Designing hull. Lots of issues, even contractors gave up.

[l.cariouVF6EP]

Hello guys,

I hope you will be able to help, I am struggling since months to design an oil and gas vessel hull.

I am working for a friend on a project to design and 3D print a mould in order to use resin and fiber glass to do a model.

My friend even paid some contractors on Malt and Fieverr but all of them were unable to deliver a proper file usable and editable. I am able to get a nice form myself but it's buggy and I cannot use shell fonction or combine to get a mould shape.

I need to design the master first (the hull) so I can either directly 3D print it or get the mould shape and 3D print it.

I tried with solid, surface and form but end up with the same issue. The 2 files attached are the same design but with 2 different loft approaches:

1. Using only 2 profiles with 4 rails and sketches used as template for rails position.
2. Using mainly profiles and multiple lofts: I get a form but top and side are not flat and shelf function is not working.

2profiles+railsonly profiles

Option 1 results in a non valid form: 

non valid form

Option 2 seems better but the top and side are 1 flat surface + the last loft create a curve on top edge when it should straight.

option2non flat surface

The 2 f3d files are attached, I really hope you will be able to support.

Thanks

BR

Laurent

[wersy]

Hi Laurent,

The order is not correct.
First draw the longitudinal lines. Then the frames are created via intersection.

Michael

[l.cariouVF6EP]

Hi Wersy,

Thanks for your feedback. The issue I see is that I can design the longitudinal (rails) once I have the frames (profiles) in place. Profiles are designed using the canvas, without this I don't know the shape of the rails.

LC

[wersy]

The shape of the rails of the longitudinal sections can be seen in the side view. The position of these rails can be seen in the top view.
The shape of the vertical sections is shown in the plan view. The position of these rails can be seen in the side view.
However, as the pictures are blurred and usually not precise, this is difficult.

[l.cariouVF6EP]

Hi,

I just spend some time on it and I don't see how to do it. In fact i don't understand why designing the profiles or the rails first could have an impact.

I tried to rework the big profile and by simplifying it and making it with the same qty of spline line points it works better. The top surface is now a plane, unfortunately the side face is not a plane. I don't understand because the side on the 2 profiles are straight lines and the rails on this side are both 2D.

not plane

I tried by mirroring the profiles before doing the loft but then I cannot shell the form. So frustrating. 

[TrippyLighting]

This is a complex shape and a single loft is unlikely to give you the result you are looking for.

Depending on what the overall goal is, this is not a beginner project. If you just want to model for 3D printing Fusion 360 is a fine tool,. If you are after a very accurate  reconstruction, Fusiosn 360 might not be the right tool It simply does not have the surfacing tools needed.  

It is not the case that more data e.g. more spline points, more profiles/rails give a more accurate shape. The opposite is the case when working with NURBS surfaces. 

Lets start with the splines. This spline is not  bad, but it can easily be better. That wiggle in the curvature can be removed by deleting one spline point and working with the remaining tangent handles. In fact a 3 degree control point spline with 4 control points will do better. 

[wersy]

As @TrippyLighting already pointed out, the most accurate replica of a hull is hardly possible with Fusion. This is especially true for a round hull when using frames.
One possibility is to use longitudinal lines, but if you compare these with the ribs, you will find that they are not exact either - as usual.
As an example, I show the principle of how frames are created from rails.

You don't have to use all the rails and you need fewer profiles.
But to approximate the longitudinal lines to the frames until a smooth shape is created would be a tedious and long job with several iterations.

You will probably have no choice but to work with the frames and do the best you can.

[l.cariouVF6EP]

Thank you guys for your feedback. You pointed out something I was starting to fear, F360 is probably not the best for this job.

Even with approximation my issue is that after the loft is done (without warning) the solid cannot be shelled or combine function used to have the contounter form.

I will simplifying more the spline but not sure it will solve my problem.

I was reluctant to learn a new software but maybe I have no choice.

[TrippyLighting]

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@l.cariouVF6EP wrote:

... I was starting to fear, F360 is probably not the best for this job....

I was reluctant to learn a new software but maybe I have no choice.

---

Learning is the key here!

But that also very much applies to your understanding of the type of geometry you are working with.

As such I would suggest you continue with Fusion 360 until you actually have a firm understanding what the limits of the software are and why!

Currently, you don't have the knowledge to even assess what might be a better software. let alone to work with it.

I would start by reading through the Autodesk Alias Theory Builders.

I can elaborate more on why you might run into limits with surfacing in Fusion 360. But those can be alleviated to a degree with T-Splines. There are currently only two Autodesk Expert Elites active on this forum who have the experience to attempt this with T-Splines.

[TheCADWhisperer]

@l.cariouVF6EP 

I would not include 4 (and possibly a 5th) planar faces in Loft geometry.

First attempt I would do in Surface environment as patches that are then stitched together.

Edit: Yep, looks like the Design Intent is for this 5th face to be planar as well.

Edit 2: Where are your dimensions and logical geometry constraints?

How would this geometry be held to 9 decimal places in the real world?

[wersy]

I thought I would give it a try to align the longitudinal rails and frames with each other.
It doesn't get much better if you leave out some profiles.

This is guaranteed to be the last time I engage with something like this 🙂
It's even quite a lot of work to do this for an chine hull, but there's a real chance for a good result.

[laughingcreek]

I haven't had a chance to try my hand yet. but one thing I've observed from the attached canvases is that frames 8-10 are identical. (11 nearly so but the side profile shows there is a slight difference even though it doesn't show on the frame profiles).

that means that those frames should be a straight extrude, NOT part of a loft.  this is VERY fortuitous because now you will have a surface to define curvature at the edge of the lofts that extend off this middle section.   this area needs to be the first surfaces created.  trying to loft thru this section from adjacent areas will never achieve the correct surfaces here.

[davebYYPCU · Accepted solution]

Agree with Alex about the Extrude, I did that and then had so many other surfaces, I ignored it in the end and replaced with another small simple loft for it.

With license, your line drawings have inaccuracies, so some points made to align with the side view as priority.

You had followed a common mistake of too many spline points and too many bulkhead sketches.  Break it down to sections, and when stitched together, not too bad.

As you didn't start at the stern, I have left you plenty of room to attempt it yourself.  Your old work is right of timeline marker.

(I am travelling till mid Feb and will not be able to respond with desktop access.)

I am not one of the Tspline experts.

Step up the timeline and Edit features for settings.

Might help....

[l.cariouVF6EP]

Thank to all of you guys, I really appeciate the effort.

For a bit of context, I am comfortable with solid functions, I already used loft before but not at such level. For mechanical shape I am ok but for organic shapre I am definately a noob. I started to follow the video of "Learn Everything About Design" on youtube which I think are great to learn more on that. If you have better learning source to propose you are more than welcome.

Here are just 2 examples of the stuff I am designing, 2 cranes for oil & gas vessel, designed for 3D printing (FDM and SLA) + laser cutting. Fully functionnal, scale 1/72.

cranes

And then a first test to see how it looks on an ongoing fabrication done by my friend.

vessel

So here is my homework for the next days:

• Check profiles to round dimensions
• Check splines to simplify it
• Mix extrusion for the straight section and loft or modify profiles to avoid 2 similar profiles in the loft function
• Open and analyze files provided by Wersy and  davebYYPCU

When I said I was reluctant to learn a new cad software it's because F360 seems very powerful, I am aware that I am probably using 20% of it and for everything else F360 is enough for me. So learning a new software just to design the hull seems tidious. 

Thank again guys and I wish you a great day.

BR

Laurent

[l.cariouVF6EP]

Hello,

I check quickly the file you posted and closed the form to see if I can use afterward.

Unfortunately I have error messages when I tried to shell the solid. When you are back can you have a quick look to see if I am doing something wrong?

hull

BR

Laurent

[davebYYPCU]

There is a sketching / modelling error here (my Stern area) with this sliver section of the sweep body, that was then cut to shape, leaving a tail here.  Caused me some trouble earlier in the day but thought it was fixed.  You can probably get that sorted, but I am just about out of here.

I was able to boundary fill, but the Shell at 3mm failed.  I unstitched the surfaces and was able to thicken each panel to 3 mm. Combine joins all but that one body causing the error. 

Sorry I could not get it fixed, but that will definitely be the position of the cause of the problem.

For a plug, why would you need a skin?

Might help....

[l.cariouVF6EP]

I'll see if I can spot the error.

I have 2 options, I can thicken the face to 5mm for example, cut in pieces and 3D print directly the hull. I can also decide to thicken to 20mm for example, cut and 3D print and use it as a mould for epoxy/polyester resin + fiber glass.

Thanks for the help

BR

Laurent

[wersy]

Hi @davebYYPCU,

I am thrilled how you manage to create such a perfect hull from extremely few guidelines.
It makes me realise how little practice I have with surface work. I still have a lot to learn.

On the other hand, you can see how difficult it is to draw a hull when the shape is supposed to correspond to the frames - even if only approximately.
The intersections on frames 14, 15, 17, 18, 19 show the differences.

[TrippyLighting]

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@wersy wrote:

I am thrilled how you manage to create such a perfect hull from extremely few guidelines.

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He separated this into several lofts to have much better control over the surfaces.

I mentioned that above 😉

However the surfaces also have at least a couple of problems. Those problem may not be visible in a 3D print, so from that standpoint they might be acceptable.

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@wersy wrote:

Hi @davebYYPCU,

...

On the other hand, you can see how difficult it is to draw a hull when the shape is supposed to correspond to the frames - even if only approximately.
...

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That is why I mentioned above, depending on the accuracy that is required to represent the original shape, Fusion surfacing tools might not be the right tool to do so. Let me explain:

In Fusion 360 and most other mainstream parametric CAD software surfaces are created from curves/splines.

Those curves usually define the boundaries f the surfaces. If a surface created  from such boundaries does not create the desired shape, there are two things that cn be done in such CAD software:

1. You can add more rails or profiles. But often users overdo it and then that results in surfaces that are even worse!

2. The other approach is to break a large surface down into smaller pieces, more than one loft. That is usually a better approach, bit also has limitations, as can eb seen above.

Ultimately Lofts cerate NURBS surfaces. The shape of a NURBS surface is determined by a rectilinear grid of control vertices. Other, non-parametric software packages provide tools that allow direct manipulation of these CVs.

There are also some software packages available that are specialized tools just for creating boat hulls.

On the other hand I suggested that T-Splines might be another way to approach this shape. T-Splines are similar to NURBS in that their shape is defined by a rectilinear gris of CV's. As opposed to NURBS in Fusion 360 we can directly manipulate those CV's.

It's worth a consideration 😉

[davebYYPCU]

First rendition, having done it once a second attempt may be more efficient.

I learned a long time ago that these types of line drawings can be inaccurate.  I therefore plump for the longest canvass, develope the early sketches and interpret what should be.

I will highlight the main problem I had, was the flat bottom keel, two sections were depicted in the top view but the piece in the middle was missing, hence 14 and 15 look bad in your pic, so then you refer to front and back for contours, and as Alex noted 8 - 10 are the same, so I used Tangent spline to connect them, for a cleaner Loft, over those line contours.  You should note there is no line contour at position 17.2, where the bow finishes at the keel, my curve accords with the thruster tube.

I agree with Trippy it’s what I can get given the Canvass quality, and Fusions Lofting rules, and stated output as a 3d print.  Most likely the contractors took the front contours literally.

(No access to Fusion till mid Feb)

Might help....