Tokala Dharshan Kumar

Propellor Yacht

• The first step was to use the appropriate plane and draw or sketch using basic tools like line, spline and many more, also giving appropriate relations and dimensions to the sketches.
• The first part to be sketched is propeller.So,sketching some lines and spline and after that revolving the sketch to get appropriate shape for the propellor.
• The next step is to create blades or fins for the propeller so,used two 3 point corner rectangle to get the shape and direction of the blade.
• After sketching the 3 point corner rectangle,surface loft command has been used to get a solid surface, which will be defined for blades of propeller(making sure that before executing the command, the green balls of the profile of the sketches are on the same side, and if they are not, then we have to manually drag it).
• After completing the above opeeration,giving the solid surface fillets,for its exact appearance,i.e. 135mm for blades.
• Creating an extrude cut to the axle of the propeller, so that it can be assembled in the assembly of yacht with certain or appropriate dimensions.
• After completing the 1 blade operation, using circular pattern tool to get the same solid body around the axle. In circular pattern tool there are options to select the face and the dia to which we want the operations to be done,also the no. of pattern we need to execute and ofcourse the solid body or surface we would like to pattern.(making sure equal spacing is ON to get equal spaces b/w the pattern,giving fine appearance to the body.
• Atlast giving appearance to the whole body,making our first part done.

Radar

• For Radar again starting from the basic step i.e. selecting the appropriate plane i.e. Right plane,and drawing some lines to get the appropriate shape of the Radar and making fully defined by adding dimensions and relations.
• Next step is to create a fillet to make the edges round of the radar. Giving it the basic design of the Radar.
• Using the offset tool as to create a bolt design to the outer surface of the radar. So,we have to use offset tool making sure its inwards, and is changed to construction line. Then creating a circle and extruding it.Again for perfect design using fillet tool.
• Using polygon tool as to get the appropriate shape for the bolt.
• The next step is to use sketch points for the placement of the other three bolts.With certain dimensions.
• As we sketched the points for the other three bolts, now we will use sketch driven pattern to pattern the other bolts on the face of the radar.
• Using the mirror tool to mirror the radar and also merging the solids, knitting surfaces and also propagating the visual properties.
• Adding a text to the Radar with the reference to the centreline and giving it appropriate font, font style,height and space.
• Using the split line tool as to project the text to the surface of the Radar. All we have to do is select the projection type as the type of split, and for the selections we have to select the two surfaces.
• At last changing the colour of the projected text by selecting the text faces and giving it desirable colour.After this step we have finally completed the Radar part.

Blueprints

• Blueprints are very helpful to create a precise design of any part or assembly. So we will be using the blueprints of the yatch model.
• The first step is to select the appropriate plane i.e. front plane. After selecting the plane we have to select the sketch picture option under the tools options and browse the desired picture we want and with the help of the properties i.e dimensions,we can paste the picture anywhere we would like on the screen.
• Doing the same for the other pictures i.e for the other plane such as front plane, top plane, bottom plane,right plane etc also giving them appropriate tangency.
• Changing the blueprints name, to make sure we are on the desired plane of the picture.
• Also created additional planes to paste the sketch along the desired plane according to will.
• Once this process, i.e selecting the plane and adding sketch picture to it, is over then we will get our final results as blueprints for yatch model.

Hull

• For creating the hull, the first step is to open the blueprints and start drawing lines and splines making sure we are matching it with the blueprint for precise design and again making sure providing appropriate dimensions and relations.
• The second step is to give equal curvature relation to the spline and the line also giving dimensions to make the spline fully defined.
• Moving further and again creating more lines and splines to match the blueprint's outer surface line and giving relation like tangent at the contact point of the spline and line.Also dragging the spline handles to match the curves and lines of blueprints.
• Add or create a projected curve using the two sketches made,giving us a 3D fully defined line or curve.
• Next,doing the same for the lower curve of the yatch model, the difference is we will only use spline with only one midpoint and ofcourse giving all the dimensions and relations to make it fully defined including equal curvature option(relation).
• Again creating a projected curve using the last two sketches which has been created.
• Using spline tool again and this time connecting it to both of the curves with the help of peirce relation.
• Doing the same operation at the front side of the yatch i.e. creating a spline and giving it peirce relation to the curves which has been created earlier.
• Executing surface loft tool to create a solid surface to the curves and splines which we have created and also making sure that while dealing with surface loft the profiles which are green in colour should be in the same side after it has been made sure, go to the guided curve option and select the other two curves to make sure that surface is directioned on the same path.
• All the procedure that we have done earlier has to be done again for the bottom part of the yatch model i.e creating line, spline then giving them relations, then executing the surface loft option to get the solid surface.
• Now, the next step is to trim the excessive surface by using the trim option and trim tool, then making sure, remove selection option is checked, then selecting the surface to be trimmed.
• Creating a third loft at the back plane of the yatch model and then creating a new sketch on the midplane and create certain lines and then extruding it blindly, and then again trim the excessive surface bodies.
• When it is all done then knitting the surface to make sure that there are no gaps between the surfaces and if there are,the gap control would take care of it by providing the definite tolerance.
• using the surface fill option to cover the top hollow surface of the hull and then knitting it all over again to form a single body.
• The next step is to use the shell tool to create a shell inside the solid surface with a thickness dia of 120mm.
• Then offsetting the edge of the outer hull lines and expanding its surface by using upto next option and also making sure merge results in on.
• Making other fewer designs by creating or sketching lines and then extruding it with the help of appropriate extruding option.
• Creating a new sketch at the bottom plane for the bottom surface by creating splines and giving relations and dimensions, then used extrude cut option to cut the desired amount of the extruded surface.
• Then adding fillets to the extrudend surface which was created of certain dimensions.
• Sketching the windows for our yatch model with the help of lines and fixing the lines and giving them horizontal and vertical relation.Also sketch fillets for getting rounded corners with desired dimensions.
• After creating one window, using the linear pattern feature the pattern the sketch linearly across the x-axis with the no.of instances we want, in this case we need six of them and when this operation is complete then we have extrude cut the same with the option of offset from surface and selecting desired face and making sure reverse offset is checked on and also translate surface if needed. After giving them fillet feature for smooth design.
• The next step is to design port holes using the slot feature just by sketching the straight slot under slot type and matching it with the blueprint and fixing that slot for fully defined sketch.
• After the completion of the one port hole we can copy and paste the port holes sketches according to our need and by matching the blueprint.
• When all port holes has been copy pasted, then we have to use extrude cut feature with the same option i.e offset from surface and selecting the desired face.
• Used solid sweep feature as to create the outer cover of the port holes by creating a new plane on one of the edge of the port hole and then creating a small circle on that planer and then sweeping it to the outer line of the port hole on which the small circle is created. Doing the same procedure for all the port holes.
• After creating port holes, moving further we have to create cable holes using the same slot feature by manipulating the parameters box and changing the dimensions that we need and also fixing the slot for fully defined sketch.
• Using the extrude cut feature after creating the cable holes and cutting it through all of the surface of the hull.
• Again creating the outer cover for the cable holes as we did for port holes. i.e with the help of solid sweep feature.
• Creating the stairs by sketching the lines and extruding it upto surface with certain dimensions provided on the sketch.
• Creating a new sketch on the bottom plane to create the blades present at the bottom of the yatch with the help of spline without any midpoints and dragging their spline handles to match the curve of the blueprints. After offsetting them and joining them with single lines to make it a close contour and then extruding it with the option of offset from surface with appropriate distance.
• Adding chamfer to those extrudend splines for precise design of the model with the option distance to distance proving D1 and D2.
• Learnt about the helix spiral feature by creating one circle and while its selected we have to go to helix spiral feature and select the parameters as constant pitch and giving certain dimensions for pitch value, revolution value, the start angle and the option to which it has to rotate i.e clockwise or anti clockwise.
• After this is completed we have to use the solid sweep option as we used for port holes and cable holes.
• Next step is to create a new plane near the stairs using the stairs face as inteference. On that new plane create a new 2D sketch and draw a 3 point centre rectangle and giving it relations and dimensions to fully define the sketch, then again using the same rectangle to create a new plane and create a circle at the end point of it and create a solid sweep, same as we have done for port and cable holes.
• Offset the edge of the hull (outer edge) making sure its in upward direction for 335mm and then sketching vertical lines connecting the offset line and the outer edge of the hull, also making sure that matches the blueprint. After that again offsetting the edge to the other side by clicking reverse option. Then trimming the reversed offset line by trim entities option and fixing the whole offsetted curve and vertical lines and giving sketch fillets for rounded corners.
• Again offset the outer edge of the hull, and create a projected curve using both of the sketches and then create a new plane on the end tip of the projected and create a circle and solid sweep on it.
• Learnt above the delete face feature, as after creating the solid sweep some of the part was visible outside of the hull. So, selected that face and clicked and delete face option with Delete and fill option turned on.
• In the rest of the hull pant 3, we have only drawn line sketches to match the exact blueprint and boss extruding them or cut extending them or revolving them to get the desired shape and size.
• Starting for hull part-4, start from sketching the lines making the blueprint and then extruding them to the desired dimensions and also merging the results.
• Also giving approriate fillets and chamfers to the part modeled.
• Used a 3D sketch to link between the propellor shafts and then Boss Extruding that 3D sketches and extruding every single part of it and after extruding,mirroring it to its own face to get the desired shape of the anchor.
• Learnt about the combine option, which is used to combine the newly generated body to each other. There are few operation types such as add, subtract and common.
• For creating a Garage door and garage space, we have to select midplane and create a rectangle through lines and then cut extruding it, after that converting the sketch and again extrude cut it.
• Then using split feature to split the body from the existing body and thereby saving it as garage door.
• Again giving apperance to the body, face of different parts of the hull model, i.e windows flood light, Anchor railing, port holes and anchor hole edges etc.
• After apperance is done we have to mirror the hull through the midplane by selecting merging solid,knit surfaces, etc.
• At last by the help of PV 360 adding decals to the deck surface by the option to add decals , and under the mapping tab, selecting the mapping properties such as projection, and selection of face, the distance for X , Y plane, to fit the height, width and aspect ratio. We can also provide angles to the decals.In this case, we will select the appropriate decals, and selection will be done as projection and making sure that we fix width to selection, fix height to selection and fix aspect ratio and manually changing the width to 5500mm.
• Again adding same decal for the garage space with the same mapping specifications just by unchecking the fix width to selection and aspect ratio.
• Adding some decals to the other desired faces with the above same procedure.
• For stair step we have to follow the same procedure by just selecting a different decal.

Garage Door

• Open the garage door part which was saved then create a line coincident with the top and bottom edge of the garage door part and apply extrude cut option.
• Secondly create a shell to the left part with certain dimensions i.e 100mm.
• After this adding fillets to the garage door, giving it a smooth design.
• Adding a text over the centreline drawn on the front face of the garage door. By Selecting appropriate font and style also some mesurement.
• Projecting the text to the face of the garage door by extrude cut tool and selecting the feature i.e offset from surface again selecting the appropriate face and making sure reverse offset is checked on and then executing the operation.
• At last changing the colour of the whole body and desired face i.e. to the text.

Front seat

• Step 1 is to open the blueprints and then we have to go to insert part and insert the hull part which we have made earlier.
• Just making sure that we uncheck all the transfer option except surface bodies and then click ok, and now we can continue with our front seat design.
• Select the deck surface body and create a new sketch and draw a spline matching the curve of the blueprint, also match it by dragging the spline handles to get the exact design and then fully define it by giving dimensions and relations.
• Through that spline we will create a new plane which will be matching the curve of the blueprint. And we will give dimensions to that spline, and do surface sweep or swept surface to that spline which will give us a solid surface body.
• Again draw two lines connecting it with the surface sweep that we have drawn earlier and when the two lines are done dimensioning we will surface extrude or after extruding it we will trim the excessive surface, we will fill the top surface of the sketch or surface bodies we created with the help of surface fill option.
• Then again the same trim the desired amount of the surface from the top and side of the sketch the next the desired design for front seat. When this operation is over,we will use surface loft option to cover the hollow surface and then again trim the excess amount of surface by trim tool.
• When we form a solid surface body without any edges out then we will knit the surface altogether and form a single body.
• Then we will apply the chamfer accordingly to the surface body the we will sketch some lines and convert the outer edge of the front seat and trim the unwanted Line and with combining and converted entity we will form a closed contour and then create a revolve with reference to centreline.
• Drawing few more lines and also offsetting the inner edges of the front seat and then revolving it with a certain line which will act as a seat later. And again extrude cutting the excessive part of the revolve which is no longer needed.
• Now applying chamfer and fillets to give its corners smooth design and good look.
• After the fillet and chamfer we will mirror the centre body of the front seat and making sure we merge knit and propagate the visual properties.
• After mirroring the centre body, we will mirror the side body of the front seat but this time making sure we uncheck the merge solids and knit surfaces option.
• The only thing left is to mirror the matrasses the front seat. So,we will work accordingly . Again not merging or knitting.
• After this we will create a dome for each of the seat and also adding fillets for each of the edge with certain dimensions.
• At last or final work will be to go ahead and give appropriate appearance needed. By selecting the face or body.

Middle Seat

• Firstly, open the blueprints and then go to insert part option and insert hull making sure that all the transfer options are unchecked except surface bodies.
• Starting draw some liner matching the blueprints to preview and give it dimensional so that it will be fully defined and then extruding it till certain distance.
• We will select the same sketch again and offset its top face outwards, after doing offset we will trim the outer edge of offsetted entity and thus create a closed contour and then again boss extruding it.
• Creating two lines which will separate the two surfaces present and the exrtuding it till certain distance.
• Creating chamfer and fillets to get the desired shape for the middle seat, the fillets size will be different for edges and seats.
• After the chamfer and fillets are done we will mirror the two main bodies of the middle seat with reference to its right face, making sure that we mere solids and knit the surfaces.
• Next is to mirror the remaining bodies of the middle seat with reference to midplane and adding some more fillets to the edges.
• Now create a new sketch on the top view, start creating lines and giving them certain dimensions and relations which will make it fully defined and then extrude it till certain distance. On that same face create a new sketch and offset its entities with certain distance ,i.e 550mm.
• Do the same as done above, select the same face, offset it till certain distance and then Boss extrude it merging the results.
• Again apply the same procedure, i.e offsetting the entities of the same face, but this time do multiple offsetting for the table by applying different different dimensions values and also cut extruding it till certain dimensions. In this case it is 0.5mm. The second last step is to again give fillets to the table for its smooth design to the top of the table and to the base of the table.
• And now the very last step is to give it appearance according to our will,just by selecting each face of the table or by selecting the whole body and giving desired appearance.

Rear Seat

• Again starting from the same procedure first of all open the blueprints then insert part hull and uncheck all the transfer option except surface bodies and click ok.
• For rear seat select the mid plane and go normal to and start sketching one line and two spline matching the blueprints and provide dimensions and relations. Then draw these two splines to match the blueprints of the rear seat. Exit that sketch and create a new plane with reference to that sketch.
• Draw another spline and make sure to connect its one end to the previous spline we created. i.e. coincident relations. Then drag those spline handles to match the curve of the blueprints with providing certain dimensions.
• The next step is to create surface sweep providing profiles and path which will create a solid sweep surface.
• Offset the outer surface of the surface body and draw a new sketch on the previous plane and on that plane draw a vertical line with certain dimensions and click on surface trim option and trim the left surface of the rear seat and also trim one of the inner surface of the ruled surface.
• After trimming the surface create a ruled surface on the outer edge of the rear seat and then knit those surface together so that they will form one making sure we are merging the entities and checking on gap control with defined tolerance.
• We have to extend few surface after trimming operation so for that we will select a particular edge of the surface and perform the action till certain distance.In this point of view we will perform different actions like surface sweep extend surface.
• The next action will be to trim the extended surfaces in X and Y plane and making sure remove selections is on. And then knitting the left surfaces together and the again trimming one of the extended surface from the body.
• Continue this actions one more time.Then once again, knit the surfaces of the rear seat all the extruded surfaces and untrimmed surfaces.
• Create a 3d sketch to apply a surface loft between the two edges making sure that the profiles are on the same side, i.e both of the green balls and for guided curve select one of the other edge, then click ok, and the surface loft will be applied. Again along with the surface loft created knit all the surfaces altogether by checking on merge entities and gap control.
• Convert the bottom entity of the rear seat and execute surface extrude command with the selection as upto surfaces and selecting the corresponding surface.
• Again draw a 3D sketch and convert the entity of side face of the rear seat and then execute the surface loft option to create a solid surface across the side face. The knit all the surface together with merge entities and gap control on.
• Hide the deck surface and execute the same procedure as done twice earlier. Once surface loft operation is done, then apply surface extrude command at the end edges of the rear seat for avoiding any gaps so extrude the surface bodies and then surface trim the useless amount of surface to create a closed contour.
• Then again knit all the surfaces together and if all the edges turn black in colour that means that we have knitted all the surfaces together properly.
• This time unhide the deck surface and select the bottom edge of the rear seat and convert the entity and again draw one line and spline with certain dimensions and then boss extrude it till certain distance.
• Create a new sketch on the front plane and sketch one rectangle at the lower face of the rear seat and fully define it with appropriate dimensions now, offset the same rectangle inwards 5mm by clicking reverse option. After offsetting apply extrude cut to the sketch drawn with the option offset from surface and select the appropriate face and making sure that reverse offset is checked on.
• Draw some more sketches for cup holders on the seat and extrude cut the same. After this operation add few fillets of certain dimensions and click ok.
• Draw same sketches on the lower cabin door of rear seat and boss extrude them after fully defining them which will act as a handle and hindges.
• For creating pillow or back rest convert the seat line and extrude it to the certain distance after its done, to give it a shape execute a chamfer with the distance to distance with providing certain D1 and D2. Also giving fillets for smooth design and texture.
• For designing railing select the particular plane and draw lines with absolute dimensions, then add sketch fillets to both of the corners of the sketch. Then create a new plane on the end tip of the line and create a circle of certain dimensions and create a solid sweep.
• Draw a circle between the sketch that we had drawn previously and then create a centreline coincident with the centre of the circle and to the edges of both of the lines and then trimming half of the circle then again create a new plane at the end tip of semi circle line and draw a small circle and create a solid sweep along the semi circle.
• The very next step is to mirror the railing that we have created making sure we merge solids and knitting surfaces and propagate viual properties.
• Mirror the rear seat with reference to the mid plane and again making sure to merge the solids, knitting surfaces and propagate visual properties.
• After mirroring the rear seat mirror the pillow with again reference to the midplane band this uncheck merge solids, knit surfaces.
• Now, mirror the railing with reference to the midplane to the other part of the rear seat and again uncheck the merge solids and knit surfaces.
• For creating the flag, add 3D sketches of spline without any midpoints and also matching it with the curves of the blueprint and making all those splines a closed contour. Then exit the sketch and applied surface loft on the 3D splines created by providing two profiles and two guided curves.
• At last providing desired appearance to the rear seat body and faces. Thus,completing the rear seat part.

Superstructure

• First open the blueprints and the insert part i.e hull and making sure that all the transfer options except surface bodies.
• create a new sketch on the deck surface and create lines and splines and also giving them certain dimensions and relations and also making sure its matching with the blueprints.when this is done, we have surface extrude the sketch till certain distance.
• Create a single line at the end tip of the extruded surface perpendicularly and surface sweep that line.
• On the swept surface create another ruled surface with the option to tapered vector and selecting particular distance and face and ofcourse selecting the edges to be ruled.
• Draw some more splines to match the blueprint and add relations to them such as tangent relation etc and fully define it by adding dimensions. Do this action one more time on the sketch and the create a projected curve with the help of two splines which has been created.
• Again offset the outer edge of the curves and also add some lines and splines to match the exact curve of the blueprint and again fully define it by adding relations and dimensions and atlast create a projected curves using those curves.
• Then create a surface loft by providing two of the 3d profiles and two of the 3D guided curves and click ok.
• Then execute surfaces fill command by providing all the 3D surfaces or sketches to be filled and making sure that the transition of the edge to curvature.
• The next step is to trim the over extended surface by drawing a single line which will be used as a trim tool for removing the extra amount of surface.
• Then making sure to knit the surfaces properly with the solution of gap control. Again creating a new plane, and on that new plane, and on that new plane have to create spline which will be used for sweeping out the surface, i.e swept surface.
• As explained in the pdf we again have to create few more splines to be used as the edge of the superstructure as well as for the trim tool and drag the spline handles as to match the curve of the blueprints and for defining them we will go ahead and fix it. Later we will create a projected curve using two of the sketches or spline drawn and then click ok.
• We will repeat this step and create two more projected curves for the sake of window of superstructure and for creating a solid surface body we will use surface loft command to get the desired shape between those two of the projected curves.
• Again for the roof of the superstructure, we will create two more projected curves and will use surface loft command for the same, which will give solid surface body.
• Again for wind screen or wind shield we have to create a spline matching the curve of the blueprint and executing the command surface loft and selecting the profiles and the guided curves and then click ok.
• Now for the side windows select the outer edge of the superstructure and execute the command for ruled surface by the type of tapered to vector and by certain distance.
• Now trim the upper surface of the ruled surface which has to be removed and also make sure to keep the surface split option as linear. After trim operate knit the newly genrated surfaces with each other.
• Now there are command used such as surface extend, surface extrude,surface loft, trim surfaces or surface trim, and knit surface to make the other surface bodies and making it with the blueprint.
• Again adding some more splines and surface extruding it will form solid surface body and the partition can be used as a trim tool. After trimming operation make sure to knit the surface along with gap control and merging results.
• Trimming and keeping selections of body will continue to remove the unneeded surface bodies from the sketch and after doing so, we will keep knitting the surfaces and adding fillets for the good design of the superstructure.
• Draw a circle at the deck and extrude it till certain distance. Then again select the top face of the circle and draw another circle on it. This time use the command extrude cut to create a hollow at the centre with the given distance. Now again select the same face and draw two circles and boss extrude it till provided distance with merging the results. After this operation apply fillets to the drawn sketch for good and standard design.
• Draw a rectangle from the centre of the circle and use the command extrude cut to cut the body in half so that it wont be a problem when mirrored. And as it will a closed and solid body, we will select the inner face of the cut section of the cylinder and delete that face.
• Then we will draw lines according to the dimensions provided and will surface extrude those lines till the next surface and thus our front stairs will be done.
• When there operations will be done we will go ahead and knit the surface altogether and also we will go ahead and trim the front and rear part of deck surface with is not coincident with the superstructure and then knit the deck surface and the superstructure.
• Now create a horizontal line parallel and coincident with the centreline of the superstructure (while viewing through top plane). Create a surface extrude of the horizontal line with certain distance and then trim the excess or extra amount of surface body which is not needed. After this knit the surface body which is not needed. After this knit the surfaces altogether to form a single body.
• Learnt about the thick surface command, it is very helpful especially when we need to thicken as surface with certain thickness amount and distance. After thicken the surface we can again start sketching on that same face. So, draw one or offset the edges which was offsetted earlier and join them with lines making them closed contour and extrude cut it throughout the surface.
• Draw another rectangle on the same face with certain dimensions and relations and then cut extrude it with the option up to body and select that body till which it will extrude cut it.
• Now create a dome to the front thicken faces of certain thickness i.e 30mm in this case and say ok. Apply the same to the other two faces of the surfaces then add fillets for smooth look and design.
• For creating the railing draw a circle whose dia is more than that of the outer circle and trim it to desired angle, in this case its 55degree and then at the end tip of that circle add a 3 point arc and give tangent relation to the line connecting with the arc.
• Sketch a circle and select its midpoint and ctrl select the midpoint of the curve we created and give coincident relation. Then apply a solid sweep operation by taking the small circle as the profile and the curve as the path.
• Do this same procedure for the outer railing of the superstructure and also for the cabin near the rear seat of the superstructure.
• convert the entities of the wind screen and draw vertical lines as well with particular distance and create a boss base extrude which will act as a partition between the wind screen wipers and also add same fillets for smooth design and texture.
• Draw same rectangle to back of the superstructure as we did for the wind screen for the partition draw two rectangle at the back and boss extrude it and then add few fillets to those extruded parts.
• offset the entities of the outer edges of the windows of certain distance and trim the extra amount of lines present to make it as a closed contour then extrude cut the same with the option offset from surface and selecting the particular face. After its done provide a fillet to its outer for a smooth texture.
• Apply the same procedure for the other side window and provide edge fillets for smooth texture.
• At the rear end offset its entities to form a closed contour (All four of them by selecting the face) and use the split line command as projection and select the corresponding face on which it should be projected on say ok.
• Now sketch rectangles on the side windows as we did earlier for window screen and provide certain dimensions and boss extrude it with the option offset from surface and select the corresponding face. After its done apply same fillets.
• Mirror the main body of the superstructure with the reference to midplane and making sure to merge solids, knit surfaces and propagate visual properties. Also mirror the two sun deck mattresses but this time not merging the solids nor knitting the surfaces.
• Next mirror the jawzzi waterline accross the midplane and for the merging and knitting the surfaces.
• Draw rectangle parallel to the partition line with certain dimensions provided and boss extrude them accordingly with the option offset from surface and select the face and offset distance. Apply this procedure of adding blades two times on the other two wind screens and extrude them.
• Create a chamfer to give the blade its looks with the distance option and providing D1 and D2. Then offset the face of the blades inward and extrude cut it. Do the same for other wiper blades and add fillets as well.
• Now create a 3D sketch line from the rotor to the wiper blade. Then create a new plane at the end tip of the 3d sketch and create a circle of certain dia on that new plane and execute boss extrude command till certain distance with mergine the results. Apply the same procedure for the other wind screen wipers and extrude the 3D sketch.
• At last giving appearance to the body and the faces of the main superstructure for window it should be black adding decals to the stairs step as we have done earlier on hull part.

Radar Mast

• Open blueprint and then go to insert part and open superstructure and for the transfer option make sure except surface bodies everything else should be unchecked.
• Select the midplane and sketch horizontal line matching the blueprint and fully define it with certain dimensions. After doing so create a new plane from the sketch we created and on that plane create a new sketch. Start sketching splines and provide dimensions and also drag the spline handles to match the curves of the blueprint and simply extrude it till certain distance and add fillets to the same.
• Now create a new plane with reference to the front plane and with certain distance and start sketching lines and centreline to match the exact design of the blueprint (also give dimensions to fully define it). After completed with the lines add a 3 point Arc from the end point of our sketch till the centre line of our sketch.
• Now create a revolve with reference to the centreline i.e 360 degree with merge results checked on after the operation is done add fillets to the sketch created.
• Draw the cable by drawing the circle on the top face of the Radar mast and boss extrude it, then again select the top face of the extruded body and sketch a new circle of lower dia and again extrude it.
• Do this process one more time for again lower dia and increase distance, then add fillets for its smooth design.
• Now create a railing by sketching first a vertical line and the coincide with spline and for the lower handle of spline give vertical relation and for the top handle of spline give horizontal relation. Then create a new plane at the tip of the spline and create a circle on that plane and solid sweep it by providing profiles and path. At last mirror the sweep with reference to other plane.
• Now sketch three circles on the face of mast which are tangent with the outer edge of the railing and also provide certain distance and dimensions to fully define it. Then boss extrude same with the midplane option and providing to distance till which it should be extruded.
• Create clamps at the mast by adding line sketches rectangular in shape, and it should be 2 shape 3D that it can handle and it can support the mast lights which has to be placed on the surface. So, first sketch and then boss extrude it till certain distance.After this operation apply fillets to the extruded body.
• Now create mast lights on the surface of the clamp body first draw line sketches matching the blueprint and then exclute remove command selecting the centre line or mid line as the revolve reference and revolve it for180 degree . Again apply the fillets for smooth curvature.
• Mirror the mast lights accross the primary face i.e right side or left side according to the selection.
• Now create a blow horn by selecting a new plane and with the help of sketch lines and splines create the sketch for a horn and fully define it by adding relations and dimensions. then again create a revolve by making the centreline or the axis of revolution and revolving it 360degree with merging results. Also create a dome on the back face of the blow horn for certain dome distance.
• Add fillets for the blow horn for smooth design and create a shell on the front face of the blow horn which will give premium look as same as blowhorn.
• Now mirror the radar mast with reference to the midplane and making sure to merge the results and knit surfaces and also propagate visual properties. Now create slot on the surface of the blow horn and extrude it with the option upto surface and selecting the appropriate face.
• Now mirror the blow horn accross the new plane, by selecting the features to mirror.
• Now change the appearance of the whole radar body mast, the mast lights and other more features.

Yatch Assembly

• Open solid works and select new,then assembly.Then click on option insert components, click on browse and open hull and simply click ok, it will automatically get fixed on the screen.
• Second, insert superstructure and again just click ok, and it will get fixed automatically.
• Now, import the radar mast and click ok it will automatically get fixed on its right place.
• Do the same for the front seat and the middle seat it will automatically get fixed to its right position.
• Import the rear seat and click anywhere on the screen to just place it on the screen, then for defining its position manually select the bottom face of the rear seat and select the, surface of the hull and give coincident relation. Created one more mate relation between the midplane of the hull and midplane of the rear seat. Now give another coincident mate between the bottom centrepoint of the rear seat and centre point of the deck surface and also giving certain distance value.
• Import garage door and click anywhere on the screen to place it on the screen and then give coincident mate between the midplane of the hull and the right plane of the garage door, this moment distance should be zero.
• Create a concentric mate between the hindge tube and hindge hole of the garage door.
• Now import the propellor and click anywhere on the screen. Then create a concentric mate between propellor shaft face and propellor hole and click ok. Again create a coincident mate the other two propellors the same way.
• Import the radar and click anywhere on the working screen and create a concentric mate between the radar mast axis and the blue hole of the radar and change the distance to zero(0). This is the final step of the yacht model and our model is complete.