How to draw a boat hull

[andrewWMZPK]

Hello,

I want to do some power boat hull design. I've had some parametric modelling experience with solidworks but I'm new to Fusion 360. The end game is to build a 4m long open power boat from CNC cut flat panels (e.g.plywood or Duflex). I must understand how to draw this myself rather than borrow another design from grabcad.

I'm having great difficulty getting started and getting the basic chined hull form modelled. I'm sure there are plenty of ways to achieve this and it sounds simple but so far I can't control the basic hull shape.. 

1. I want planar bottom surfaces in the aft half of the boat (for efficient planing).

2. I want curved surfaces in the forward half of the boat that can be formed from flat panels (e.g. plywood or duflex).

I've tried sweeping sketched lines and sculpting t-splines but not with good results so far. I'm having difficulty with the combination of a curved surface coming off a flat surface.

I've attached a screen shot of a basic hull shape I sculpted from a t-spline box on the weekend. On close inspection the aft end bottom panels aren't flat even though I used the "flatten" parallel to a plane command. The aft "flat" panels appear to be affected by the curvature of the front of the boat (the bending spline). The t-spline surface appears to be distorted (more visible with zebra analysis) around the "flat" to curved transition area. I also don't seem to be able to add dimensions to control the size of the t-spline box. I can sculpt and pull the t-spline box to a rough dimension but not set an editable and accurate length, width, height, angles like dimensioning a sketch. Appreciate any advice as to how to accurately sculpt a hull from a t-spline box.

Also appreciate any advice as to whether I'm heading in the wrong direction with sculpting t-splines and suggestions for a faster, more accurate way to get a basic hull shape modelled.

Thanks!

Andrew.

[Mike.Grau]

Hi @andrewWMZPK,

Thank you for posting your question to the Forum.

Your design looks good, you might just want to add more edges to give your boat more details.

An option to design basic the shape could be achieved by using sketches and the loft feature in the sculpt environment.

The trick is, you would just create one side of it and mirror the other side, like in the picture here.

I have just created that quickly but you could follow this work flow:

1. Create a number of planes which might be sufficient enough to represent the surface
2. Create a sketch on every plane that woul represent a cut in this section of the boat
3. Use the "Loft" feature in the "Sculpt" environment and select multiple sketches
4. Delete the surfaces you would not need and mirror your design

Here is the link to the example design. Please, feel free to use it. http://a360.co/29HVRzu

 

I hope this helps and gives you more ideas how you could design it.

Thanks,

[TrippyLighting]

You should be able to achieve this by lofting between differnt sketch profiles. You might need rails to control the surface better.
It takes a litel getting used to but loft with rials can provide you with excellent control ofer the features you describe.

I would not attempt to do this particular shape with T-PLines (Sculpt, Form).

[TrippyLighting]

MIke, you are using way too many edge loops for this T-Spline.

Start with as few segments (edge loops) as you can get away with and only add when more detail is needed an a given area.

The fewer polygons you have to deal with the easier this is to edit. It also helps manintianing better surface continuity.

[andrewWMZPK]

Thanks for your help and advice Mike & TrippyLighting,

I'm going to work on the lofting options in the next few evenings.

Andrew

[andrewWMZPK]

I've been sketching some lines and curves to use as rails (chine lines) for lofts. After I use the modify, move command to pull the line or curve off the xy sketch plane (in a z direction) to create a 3D line I lose all the xy dimensioning I've added and I can't add any meaningful dimensions to the line ends or spline nodes. Sometimes it will dimension from the origin to a spline node but only in a straight line, not with any alignment to xy or z.. Any suggestions how I can sketch 3D lines with dimensions?

[Mike.Grau]

Hi @andrewWMZPK,

I`m glad that our suggestions helped.

You might want to use dimensions in the vertical cut planes to define the XY position and the plane could define the Z position of your points.

Could you perhaps share a screen cast with us that we can see what happens 

with the dimensions when you pull a line?

Thanks,

[jeff_strater]

@andrewWMZPK,

You are correct - in the current sketch environment, dealing with 3D geometry is very limited.  No dimensions, minimal constraints, minimal creation capability.  It's on our list, but at the moment, to be honest, 3D sketch enhancements are not as high as I'd like to see them, but we have a very long list.

Sorry not to have better news...

Jeff

[andrewWMZPK]

Thanks for your replies. I've attached a very simple sketch of a couple of lines I've pulled away from the xy sketch plane in a z dimension. Both lines had dimensions to the nodes when drawn on the sketch plane. The dimensions disappeared when I grabbed a node and pulled it off a plane. The only dimension I seem to be able to add once off the sketch plane snaps to tangents but not with any control..

[andrewWMZPK]

Also appreciate if someone can tell me how to permanently connect the nodes on my 3D chine line (which will hopefully become a usable loft guide rail) to the corner nodes of my stern, mid and bow cross section sketches. I tried to use concentric constraints but I couldn't get my 3d chine line to associate with the other sketches... I could move the nodes to align but they wouldn't connect. If I change a dimension on a cross section sketch the corner moves away from the 3D line again. Drawing attached.

[davebYYPCU]

I was following this thread to see how sculpt might work for my work, (model aircraft) and you now seem to have dropped sculpt, going for patch (or solids) to output your boat panels. 

More to the point Fusion can't flatten surfaces after obtaining the 3D model, but sheet metal is on the way....

An answer to your last post, I can't check this on IPad, so here goes, depends on what you have done first, bulkhead sketches, or spline sketches,

the result is the same, but techniques are different.

If the Rails came first, my method, 

I obtain Loft Rails, by drawing / dimensioned 2d curves, in the top and side view, then using "Intersect Curve" in the project menu area, to develop the 3D chine, as a 3D sketch.  

then it is a case of draw the bulkhead sketch/s, and "Intersect Project" the spline line, a red projected dot is the result,

and the sketch profile MUST snap to those projected dots.

If the bulkheads came first,

then using "Incude 3D Geometry" project the spine point of intersection from the bulkhead sketch/s into you 3D sketch for the chine/spline, and draw the spline snapping to these points.

Loft is very good at previewing each selection, will not continue if not happy.  It's very hard to find the source of the errors, so I normally select the first 2 bulkheads, then one rail at a time, when I have all the rails working add more bulkheads, helps debug the intersection errors if you missed a snap point.

Hope that makes some sense, will check your file tomorrow, if you need something else.

Browny

[andrewWMZPK]

Thanks for your advice Browny. I'm going to try your suggestions tomorrow night.

Yes, I've dropped sculpt for now as I'm not confident I can keep the aft planing surfaces perfectly flat. Quite important for my boat design for both planing efficiency (curves on a planing surface create unwanted negative lift, drag) and eventual fabrication with Duflex panels. I don't think sculpt would be useful for me unless I could dimension the t-splines. II guess there may be a way to connect a t-spline box to a lofted solid to get the best of both worlds...

I'm hoping the "Exactflat" app add on will be able to flatten my panels into something I can then convert to a dxf file for CNC routing. From the video tutorials Exactflat shows promise but I've not played with it yet.

Yea, I'd be super keen on you taking a look at my last sketch to attach my chine spline to the bulkhead sketch corners then loft along the rails. 

[davebYYPCU]

Hey Andrew,

You were so close, the Deck curve and Keel curve were both working as I found it,

I have updated the file with new name, so you can check out what I did,

From what I found in V8, I turned your chine sketch off, but did not delete it, there were two bow sketches, left the obvious one on, turned the other off.

Created Sketch 12 so you will find it, on the centreline plane, and making sure it was a 3d sketch, tick box in the sketch panel.

Then in the Project Menu, used "Include 3D Geometry"and selected the three chine points,

Drew line from rear to mid profile, then tangent arc to the bow, for the new chine rail.

(I didn't try to move your chine lines, was easy to replace it, let you compare / edit them,  and you can try the move now that the snap points exist.)

I see in your post you wanted a loft to be produced, went to patch environment, and got it working, had a crash, and some odd behaviour with the keel curve, had already tested it was OK

so selected it as the first rail to make it behave, Loft can be like that,  (It's turned off at the moment, so you can open the feature and check the selections)

I saw that App today when surfing the net for something else.  I haven't used it either.

Away you go...

Browny

[andrewWMZPK]

Massive thanks Browny.

Loft is a little tricky isn't it. It took a while before I figured out I needed to select the profiles before the rails. The first loft preview was ugly then it magically got progressively better looking as I selected the three rails. Quite similar to the way people usually get better looking after each beverage consumed.

Cheers, Andrew.

[davebYYPCU]

You got that right.

[andrewWMZPK]

Help.. I seem to have broken my loft in model workspace..

I've been playing with the dimensions on my profile sketches and the loft appears to have broken free of my mid plane profile sketch.. 

Also, my bow profile sketch appears to have moved sideways away from the centre plane without my deliberate editing and I don't know why.

Also, is there any reason why I can't see my tunnel cut on the browser tree so I can turn it on and off (I can see it in the timeline)?

[andrewWMZPK]

Hi there. If I edit one of the sketches defining the attached hull cross section shape (say the mid plane) the link between the cross section and the chine 3D sketch is broken.. Surely I don't need to redraw the associated chine sketch (which is used as a loft rail) every time I want to tweak a cross section sketch? Any suggestions what I'm doing wrong here?

[davebYYPCU]

Late now, the yellow sketch icons have to be fixed,

Will reverting to an earlier version have normal sketch status?

Because the sketches are broken, the lofts ae too, appears there are two lofts on top of each other

Depends how you edited the profiles, I have not seen this myself,

guessing, did you drag the end points, or

delete line and redraw new ones, the latter will unhook from the chine,

the former won't if all things are normal.

More later,

Browny

[cekuhnen]

@andrewWMZPK Hard to say what happened. Be very careful with moving points after the sketch got constraint - specifically when moving elements that are in a relationship to elements from a different sketch. That can quickly explode.

Out of curiosity, do you want in the front of the boat the surface to be bend upwards and also caved in or bend upwards as a flat surface so you could use bend ply wood which you can only bend alone one direction well?

That is how I somehow read you initial T-S Model.

[Anonymous]

I too am modeling a boat from 20 stations.  I lofted in modeling mode.  is this different than in sculpting mode?  seems I can't select any of the body parts edges or faces in order to modify them.  my geometry all came via .dxf from draftsight.    what am I doing wrong?   you can see I lofted the exterior and then lofted the interior to hollow it out.  I sliced the boat into machineable-sized parts.  I can't modify these parts however.   http://a360.co/2aekaQO