Modeling an American Chopper
1. Transmission Belt
Commands used: Line, Smart Dimension, Off-set Entities, Extruded boss/base, Fillet.
Step 1: Front plane is chosen for sketching the profile is drawn. The profile is constrained by providing dimensions and relations. After the sketch is drawn, we exit the sketch.
Figure shows: Sketch of the Transmission Belt
Step 2: Extruded Boss/Base is chosen from the features tab and the profile is chosen, with end condition as blind and the dimension is entered as 88mm. The edges of the transmission belt is filleted with 1mm as fillet radius.
Figure shows: Transmission Belt
Step 3: To change the appearance of the model click appearance followed by Appearance> Rubber> Matte Rubber.
2. Kickstand
Command used: Ellipse, spline, smart Dimension, lofted boss/base, Extruded cut, split, Extruded boss/base, fillet
Step 1: Front plane is chosen for sketching the profile which is ellipse and the profile is constrained by giving dimensions and adding relations.
Figure shows: Sketch of the ellipse
Step 2: Right plane is chosen for sketching the centerline path by using the Spline from the sketch tab.
Figure shows: Sketch of the centerline path
Step 3: A new plane is created normal to the centerline path curve and an ellipse is drawn
Figure shows: Sketch of the Ellipse in Created plane
Step 4: Using the lofted Boss/Base command, both ellipse sketches are selected as the profile and the centerline path as the centerline parameter to convert the sketches into solid body.
Then dome command from features tab is used to make both the elliptical edges with elliptical dome, enter the dome dimensions for each elliptical edge seperately and select elliptical dome check box.
Figure shows: Lofted Solid body with Dome
Step 5: Right plane is chosen and then sketched the profile to cut from the solid body to get the required shape, extruded cut command is used to cut that portion from the solid body with condition as through all both
Figure shows: After Extruded Cut
Step 6: The bottom of the kickstand should be flat. To make that, the newly created plane is chosen and the line command is used to sketch the line with the condition of symmetric about the center line, then the dimensions and the relations are given.
The Split command from the Insert> Features> Split is used, the portion which need to cut is selected then choose consume cut body option.
Figure shows: After splitted
Step 7: The extruded cut portion is chosen, sketched the profile that need to extrude and the dimensions and relations are given.
Extruded boss/base command from the features tab is used to extrude the profile, the condition is given as upto next and the edges are filleted using fillet command.
Figure shows: After Extruded
Figure shows: Kickstand
3. Front Fender
Commands used: Center line, Three point Arc, Off-set Entities, Smart dimensions, Trim, Revolved boss/base, Spline, Extruded cut, Fillet
Step 1: Front plane is chosen and the profile that is to be revolve is sketched and is revolved.
Figure shows: Sketch that is revolved
Step 2: Split command is used to cut the body to get the required shape. Two profiles are drawn one on Top plane and the other on front plane. Both the profiles are used for cutting the body using split command.
Figure shows: Sketch of the Profile to cut body in Top plane
Figure shows: Sketch of the profile to cut body in Front plane
Step 3: Fillet commands from the features tab is used to fillet on the edges with the fillet radius as 6mm.
Figure shows: Filleted body
Figure shows: Front Fender
4. Rear Fender
Commands used: :Center line, Three point Arc, Offset Entities, Smart dimensions, Trim, Revolved boss/base, Spline, Extruded cut, Fillet
Step 1: Front plane is chosen and the profile that is to be revolve is sketched and is revolved.
Figure shows: Sketch that profile is revolved
Step 2: Split command is used to cut the body to get the required shape. A profile is drawn on the top plane and is used to cut the body using split command.
Figure shows: Sketch of the profile to cut body in Top plane
Step 3: Four courners are chosen for filleting with the fillet radius as 45mm and the Outer face is chosen for filleting their edges with the fillet radius as 4mm.
Figure shows: Courner and Edge Filleted body
Step 4: Inner surface is chosen to shell and the shell dimension is given as 4mm.
Figure shows: Shelled Body
Figure shows: Rear Fender
OIL TANK
Commands Used: line, centerline, three point arc, point, smart dimension, extruded boss/base, spline, combine, fillet, shell
Front plane is renamed as Midplane oil tank.
Step 1: Top plane is chosen and the profile need to extrude is drawn with the help of dynamic mirror entities command, and then provide the dimensions and relations then exit the sketch
Figure shows: Sketch of the profile to extrude
Step 2: Using extruded boss/base command the profile is extruded with condition as blind and dimension as 170mm in direction and 10 mm in direction 2.
Figure shows: Extruded body
Step 3: Midplane Oil Tank is chosen and the profile need to extrude is drawn with dimensions and relations then exit the sketch
Figure shows: Sketch of the profile on midplane to extrude
Step 4: Using extruded boss/base command the profile is extruded with condition as through all in direction 1 and 2.
Figure shows: Extruded body
Step 5: combine command followed by insert> features> combine is used to get the common body between 1st extrude and 2nd extrude by selecting both the extrude and the condition is selected as common.
Figure shows: combined Common body
Step 6: Fillet command from the features tab is used to fillet on the outer edges with radius as 10mm.
Figure shows: Filleted body
Step 7: To make this body as hollow, shell command from the features tab is used by giving dimension of shell thickness as 3mm and without the selection of any faces from the body, the shell is created in the entire body.
Figure shows: Oil tank
CHAIN
Commands Used: circle, three point arc, center line, Blocks, Extrude boss/base, Fillet, Curve driven pattern, convert entities, Mirror
Planes and their renames are as follows
Front plane as Midplane Chain
Top Plane as Centerplane Chain
Right Plane as Frontplane Chain
Step 1: sketch the shown profile 1 and profile 2 in front plane separately and select the profile 1 and save it as block followed by Tools> Blocks> Save> Chain link 1 and the same as done for profile 2 also but named as Chain link 2
Figure shows: Sketch of the profile 1 to save as block
Figure shows: Sketch of the profile 2 to save as block
Step 2: The path profile for the chain is sketched in the midplane Chain, then the dimension and relations are given.
Figure shows: Sketch of the chain profile
Step 3: For patterning the blocks are inserted followed by Tools> Blocks> Insert, then drag the blocks and add relation to the block and the profile such that the center of the chain link 1 and chain link 2 are in coincidence with the profile and exit the sketch
Figure shows: Sketch of the profile with blocks
Figure shows: Sketch of the Blocks coincidence with profile
Step 4: Now use extrude boss/base command and extrude the only the pins as shown with mid plane and is extruded for 25mm
Figure shows: Extruded pins
Step 5: Now use extrude boss/base command and extrude the only the chain link 1 merge results is unchecked and offset is done for 9.5mm and is extruded for 2 mm
Figure shows: Extruded chain link 1
Step 6: Now use Extrude boss/base command and extrude the only the chain link 2 merge results is unchecked and a vertex point is chosen and extruded for 2mm
Figure shows: Extruded chain link 2
Step 7: Fillet the faces of the pin with fillet radius of 0.5mm
Figure shows: Filleted Pins
Step 8: As the curvature of the sketch profile 1 is not uniform, we cannot use the curve driven pattern to the profile 1. Therefore, individual curves in the profile 1 are selected and curve driven pattern is used to pattern the bodies.
The number of instances is decided by trial and error method. We select a number such that body is just before the end of the curve as shown
Figure shows: Patterned preview
Step 9: Midplane Chain is selected and the chain link 1 and chain link 2 is inserted and Step 3 to step 8 is repeated for the other curves.
The last body is deleted because it is not properly coincided with first body.
Figure shows: Patterned with last body deleted
Step 10: Midplane chain is chosen and the profile is drawn to fill the gap, which is created due to the deleted last body and the profile is shown below
Figure shows: Sketch of the last body profile
Figure shows: Modeled one side of the chain
Step 11: We have modeled only one side of the chain as shown therefore only the chain links 1 and 2 are selected and is mirrored.
Figure shows: Chain
PEDAL
Commands used: line, spline, circle, smart dimension, extruded boss/base, fillet, chamfer, linear pattern, revolved boss/base.
Step 1: Sketch the profile in front plane as shown and add relations to make it constrained.
Figure shows: Sketch of the profile
Step 2: Extrude the profile to 8mm with circle closed by selecting the circles too.
Figure shows: Extruded body
Step 3: Use the same profile to extrude the circles as shaft, select circles to be extrude and extrude it in reverse direction to 20mm. Check merge results
Figure shows: Extruded shaft
Step 4: Sketch the profile in top plane and revolve it to 360 degree. Dome command is used on the face of the revolved body with radius as 3mm and dome is not elliptical. Filleting is done to avoid sharp edges with fillet radius as 1mm.
Figure shows: Sketch that is revolved
Figure shows: Revolved and Domed body
Step 5: Profile 1 is chosen and the next 2 circles are chosen and is extruded to 100mm as shown
Figure shows: Extruded body
Step 6: Chamfer is done in distance distance mode with d1 as 16mm and d2 as 9mm as shown
Figure shows: Chamfered body
Step 7: Chamfer is done in distance & distance mode with d1 as 16mm and d2 as 7.5 mm as shown
Figure shows: Chamfered Body
Step 8: Front plane is selected for sketching and offset command is used to draw the profile as shown
Figure shows: Sketch that is Extruded
Step 9: The profile is extruded for 2.5mm with offset of 20mm, then fillet is done with fillet radius as 1mm
Figure shows: Extruded body
Step 10: The body is chosen for linear pattern with 4 instances and spacing 20mm.
Figure shows: Patterned body
Step 11: Fillet is done with fillet radius as 1mm
Figure shows: Pedal
Front wheel
Commands Used: line, spline, fillet, centerline, smart dimensions, revolve, extruded boos/base, extruded cut, sketch mirror, chamfer, offset entities, trim, three point arc, Intersection curve, revolved cut, circular pattern, combine, appearance
Step 1: Front plane is chosen and the profile that is to be revolve is sketched and is revolved for 360deg.
Figure shows: Revolved Body
Step 2: Right plane is chosen and the profile that is to be extrude is sketched with giving the dimensions and relations.
While Extruded mid plane condition is chosen with dimension as 122mm and deselected the merge results.
Figure shows: Extruded Body
Step 3: Right plane is chosen and the profile that is to be cut is sketched.
Extruded cut is used to remove some area from the body to get the required shape, in the selected contours select the three area which need to be remove and deselect the auto select option and select only the spork where the profile inserted and condition as through all – both.
Figure shows: Extruded Cut body
Step 4: Right plane is chosen and Sketched the profile that to be add with the spork and extruded it with deselected auto select option and only the spork is selected, dimension as up to vertex with the selection of spork vertex in direction 1 and direction 2. With Selected the merge result condition.
Figure shows: Extruded Body
Step 5: Front plane chosen and intersection curve command is used with the selection of inside surface of the rim. Then sketch the profile that to be cut from the Spork to get the required shape and revolved cut command with 360deg is used to remove that portion with deselection of auto-select and select the spork and hub.
Spork is selected and Circular pattern with 3 instances with equal spacing is done and combine the three spork with hub and outer rim with the combine command and filleted on the both faces (front and back) of the spork with fillet radius as 4mm.
appearance for the rim, hub and spork are applied
Figure shows: Patterned, combined and filleted
Step 6: The rotor profile is drawn on the right plane and extruded with offset 45mm and dimension as 7mm, then the small circle of 8mm dia is drawn on the rotor body and linear pattern is done with 4 instance and the dimensions are given.
Extruded cut is used with up to next condition to make the hole with the circles with deselected auto select option and only rotor is selected, then the circular pattern command is used to patter those holes on the rotor with 14 instances with deselected auto select option and selected only the rotor.
The profile to cut from the rotor is sketched and removed using extruded cut and filleted the edges and circular pattern is used with 360deg to pattern it around the rotor with 10 instances with deselected auto-select option and selected only the rotor.
The right plane is chosen and the small circle of dia 14mm is drawn on the hub with center as origin and extruded cut with condition as through all-both.
appearance for the rotor is applied
Figure shows: Rim with Rotor
Step 7: The outer surface of the rotor is chosen and the profile for caliper is drawn and extruded it. Then chamfered by using the chamfer command with dimension, dimension condition is used and filleted by using fillet command.
Dimensions for Chamfer front-side is 6mm and 20mm, chamfer back-side is 20mm and 6mm.
Dimensions for fillet on the two outer edges is 8mm and for other edges is 4mm.
appearance for the caliper is applied
Figure shows: Rim with Rotor and Caliper
Step 8: Front plane is chosen for sketching and intersection curve command is used with selection of outer surface of the rim, then the cross sectional profile for tire is drawn and revolved it.
appearance for the tire is applied
Figure shows: Rim with rotor, caliper and tire
Step 8: Front plane is chosen and the profile to remove from the tire is drawn and extruded cut comment is used with offset option and the dimensions are given.
Filleted with full round condition and the three faces of the stripes are selected accordingly to create the fillet. Then the circular pattern is used to get the stripes around the tire.
Figure shows: Front Wheel
Rear wheel
Commands Used: line, spline, fillet, centerline, smart dimensions, revolve boss/base, mirror, offset entities, trim, three point arc, Intersection curve, revolved cut, circular pattern, combine, extrude cut, chamfer
Step 1: Front plane is chosen and the profile is to be revolve is sketched and revolved.
Figure shows: Revolved Body
Step 2: Right plane is chosen and the profile that is to be extrude is sketched with giving the dimensions and relations.
While Extruded mid plane condition is chosen and deselected the merge results.
Figure shows: Extruded Body
Step 3: Right plane is chosen and the profile that is to be cut is sketched.
Extruded cut is used to remove some area from the body to get the required shape, in the selected contours select the three area which need to be remove and deselect the auto select option and select only the spork where the profile inserted and condition as through all – both is used.
Figure shows: Extruded Cut body
Step 4: Right plane is chosen and Sketched the profile that to be add with the rim spork and extruded it with deselected auto select option and only the spork is selected, dimension as up to vertex with the selection of spork vertex in direction 1 and direction 2. With Selected the merge result condition.
Figure shows: Extruded Body
Step 5: Front plane chosen and intersection curve command is used with the selection of inside surface of the rim, delete the bottom curve and only the top curve is used. Then sketch the profile that to be cut from the Spork to get the required shape and revolved cut command with 360deg is used to remove that portion with deselection of auto-select and select the spork and hub.
Spork is selected and Circular pattern with 3 instances with equal spacing is done and combine the three spork with hub and outer rim with the combine command and filleted on the both faces (front and back) of the spork with fillet radius as 4mm.
The right plane is chosen and the small circle of 60mm dia is drawn on the hub with center as origin and extruded cut with condition as through all-both.
Front plane is chosen, profile of part for connecting the hub with sprocket and rotor is sketched that to be revolve and revolved
Figure shows: Patterned, combined and filleted
Step 6: The rotor profile is drawn on the right plane and extruded with offset 105mm and dimension as 7mm. then the small circle of 8mm dia is drawn and linear pattern is done with 4 instance and the dimensions & relations are given.
Extruded cut is used with upto next condition to cut the sketched profile (circles) area with deselected auto select option and only rotor is selected, then the circular pattern command is used to patter those holes on the rotor with 14 instances with deselected auto select option and selected only the rotor.
The profile to cut from the rotor is sketched and removed using extruded cut and filleted the edges and patterned it around the rotor with 10 instances with only selection of rotor as selected bodies.
Figure shows: Rim with Rotor
Step 7: The outer surface of the rotor is chosen and the profile for caliper is drawn and extruded it. Then chamfered using the chamfer command with dimension & dimension condition is used and filleted using fillet command.
Dimensions for Chamfer front-side is 6mm and 20mm, chamfer back-side is 20mm and 6mm.
Dimensions for fillet on the two outer edges is 8mm and for other edges is 4mm.
Figure shows: Rim with Rotor and Caliper
Step 8: End surface of the hub connector is chosen and the sprocket’s circle profile is drawn and extruded, then chamfered at the both side of edges.
Outer surface of the sprocket is chosen, the profile to be cut on the outer edge of the sprocket is drawn and extruded cut is used to remove the portions and cylindrical pattern is done to apply the removal around the sprocket.
To get the required shape of Sprocket, outer surface of sprocket is chosen and sketched the profile to be remove, extruded cut is used to remove the portion and circular patterning is done.
Figure shows: Rim With rotor, caliper and Sprocket
Step 9: Front plane is chosen for sketching and intersection curve command is used with selection of outer surface of the rim and delete the bottom curve, then the cross sectional profile for tire is drawn and revolved it.
Figure shows: With tire
Step 10: Front plane is chosen and the profile to remove from the tire is drawn and extruded cut comment is used with offset as 400mm and offset from the surface with selection of tire surface and deselect auto select option and select only the tire.
Filleted for the removed profile is done using fillet command with fillet radius as 4mm. Then the circular pattern is used to get the stripes around the tire.
Figure shows: Rear Wheel
Front Fork
Commands used: line, revolve boss/base, circle, extruded boss base, fillet, linear pattern, extruded cut, dome, revolve cut, move/copy body, project curve, sweep, mirror combine
Step 1: Front plane is chosen, the profile to be revolve is sketched and revolved
Figure shows: Revolved body
Step 2: Flat end side of the body is chosen and sketched the profile, then extruded for 40mm with offset for 20mm and deselected merge result.
Filleted all the edges without the edges in the surface as the reference to mirror with fillet radius 5mm
Linear patterned with 2 instances and distance as 240mm
Figure shows: Patterned body
Step 3: Front plane is chosen and the 40mm dia circle is sketched with dimensions and extruded with up to surface condition with the selection of the surface which is going to use as a reference for mirroring. Deselect auto-select option and select only the revolved portion of body.
Figure shows: Extruded body
Step 4: Top surface of the 2nd instance patterned body is chosen and sketched the profile to be extrude and extruded with up to next condition with selection of the 1st instance patterned body. Deselect auto-select option, select only linear patterned, and filleted bodies
Figure shows: Extruded body
Step 5: Front plane is chosen and half the cross sectional profile of head light is sketched for revolve and revolved.
Extruded cut option is used to remove some portion on the front side of the light with sketching the profile to be remove. Filleted on the outer edge with radius as 3mm and inner edge with 1mm at the front end of the light.
Dome is used to make bulb like structure on the front portion of the light with radius as 7mm.
Revolve cut is used to remove some area on the bulb surface with the sketched profile.
Move/copy body command is used to move the light to avoid the intersection with fork.
Figure shows: With light
Step 6: Top surface of the linear patterned 1st instance is chosen and the circle is drawn with dia of 35mm and reference dimensions are given.
Top plane is chosen and sketched the profile of the handle bar when see in top plane.
Front plane is chosen and sketched the profile of the handle bar when see in front plane.
Projected curve command is used with selection for the profiles drawn in both top plane and front plane. With these profiles combination the projected curve create new profile
Sweep command is used with the profile as drawn circle and the path as the newly created profile by the projected cure is chosen
Figure shows: With handle bar
Step 7: The end surface of the handle bar is chosen and the line is drawn horizontally on the center of the surface
New plane is created with first reference as the end surface of the handle bar and second reference as the drawn horizontal line.
New plane is chosen and sketched the profile of the hand rest in handle bar to be revolve and revolved.
Figure shows: With hand-rest
Step 8: New plane is chosen and the profile to be revolve is sketched and revolved
Figure shows: With revolved body near the hand-rest
Step 9: new plane 2 is created with first reference as new plane 1 with 160 deg and reference 2 as the axis of the hand rest.
New plane 2 is chosen and the profile for the clutch lever or break lever is drawn and extruded with mid plane condition and dimension as 15 mm and deselect auto select option and select only the handle bar.
Filleted on the edges using fillet command and the radius used according to the size of that portion
Figure shows: With clutch or break lever
Step 10: like the handle bar drawn the path profile for the clutch or break wire is drawn in the top plane and right plane then projected curve is used to get the combined path profile and the profile is drawn on the lever’s side surface
Sweep command is used with profile as circle and the path as the projected curve.
Figure shows: With clutch or break wire
Step 11: mirror commanded is used to mirror the bodies
Combine command is used to combine the bodies accordingly
Figure shows: Front Fork
New plane is created to make it as a new view by using orientation icon on the top of the screen and select the add view icon and named it accordingly.
Appearance on the bulb surface is changed followed appearance >light >area light and changed the luminous intensity as 1 w/srm^2.
Figure shows: View of Front fork from newly created view
CHASSIS
Commands Used: sketch picture, line, circle, spline, centerline, smart dimensions, swept boss/base, Mirror, Extruded Boss/Base, Extruded Cut, Chamfer, fillet, plane, Dome, Split, combine, revolve boss/base
Front plane is named as Mid-plane Chassis and top Plane is named as Bottom-plane Chain
The picture is inserted by using tools > sketch tool > sketch picture command and their positional dimensions are given.
Sketch the guided profile of the chassis frame, which should be used as a guided curve in swept boss/base. Sketched in different plane according to the profile viewed on that plane.
Then the projected curve command is used to get the actual guided curve profile for each frames in the chassis that to be used in swept boss/base.
Then the edge of the projected curve profile’s are chosen then planes are created and sketched the cross sectional profile of frames with pierce relation is given between the guided profile and cross sectional profile.
Then swept boss/ base command is used get the frame and mirror command is used with selection of the body that to be mirror and about axis also.
Extrude commands are used for the profiles that to be extrude with the constrained sketches.
Split command is used to remove the unwanted portion by the selection of required portion with the selection of consume body option.
Combine command is used with selection of bodies that to be combine.
The profile that to be revolve is sketched and revolved.
Then fillet, chamfer and dome are applied with the respective dimensions.
Figure shows: Chassis
ENGINE
Commands Used: sketch picture, line, circle, Extruded boss/base, Fillet, Revolved boss/base, plane, Circular pattern, Dome, Extruded cut, Chamfer, Linear Pattern, Mirror, Split, three point arc, Swept boss/base, composite curve, projected curve, Combine
The picture is inserted by using tools > sketch tool > sketch picture command and their positional dimensions are given.
Sketched the profile that to be extrude and extruded the portions separately to the required dimensions.
The profile that to be revolve is drawn and revolved it
The plane is created and the profile that to be revolve is drawn and revolved it.
The profile that to be circular pattern is drawn on the respective face, then extruded and circular patterned.
Dome is applied on the respective faces and profile that to be cut is drawn and extruded cut is applied with offset and offset from surface condition.
Chamfer and fillet are done on the respective places.
The profile is sketched and extruded boss/base with draft to required degree in one direction and without draft in other direction to required dimensions and a bottom profile is drawn on the bottom face of the extruded profile and extruded it with condition as up to next. Fillet and chamfer are applied.
Extrude cut profile is drawn and extruded cut is applied and then linearly patterned that cut to get the required shape and filleted. For the small projection on the front side top, the profile is sketched, extruded and domed.
The spark plug connector profile is drawn and extruded, then filleted. To Split the other part from the part to mirror split command with unselecting of consume body is used. Then mirrored that body.
Base stand profiles are drawn and extruded, then filleted.
Sprocket outer profile without teeth is drawn and extruded, chamfered and extruded cut is applied with the sketch for one teeth profile to get the teeth and filleted and then circular patterned it. Then chamfered on the required place with required dimensions.
Then the profiles (guided curve and cross sectional profile) of connector between the two cylinder case, that to be sweep is drawn and swept it and then mirrored for the other side. Combine all the bodies by using combine command.
Sketched the sweep profile (guided curve and cross sectional profile), which connect in the middle of the connector and swept it and at the end of the swept body the profile to be revolve is drawn and revolved it, filleted, extruded cut profile is drawn and extruded cut is applied and circular patterned that cut to get the required shape.
The exhaust silencer profile (guided curve) for the two cylinders are drawn by using two projected curve and one composite curve commands
For front cylinder
1st projected curve combines the profile in front plane and top plane
2nd projected curve combines the profile in right side plane and front plane
Then the composite curve combines the profile of projected curve 1 and 2.
Then the plane is created normal to the curve and coincide at the endpoint the sketched the cross sectional profile the swept boss /base is used with guided curve as composite curve and profile as cross sectional profile.
For rear cylinder
1st projected curve combines the profile in front plane and top plane
2nd projected curve combines the profile in right side plane and top plane
Then the composite curve combines the profile of projected curve 1 and 2.
Then the plane is created normal to the curve and coincide at the endpoint the sketched the cross sectional profile the swept boss /base is used with guided curve as composite curve and profile as cross sectional profile.
At the end of the silencer the body to be sharp edge so the line is sketched and split command is used to remove the portion to get the required profile.
Then the cable for the spark plug is created using swept command with the guided curve and cross sectional profile.
Figure Shows: Engine
Gas Tank
Commands Used: Sketch picture, spline, smart dimensions, Surface Sweep, center line, Surface trim, plane, surface loft, projected curve, boundary surface, mirror, surface knit, split line, surface extrude, fillet, cut sweep, shell
Front plane is named as midplane fuel tank
Top plane is named as bottom plane fuel tank
Right plane named as front plane fuel tank
The picture is inserted through tools> sketch tools> sketch picture command
To sweep the guided profile is drawn in the midplane fuel tank and the cross sectional profile is drawn in the front plane fuel tank and surface sweep is applied.
Bottom plane is chosen, the profile to trim is drawn and surface trim is applied with remove selection and selection the portions to be remove.
Sketch the profile to be surface loft in midplane, the guide curve is drawn in both front plane & midplane and combine them using project curve. Then Surface lofted it.
Project curve is used to combine the profiles in bottom plane and midplane. The boundary surface command is used to create the side portions with the help of projected curve and a straight-line sketch is drawn from the projected curve to upper surface with pierce relation to avoid twists.
Mirror command is used to mirror the surfaces and surface-knit is used to knit all the surfaces.
Profile for the seat is drawn and the split line command is used to split the sketch according to the surface, then Surface extrude command is used with cap end and delete original faces with knit result condition, then filleted.
Boundary surface command and surface commands are used to close the surfaces at the bottom side. Surface knit is applied with all the surfaces with try to form solid condition.
Filleted using fillet command, sweep cut is used to remove the portion of the body to allow chassis frame to assemble with gas tank. Filleted on the cut portion.
Shell command is used without selection any face to shell entire body.
Figure Shows: Gas Tank
Rendered using visualize:
The Chopper is modelled using solidworks and is imported in Visualize environment then the background is selected
Then the view (background image size, chopper angle and size) is adjusted to get the best desired image.
The colour of the chopper parts are chosen and the brightness & gamma values are adjusted. Then the fast render is chosen in rendering selection and then it is rendered.
Some of the rendered images:
Figure shows: Rendered With Decals in Solidworks Visualize
Figure shows: Rendered Without Decals in Solidworks Visualize
Figure shows: Rendered Without Decals in Solidworks Visualize
Figure shows: Rendered with decals in Solidworks Visualize
Thus the parts of the American chopper is modeled, assembeled and then rendered.
Rendered using photo 360:
The model is opened and plain white background is selected and the decals are applied to the chopper parts separately.
In the view settings perspective is selected and then the camera is added and is adjusted to desired position, field of view, aspect ratio are set at preferred levels.
In the rendering option image quality and the gamma values are adjusted to get the desired quality of the image.
Some of the rendered images:
Figure. Rendered in Photoview 360
Figure. Rendered in Photoview 360 (camera view)