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An attempt at hull modeling with Fusion 360 Loft + Rails

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I have been slowly learning Fusion 360 with a goal of accurately modeling a hull as a 3D object based on lines plans.  I haven't been completely successful, which is why I titled this "an attempt".  I am posting with the hope that individuals with more Fusion 360 than me can tell me if I'm headed in the right direction with my approach, and if so, how to proceed from here.  Thanks in advance for having a look.


For this exercise, I have used the plans of the schooner Ernestina, which can be freely downloaded from the Historic American Engineering Record at the following link: http://www.loc.gov/pictures/item/ma1719.sheet.00018a/


I chose to use the Ernestina plans because they are very clean and accurate, requiring little extra work to make them usable.  I cropped each of the views and saved each to a separate file.  Then each plan was brought into Fusion 360 as a canvas, as shown below.  To ensure correct scale, I calculated how large each image should be in the 3D environment, I created rectangles of the correct dimensions, then placed the canvases onto those rectangles.  That put the images into the 3D world at the correct size.  The canvases were positioned so that the world origin point was at intersection of the baseline, center line, and forward perpendicular.



Next I created offset planes for each waterline (4 total) and each station line (15 total).  It is a mystery to me why Fusion 360 displays larger and larger planes the further each offset plane is from the origin.



I created fit point splines for each waterline, drawing each on the appropriate waterline offset plane.


I learned early on that if I want to use the Loft operation with Rails, it is a requirement that every profile being lofted must intersect with every rail.  To make sure this would happen, I would select an offset plane and use Sketch -> Project / Include -> Intersect to create a set of points where the offset plane intersects with the waterlines.  This was repeated for each station offset plane.  The intersection points are visible as the purple circles in the image below.  Note that one forward station and the four aft-most stations do not intersect all 4 waterlines.


Then I drew a fit point spline for each station, making sure to touch each intersection point along the way.


Finally it's time to loft.  I switched from Model mode to Patch mode, then went to Create -> Loft.  The image below shows the result of lofting all 15 sections without using rails, then creating a mirrored body for the other side of the hull.  For this particular hull, the shape is pretty good, but I know that for other hulls the incorporation of the waterlines and/or buttock lines and/or diagonal lines is required to achieve an accurate hull shape.


So in order to incorporate the waterlines, I need to loft with rails.  I can only use the stations which completely intersect with every waterline, so some must be skipped.  The result of lofting with rails is below.


And that's as far as I can get.


My questions:

Am I following a good approach, or are there features of Fusion 360 that I have overlooked that would make this easier?

How do incorporate the station lines that couldn't be used in the loft + rails?

How do I close up the shape at the bow?

How do I force curved edges of a body like the one below into straight lines that can bend at sharp angles?


Thanks again for any insight.


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Am I following a good approach, or are there features of Fusion 360 that I have overlooked that would make this easier?

I believe your approach is sound and you are not missing some "secret."  Programs dedicated to ship hull design handle things pretty well it seems (I have not used one to date), but hulls are fairly challenging for programs like Fusion 360.  On the TurboCAD forum a ship's hull is something like the Holy Grail of lofting.


How do incorporate the station lines that couldn't be used in the loft + rails?  

It helps when all the stations have the same number of nodes.  I sometimes add a node to account for a missing water line.  The key is not so much that the added node is on the same plane as the water line as it is that the computer can loft "node to node" (I just made that phrase up).


How do I close up the shape at the bow?

Think of the rabbet on the stem as a kind of station line, draw it and loft to it.  This will get you in the ball park but is not the total answer.  Come to think of it, I'm not sure anyone really knows the total answer.  At the gripe a lofting will do some funny things.  Of course, added stations at the bow will facilitate things quite a bit.


How do I force curved edges of a body like the one below into straight lines that can bend at sharp angles?

Your picture illustrates the basic problem of lofting a hull.  You can think of the lofting process as akin to the computer connecting your stations with splines (with the fit points falling on the stations).  Now, in your illustration the lowest spline (so to speak) takes a downward drift in order to set up for the hard upward turn.  Doesn't it look like a driver who swings wide left to then turn right?  The closer the stations are to one another the less the swing which is why adding stations can help.  The same thing happens at the bow in the area of the gripe.  At the rail the problem is evident again, but is more easily fixed by using the rail line to create a loft which is then subtracted from the hull.


Now for the necessary disclaimer.  I am not trained in CAD nor do I work in the field.  The above is the result of my own experience.  I remain open to a more perfect way and bow to the expertise of others.



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Wayne, that makes a lot of sense. I look forward to seeing how it works for Peter's hull. I am learning while watching!


There is a Fusion tutorial online that shows how they constructed a curvy plastic housing for a reciprocal saw. It shows how they try to line up the contour lines to be even all around the form, as you suggest, and they are able to add in additional points as needed to do so at tight curves.



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Hi Peter,


I don't understand how you managed to get the curve in three dimensions in Fusion. Looking at my drawing below, imagine measuring up along a station line in the X-Z plane, then measure out in the Y plane to locate a point on the thick black curve. I have not seen how to switch from drawing in the X-Z plane to drawing on an X-Y plane at right angles, and selecting where the first point on the X-Z plane is located. How did you do this? I could not see how you used the "project/include" tool to find the intersection.


Best wishes,



Fusion question_20181219_0001.jpg

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Mark, thanks for mentioning that video.  Here is a link to it if anyone else is interested.  It made it clear that I was going in the wrong direction by using Patch to create the hull surface.  I should be using Sculpt / T-Spline, which is much more powerful.  I am now learning what I can about it.


I'm not clear what you're asking regarding projection / intersection.  In what I have done so far, all of my curves have been drawn in planes which are parallel to the primary XY, XZ, YZ planes.  In your drawing it looks like you have a curve in the XZ plane and a target plane that is at an angle to the XZ plane and you want to project that curve onto the target plane.  That's not something that I have done.


What I did was create waterline curves in the waterline planes, then I found the points where each station plane intersects each waterline curve.  After that, drawing in a station plane, I drew the curve for a station, making sure the curve would pass through the intersection points.  I can post a more detailed explanation with pictures if that would be of value.


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Hi Peter,


I look forward to learning what you find out about using Sculpt and T-Splines. A whole new world to me.


I apologize for not being clearer in my drawing. Let's assume the thick black line in my drawing is the top, outermost edge of the hull in 3 dimensions. The traditional way of locating that would be to go to each station line, and measure up in the Z direction on the X-Z plane the height of the line at that point above the base, top of keel usually. Then you would measure out from that point in the Y direction to find its distance away from the center line. I was hoping to do this at each station point and then link the points together with a spline to form the curve in three directions. I was then assuming I could use a series of lines like this to form the surfaces.


This is how my ship was originally drafted, and so I assume this would be the right approach to using Fusion.


The problem is that I cannot get Fusion to find the point I just drew on the X-Z plane when I turn to drawing on the X-Y plane. Nothing will click on it. I am wondering if I need to do this with solid bodies rather than just lines in space, so I can find them...



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  • 2 weeks later...
  • 3 weeks later...

Mark, I may have achieved what you want in Fusion 360.


On the Ernestina plans, there is a line identified as the "measured sheer line".  Unlike other plan lines, this line is curved in every view.


To start, I used the intersection of three offset planes to locate the point at the bow where the line starts.  I then started a fit point spline sketch in a plane parallel to the side view and created the curve shown below.  Let's call this curve A.


Next, working on a plane parallel to the top view, I created a second curve following the sheer line as viewed from above.  Let's call this curve B.  From this view, curve A looks like a straight line.  Both curves share a starting point at the bow.


Here are the same two curves viewed from the side.  In this view, curve A is curved and curve B appears straight.


Now it's time to combine them into a single curve.  I go to Sketch -> Project / Include -> Intersection Curve.  First I select a plane for the sketch.  As far as I can tell, it doesn't matter which plane I use, but I used the offset plane where curve B lies.  Next, the tool pops up asking me to select the curves.  I select curves A and B and hit Ok.


Here is the new sketch curve, displayed in purple, from the side.


And from the top.


As you can see, it curves in several directions.  Here it is along with sketches for the rabbet line and water lines.  Unfortunately, Fusion 360 does not allow me to use it as a profile in a loft.  However, I may be able to use it as a rail if I am lofting using the section curves.  I plan to try that next.


Edited by SardonicMeow
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I have done a couple "hulls" using F360. One thing I figured out was to center the canvas origin on the 00 bulkhead location where the waterline meets.

This way I found it easier to work forth and aft in right sequence, naming each plane accordingly to the bulkhead.

However, the only issue I have had is to line up the imported sketch to 0/90 angle towards the planes.

Looking good though.
I am to work the F360 tonight after work.

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Here we go with try number two.  It's a big update today.


First of all, in an earlier response, I described a method for creating a curve which bends in 3 dimensions using the intersection curve feature.  However, I found that Fusion 360 limits what can be done with this sort of "derived" feature.  I could not use it as a profile in a loft, and when I tried to perform further intersection operations using the curve, it would sometimes work and sometimes fail.


EDIT: If a "derived" feature, which displays in purple, can't be used for some operation, there is a way to change it into a regular feature.  Edit the sketch, then right click on the feature and choose "Break Link".  The feature will turn blue.


The good news is that there is a better way!  Here is the secret.  First, go to the Preferences and under General -> Design, look for "Allow 3D sketching of lines and splines".  Make sure it is checked.


Now start a new sketch.  I am going to draw the sheer line again.  I start the sketch in an offset plane parallel to the ground plane.  I use a fit point spline and create the curve as viewed from above.


In the sketch options dialog, make sure "3D Sketch" is checked.  With 3D sketches enabled in the preferences and the 3D sketch option turned on for the sketch itself, the curve can now be manipulated in 3D.


I switch to a side view.  I right click on a control point, choose Move/Copy, and adjust the point up or down as needed.  I am careful not to move the point in any direction other than up and down, because that will change the flow of the curve as viewed from above.


Once the control points are moved, the handles of each need to be adjusted so that the shape of the curve is correct in the side view.  And that's it.


Now to keep going.  I found that lofting using water lines as profiles for the loft, and station lines as rails, works best.  In my original post I used Patch, which creates a body that cannot be modified further.  This time I'll be using the Sculpt environment.


During some failed attempts, I found that I was confused by those parts of the water lines which overlap on the halfbreadth plan, resulting in curves that were too far in or out.  To fix this, I will use the intersections of the station lines with the water lines to find exactly where they go.


As I have mentioned before, when lofting in Fusion 360, every rail must touch every profile.  To ensure this, my procedure will be as follows:
1. Draw the sheer line (already done, see above) and a line at the top of the keel.  These will be the first and last profiles in the loft.
2. Find the intersection points of each station plane with the sheer and keel lines.  These will be the start and end points for each station curve.  I will only draw the stations which intersect with all the water lines, so some stations far forward and far aft will be skipped.
3. Find the intersection points of each water line with each station curve.  Draw the water line curves by passing through each intersection point.
4. Loft the body surface going from keel to water lines to sheer, using the station curves as rails.


For the keel / rabbet sketch, I have created an offset plane which comes out from the center line by 1/2 the thickness of the keel.  I start a sketch on this plane.  This sketch consists of several curves and lines which trace the line from stem to keel to sternpost to transom.  However, while there are several components to this sketch, only the line along the top of the keel will be used in the loft.


I will be drawing stations 3 through 11, because these are the ones which intersect with every water line.  For each station, I select the appropriate offset plane, then go to Sketch -> Project / Include -> Intersect.  I select the sheer line and the keel line (purple dots appear at the intersection points), then Ok and Stop Sketch.  This is repeated for each station.


Once the intersection task is complete for each station, it's time to actually draw the station lines.  I select the offset plane for a station and start a fit point spline.  I draw the curve of the station, starting and ending the curve on the intersection points (they appear black with a purple outline here).


This process is repeated for each station.  Again, I chose to skip the forward-most and aft-most stations.


Here's what we have at this point.


Now I'll find the intersection points with the water lines.  I select a water line offset plane and then choose the Intersect operation.  I click to find an intersection point at each station, as well as points on the stem curve and in the stern.  This image shows the intersection points (purple circles) for all four water lines.


To draw each water line, it's simply a matter of starting a fit point spline in the correct water line offset plane, and connecting the dots.


Now that we have all the necessary lines, and are confident that there are intersection points where they are needed, it's time to loft.


To enter the Sculpt environment, I click on the purple cube.  Then under Create I choose Loft.  I click on the keel line, then each water line moving upwards, and then the sheer line.  Then I click to choose rails, and select each station line.  (There was noticeable slowness while selecting each rail.)  I guessed about the spacing settings (8 faces in each direction).


The form is... not too bad?  It's smooth in the front, but it a little wavy aft.


In the Sculpt environment, all the vertices, edges, and faces can be moved around to refine the shape.  I am just starting to learn how to work with a form in Sculpt.  But, as a simple example, you can see here how I moved one vertex to adjust the shape of the bow to match the line on the plans.


I exit out of Sculpt, and create a mirror of the surface.  It's starting to look like an actual ship.


Now let's do something with it.  By finding the intersection of the surface with any plane I choose, I can create my own lines plans with water lines / buttock lines / station lines wherever I choose.  Here I have created an offset plane near the bow.  The results of the intersection operation are new station lines at a location of my choosing.


Continuing to work on the same sketch, I add a notch and a curve for the cambered deck.  Now I can right-click on the sketch in the browser at the left and choose "Save as DXF".  And that file can be imported into laser cutter software.  Repeat for multiple bulkheads, and you're on your way to making a plank-on-bulkhead model.  (At least, that's what I hope to do eventually.)


Thanks for following along!  I hope that others who are using Fusion 360 will share their experiences.



Edited by SardonicMeow
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Thanks for the work that you are doing. As I am on the learning curve for any CAD (busy working through a manual on F360), this will greatly improve my knowledge and ability. Please keep up the excellent explanations and images of how to utilise F360.




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  • 3 weeks later...

I have been thinking about how the hull could be lofted in pieces rather than all at once.  Each section between stations would be lofted, using whatever rails are common to the two.  In the end, there would be an option to combine the pieces together.


Here are the first several sections.




And so on down the line.  You'll notice that I skipped one section, because it's problematic.




What to do here?  If I loft between the two stations, the back end of the keel isn't covered.




I realized I need to break this into two parts.  One loft at the top from the smaller station (#12) to the upper part of the larger station (#11).  Then a separate loft from the back end of the keel to the bottom part of station 11.


To do this, I needed to break the larger station into two parts, while also retaining an intact copy for lofts forward.


First, I highlighted the curve of station 11 and hit Control-C.  Then I started a new sketch in the same plane and hit Control-V to paste.  That was repeated to get three copies of the station line.  The original will remain untouched.  Copy 1 will be cut leaving only the upper part and copy 2 will be cut at the same spot, leaving only the lower part.


Let's work on copy 1 (upper) first.  I edit the sketch, and keep station 12 visible.




Next I sketch a line from the bottom point of station 12 running horizontally to cross over the curve of station 11.




Now I go to Sketch -> Trim.  When I hover over the bottom portion of the curve below the line, it's highlighted in red.  I click to remove the red portion of the curve.




Here is the final result.




Working on the second copy, the same procedure is repeated, but the top portion of the curve is trimmed.  Only the blue portion remains.




Now I can complete the lofting.  First, I loft from station 12 to the copy of station 11 containing the top of the curve.




And then the bottom part is lofted from the back end of the keel / sternpost line to the bottom of the station 11 curve.




The final result is a set of surfaces that is an improvement over my earlier attempts at sculpting the hull as a single surface.  You will notice there are some thin gaps between the surfaces in the aft area of the hull.  I think if I loft using a larger number of faces, the surfaces will fit better to the curves and reduce those gaps.  I did try using the edge merge tool in the Sculpt environment, but I ended up with distortions in the smoothness of the surface at the merge areas.



It's not as good as the results I got from importing a mesh built in Blender (see my Blender thread for details) but it's the best result so far.




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Peter, your writeups have been very inspiring.  Thanks for exposing the twists and turns you've encountered in exploring how Fusion 360 can meet your needs.  I've also been using that software to model hull shapes for another goal.  I own a classic sloop that needs modification of the cockpit area in order to shoehorn in a new powerplant.  The engine manufacturers provide 3d models of the entire drivetrain, so it sure would be nice to have a realistic model of the hull and interior framing.


I started with as-built line and offset drawings for my boat, a 1962 Cheoy Lee Lion designed by Arthur Robb, with a carvel planked teak hull.  The as-built blueprints are archived at Mystic Seaport Museum and are available for a small fee.  I used a similar procedure as you described in a previous post, but used the body plans as profiles at 12 stations and just one of the buttocks as the (single) rail.  I tried using the rabbet line and/or the rail top as rails, but got errors about crossing rails, etc.  I had to do something similar to your second method to splice in (merge) the drawing at the bow, but other than that the loft was automatic from stern to bow.  


However, a lot of detailed manual sculpting is required to make up for deficiencies in the automatic loft.  Although the detailed plans have 12 stations, 8 waterlines, 3 buttocks, plus the rabbet and top rail, the loft still had a wavy appearance no matter the settings on the t-spline grid spacing.


But, I guess some hours of detail work with a mouse is worth it.  The t-spline editing tools are very powerful, and eventually I have a hull model that does conform to the design.  Yesterday, I spot checked some measurements on the actual boat, and there are a few centimeters difference in places.  But good enough for now, and it's time to add some framing to the hull and then bring in the drivetrain model.




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This seems to be just like the world of CAD in architecture; you start out with what looks like it should be fairly automatic and rational, and end up with hours of tweaking to make it really right. My reality never quite matched the smooth and simple tutorials.


It is fascinating to see you all working out the kinks in these programs for shaping ship hulls.



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  • 4 months later...

Hi I tried following these instructions but I can't seem to move the handles of the control points after I move them up and down in the side view.


If I don’t move the control points up and down, I can move the handles, but only left or right. Am I missing a step?

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  • 3 months later...

I wish I had seen these helpful posts earlier. I am modelling a replica, 24 feet long, 19th century, fishing boat which was measured early in the 20th century. The construction was started by a technical college to teach students, but they lofted the frames from the measurements, so they didn't make a 3D model. (In full size boats, thin strips of wood are bent across the frames and trimmed to produce "fair curves".) It will help us to satisfy the passenger licence authorities if we have a an accurate model of the boat.


I put the measurements into a comma separated file of X, Y, Z  points and imported them using the import CSV file add-on. I imported the gunwale line by enabling 3D sketches. I had similar issues with bumps and exaggerated curves from my early lofts. I found that reducing the number of points produced better results, unlike SardonicMeow, who found more points better. I kept my imported points visible to check that my shapes were acceptable. A few points obviously weren't good, but I suspect they weren't well measured.


My next problems came when I thickened the surface. The program froze or reported errors. My work-around has been to split the the hull into 3 sections and loft and thicken the sections. I was surprised that the surfaces met very nicely. I wanted to thicken the surface again to produce the frames but the program keeps crashing again. I may try splitting the body into sections just the width of the frames and try again. It is certainly not like the tutorials, but I am learning a lot.37860303_1777378799036987_19944368177340

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  • 3 months later...


first thank you very much for your very informative tutorial, it tought me a lot.

One thought: In the case of that problematic sternpost region, would it be possible and helpful to add an auxiliary station at the aft end of the keel? It should be possible to shape it by reversing the process how you generated the waterlines and other lines.

Just saw the link to your blender article here (new subscriber here) and will  read it next.

My motivation is an almost 60 years lasting interest in ship modeling, a stack of old plans on one side and a CNC milling machine (MPCNC) and 3D printers etc. in the basement on the other.

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12 hours ago, Chattermark said:

In the case of that problematic sternpost region, would it be possible and helpful to add an auxiliary station at the aft end of the keel?

Interesting idea.  I think you mean a new station as shown below by the thicker blue line.


If I try a direct loft across all the stations, it doesn't work.  My keel is made of multiple lines, so it can't work as a rail, and not all waterlines pass through all stations, so they can't be used as rails.


However, I get some good results from three separate lofts.  Curiously, the direction of the normals is not consistent between each of the lofts, but the resulting surfaces are usable.


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  • 5 weeks later...
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  • 1 year later...

Great work, very interesting posts!


I'm interested in design, especially the America's Cup boats. I did a lot of analysis of the AC75 foiling monohull, and now I'm into the SailGP F50, which is a foiling catamaran derived from the AC50.


As no plans are available, I drafted up my own in Inkscape from heaps of images from videos, plus a few published dimensions. Unfortunately I can't find how to insert an image from my pc in this forum?


Anyway, I wanted to try CAD, so started with Fusion 360 a couple of weeks ago, and have finally managed to Loft one of the hulls.  I used a number of the techniques described above, but there were several I haven't learnt about yet - very interesting.


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Hi, Max.  If you have discovered any new techniques in Fusion 360, please share.


As for including pictures, start a reply, then click on the "choose files" link at the bottom where it says "Drag files here to attach, or choose files..."  Move your cursor into the position in your text where you want the image to appear, then click the plus sign on the image.  For more help, look in the "How to use the MSW forum" forum.


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This is excellent work! The solution I use in Solidworks is to reduce the frames by the offset amount of the planking that the builder is going to use. In the end, the surface is not useful if you are doing a design in order to create laser-cut frames so there is no need to make the thickening function properly in the first place. 



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  • 8 months later...


I'm following your steps to shape the hull of the cutter Le Cerf. 

The blueprint are sufficient to perform quite an accurate job. However, I'm quite new to fusion 360 ad something is maddening me: Whenever I try and tweak some of the sketches, the intersection points between rails and profiles are not coincident anymore. I guess It is some kind of issue with the constraints I set, but there seem to be a rather large number of issues of the sort as far as 3D sketches are involved.

For instance, If I tweak the sheer line aven a little bit, I lose all the relevant snap info for all stations...

Do you have any kind of advice about this matter? 

Cheers !

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