen and a flat face is created.A circle is sketeched on top plane. An extrude is done on the circle upto the next solid face in both directions. Fillets are made with intelligent sense tool.The sketch is given a metal-chrome appearance.
Front fender-Front plane is named as vertical plane, top plane as center plane and right plane as midplane. A sketch is created in vertical plane. A three point arc is made and relations are assigned as the center point being vertical to origin and endpoints are horizontal. An offset entity is made inward. Two lines are made at endpoints of arc (vertical). The endpoints of the arc are extended to meet the vertical arc and power trim is used to remove the excess part. Revolve is created to get 3d part. This has to be always revolved about an axis. A construction line is made to right of origin (horizontal) and the sketch is revolved using revolved boss base by selecting the line. The angles are assigned in both directions 1 and 2. The appearance is given from the car painted option as sienna. A sketch is made in the central plane to go ahead. A line for construction is made at origin vertically upward. Dynamic mirror entity is chosen ( a mirror line) and a spline is with points at top of construction line, an arbitrary second point and another one which ends at the edge. Dimensions are applied to the spline. The spline handle is made vertical to obtain a smooth curve and curvature is observed a suitable position is selected. Dimensions are set for the spline handle. The split tool is chosen and cut part is selected ( consumed cut bodies is turned on ) and cut is made. Further sketch is made on vertical plane with the edge to be cut at the bottom.A line is made for construction which is coincident at the inside edge to obtain a smooth cut. The dynamic mirror is turned on a spline is made, and dimensions are added. The endpoints are made horizontal with the origin. The spline handles are made vertical and moved to obtain the desired curvature. Split tool is selected to remove the excess part. Fillets are assigned on the external face with tangent propagation on to ensure a smooth transition
Rear Fender-The front plane is renamed as a vertical plane, top plane as center plane and right plane as midplane. Initially sketching is done on vertical plane, by creating a three-point arc above the origin. The endpoints are made horizontal and the center is made vertical to the arc. A line is drawn for construction which is whose endpoints is made vertical to arc endpoint. All dimensions are provided. An offset is made on the arc. Two vertical lines are made at the end of the arc. The corner points of arc are extended to meet the vertical lines. The excess portion of the arc is removed by using power trim. The sketch is revolved using revolved boss. After dimensioning the appearance is given as sienna by selecting car paint appearance from (appearance tab). Sketching is further done on the central plane. A three-point arc is created (upward at the fender top). The endpoints are made horizontal and the center of the arc is made vertical with the origin. The split tool is used to remove the leading edge of the fender. Then fillets are applied by selecting open edges (connected to start face). Another fillet is applied on the outside face followed by shell command on inside to change thickness.