Testing boat structure with FEA

Discussion in 'Boat Design' started by EddieGreen, Feb 13, 2021.

  1. Ad Hoc
    Joined: Oct 2008
    Posts: 6,792
    Likes: 741, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    But do you know the limitations and who says it is more efficient?

    That is the skill of FEA, as knowing how to model, using the correct elements, applying the most appropriate mesh is all part of the knowledge of the user and their understanding of FEA to produce results with confidence.

    Incorrect mesh, aspect ratio and type of element yields very very different results, when compared to theory as shown below:

    upload_2021-2-15_8-30-59.png

    Dumbing it down, as many other CAD packages have done over the years, does not = confident results.
     
  2. TANSL
    Joined: Sep 2011
    Posts: 6,437
    Likes: 367, Points: 93, Legacy Rep: 300
    Location: Spain

    TANSL Senior Member

    Do not alter the order of my comments. That's a very ugly trick. And how many FEAs have you personally done? None, the same as me, and yet you continue to comment as well. How do I know? It is deduced from your explanations, very theoretical and impractical, obsolete as always. We all know how to read books and "cut and paste" is very easy. And forget me, please, dear "professor."
     
  3. DCockey
    Joined: Oct 2009
    Posts: 4,883
    Likes: 424, Points: 83, Legacy Rep: 1485
    Location: Midcoast Maine

    DCockey Senior Member

    Scan and Solve linear structural analysis software, which the original poster EddieGreen is user, has significant differences from conventional finite element analysis software. Scan and Solve uses a uniform orthogonal grid which does not conform to the geometry. It does not use distinct "elements". A 2009 white paper about the methodology with some references is available at http://www.intact-solutions.com/Scan&Solve.pdf

    I have not studied the methodology enough to provide any further comments.
     
  4. Ad Hoc
    Joined: Oct 2008
    Posts: 6,792
    Likes: 741, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Thanks for that DC.

    Upon a brief read, it appears to assume a 'solid' that is prismatic and does not use shape functions, as it sees them as... "Scan&Solve™ was developed specifically to liberate FEA from the tyranny of meshing,..."
    Interesting turn of phrase!
    It is an interesting method though... yet I do not see this being widely adopted, considering the first use of the method half a century ago.
     
  5. an2reir
    Joined: Sep 2001
    Posts: 627
    Likes: 120, Points: 53, Legacy Rep: 110
    Location: Bordeaux France

    an2reir fifty boat designs

    Hello there I wish you a wonderful week from France ! thank you for pointing the thread to me!
    I state here I am the one guilty as charged to have created the FEA animations this thread was started with.
    I am as we speak working on highly complex composite systems on large custom motor yachts in France and I think I did 200 simulations over the last 300 days
    My experience includes having introduced the Scan and Solve FEA software in Rhino to the Royal national Lifeboat Institute UK while serving in the Marine Engineering and Naval Architecture Department in Poole UK 20014-20016
    The reason for doing that was typically the procedure for FEA testing in the RNLI was to pay rather high amounts of money to subcontractors to do the FEA analysis and the implementation of a handy FEA software to test struictures in house seemed to be helping on that
    I started by doing a parallel comparative FEA analysis of a aluminium boat structure of the RNLI Atlantic boats with Scan and Solve and I compared with the FEA done by a sobcontractor in another mainstream FEA .
    The results were very very close and I repeated a number of times on different structures
    This validated the Scan and Solve at that moment
    Since then the Scan and Solve has evolved to today's Scan and solve Pro who does simulate composites fiberglass as well as wood and metals
    The hulls of RNLI boats were tested by FEA simulations amongst other procedures of testing
    In real life Boat Company Engineering office practice I do not work with one FEA system alone but I work with two or even three FEA software and I cross examine the results
    As we speak I am heading to office where we cross examine today the testing of a boat structure by Rhino Scan and Solve with simulations we did with Hypermesh FEA
    Regarding the testing of the hulls and where to place the constrains:
    1. I place my constraints on the surface of the sheerline of a hull module. This practice is the one used not only by me but by a number of naval archtecture offices in UK and France. For other simultations I place my constraints on a hull panel edges or on the boat bottom chine or on the LWL . All these options do imply limitations of the FEA results but I am well aware of those limitations and I do take them into consideration
    2. in the particular cases of the two FEA animations of wood boat structures this thread was started with
    the constraints were placed on the sheer surface.
    The FEA will show me if the wood boat structure does take without breaking the slamming or collision load on the boat bottom I am subjecting the structure to - wich are the regions of the boat structure and or framing joints where I have weaknesses



    I will respond to the other queries later on .


    Have a wonderful week
     
    CocoonCruisers and EddieGreen like this.
  6. Ad Hoc
    Joined: Oct 2008
    Posts: 6,792
    Likes: 741, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Hi Andrei..

    Thanks for the comments/reply.

    I have not come across this programme before, nor am I familiar with their method; using the Kantorovich method.
    I only know the methods/programmes I have been using for the past 30 years. It does seem at variance with this Scan&Solve in its methodology, but it also does appear (upon limited checks) to yeild consistent results.

    It is an interesting way of performing structural calculations within an FEA environment.

    I do find this comment interesting though:-
    What load case scenario is this simulating?
     
  7. an2reir
    Joined: Sep 2001
    Posts: 627
    Likes: 120, Points: 53, Legacy Rep: 110
    Location: Bordeaux France

    an2reir fifty boat designs



    Hello Ad Hoc


    I am now at my yacht company office nearby Bordeaux I need to read all the above comments in the thread to give them proper thought;


    Regarding where to position the constraints on a boat hull CAD geometry :

    1. I am placing the constraints on the composite boat hull module sheer line and the module incudes the keel the module is a cut of the aft section of the keel including transom and cut just forward of the main bulkhead constriants are as well placed on the transversal section
    I am loading a loadcase of bilge keel subject to grounding forces
    My displacement is 24 tons I apply a horizontal load of 54 tons on the lowest point of the forward of the keel

    2. Nonetheless I did as well do other simulations where my constraints are placed on the edges of a small boat bottom module to with a keel frame made of metal is bolted on like this one I attach here; This visualisation that is attached here is done in Autodesk Fusion 360

    3. Regarding the Bureau Veritas Rules

    The FEA simulations of the boat structure need to deliver results to be in compliance to the ISO or BV rules

    In order to do that I work as well with the Bureau Veritas who has its own software that is called Compose IT

    Compose IT is a softaware that calculates the compliance of a boat bottom laminate to the BV rules

    The compose IT software does have the capability of testing of a boat bottom panel and validate the panel

    I will enter the max stress values resulted from my Scan and Solve simulation in the BV Compose IT and realise this way validation of my scantlings against BV Rule


    4. Regarding the testing of wood boat structures like runabout framing structure: from my understanding of the ISO rules and of the Bureau Veritas and RINA and ABS rules if I set up my simulation by constraining the wooden hull sheer strake and a apply a load on the boat bottom surface equal to the slamming force multiplied by 2 and the wooden boat framing shows no breaking I think the boat is good
     

    Attached Files:

    Last edited: Feb 15, 2021
    EddieGreen likes this.
  8. EddieGreen
    Joined: Feb 2021
    Posts: 16
    Likes: 2, Points: 3
    Location: Nice

    EddieGreen Junior Member

    Hi all ... and thanks for your contributions which are ALL well appreciated ! Moreover a big thank you to Andrei who has accepted to join this thread and has taken the time to further explain his use of SnS with practical examples.

    I can confirm several design offices already using Rhino (by the way becoming a parametric CAD tool with the latest versions) are indeed using SnS in addition to other FEM... actually this is what triggered my curiosity.

    I continue to believe pre-processing is not that easy to master, plus cleaning an already existing model/geometry to make it mesh friendly is a tedious and not totally error free endeavor.

    Obviously any tool being only as good as its user, i am still trying to learn more, notably re. these restraints and boundary conditions.
    A sheer line (and even a full length chine) being usually stronger areas, it doesn't look awkward to me to apply some restraints there, as long as the studied geometry is not in its immediate vicinity ?

    Thanks for confirming my question is genuine, apparently am ignorant, but not totally stupid (just kidding ... english is not my first language)

    @fastwave : you either said too much, or too little !

    Can anyone explain this further for the layman ? notably this spring set-up , or mention freely available resources ?

    We want to discover all these tricks ! Sounds more sexy than Hilbert & Sobolev spaces, Taylor series, Lagrange equations ...

    Thanks again !
     
  9. gonzo
    Joined: Aug 2002
    Posts: 15,111
    Likes: 896, Points: 123, Legacy Rep: 2031
    Location: Milwaukee, WI

    gonzo Senior Member

    A spring is a constraint that is not rigid, hence a spring. For example, you can use that to model the difference in pressure as a body submerges. The K value of the spring will be the same as pressure change with depth.
     
  10. Ad Hoc
    Joined: Oct 2008
    Posts: 6,792
    Likes: 741, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    I have been trying. But it appears you want a simple click and go solution.
    There isn't one... it is more nuanced than that.

    If the spring [K] is supporting the model that is perpendicular to its support, it is a function of the distance between the main loading bearing structure, or WTBs, the shear area of each structural member and the number of load points used.
    If the spring is not normal, or rather tangential, to the model it is supporting, it subtly changes, as it becomes more dependent upon the 'length' of the spring and the E must be accounted for.
    If the spring is to account for longitudinal structure, rather than transverse, then the I and E must be account for, for each structural element, as well as the shear area and the number of load points.

    Thus it is not a plug and play....

    In my analysis, I avoid this by ensuring the model mimics reality as closely as possible.
    For example, in a multihull, a classic transverse bending moment, what is occurring... the 2 hulls are being rotated and pushed towards each other. This can only occur if there is a point/location where there is zero displacement relatively between the 2 hulls, otherwise it is not in equilibrium. This location is obviously the centreline of the vessel. So, I apply boundary conditions on the vessel's centreline.
    This does the same job as a spring.
     
  11. gonzo
    Joined: Aug 2002
    Posts: 15,111
    Likes: 896, Points: 123, Legacy Rep: 2031
    Location: Milwaukee, WI

    gonzo Senior Member

    In short, understanding the structure and its environment is the work that needs to be done before approaching FEA. Having experience with design also allows the designer to assess if the results make sense or not. For example, if there is a plate with an applied force, I can tell that the deflection is going to be within certain range. For example, if FEA is giving me a result that a plate that is 20 feet long and is supported at the edges deflects 700 feet, I know it is wrong. FEA will give crazy results if limits are not manually applied to the calculations.
     
  12. EddieGreen
    Joined: Feb 2021
    Posts: 16
    Likes: 2, Points: 3
    Location: Nice

    EddieGreen Junior Member

    I still do not see clearly the interest of using these springs (yes i am kind of slow !)

    In this case, is this the same as applying loads (and not constraints/restraints at some selected boundaries ??) which are proportional to the distance, and reach equilibrium ? would this mimic for instance the loads from the hydrostatic pressure increasing with depth ??

    This example i can understand pretty well e.g. like a beam with loads and restraints which are symmetric.
    I have also seen this as a demo/exercise :
    Model into static equilibrium, to satisfy the need for some kind of restraint, need to choose a convenient location. For this loading, the best choice to restrain the model is where the slope of deflection will be zero. In this case, zero bending slope occurs at the mid-point of the beam because the loading is symmetric. This example restrains the midpoint edge at the bottom, although the edge at the top is also a valid choice.

    However i still don't see why it would do the same job as using a spring ?
     
  13. gonzo
    Joined: Aug 2002
    Posts: 15,111
    Likes: 896, Points: 123, Legacy Rep: 2031
    Location: Milwaukee, WI

    gonzo Senior Member

    I think you are not considering the deformations of the hull created by the applied forces. I have seen a boat dismast twice because the designer failed to take deformation into account. It was an IOR skimming dish with a highly tension rig and short spreaders to allow the genoa to be sheeted in tight. On higher winds the compression of the mast would push the keel down and the tension of the shrouds and stays pull the sheer up. That would cause the rigging to loose tension, the mast get out of column and buckle.
     
  14. fastwave
    Joined: Jan 2007
    Posts: 106
    Likes: 12, Points: 18, Legacy Rep: 36
    Location: europe

    fastwave Senior Member

    Hi guys,
    There are many correct ways to perform FEA constraints depending on what question you are asking. I think my hint on springs w.r.t. the original question was clearly an overkill for the user, but I just wanted to share it to get some people thinking.
    Depending on the structure a more complicated model is needed. For example modern imoca structures have very thin ribs and longitudinals for a very thin panel support. If you constrain the panels on the edges you will get wrong results. You need to propagate the energy from a slamming analysis into the entire structure. A stiff classic bulkhead support will not do that and you don’t need to go to the extra complication perhaps.
    Also deflections as described above can have huge consequences as well said above on modern minimal structures.
    Here is a link to a very brief discussion on restraining models. There are others out there but the design details are kept secret.
    However anyone who knows what they are doing can come up with the details himself to perform a spring approach model.
    There are also other ways which I cannot discuss further.
    Again, this is at a different level to what the original post is about.

    https://repository.tudelft.nl/islan...856-a1d2-7f4633556032/datastream/OBJ/download
     
    EddieGreen and Ad Hoc like this.

  15. Ad Hoc
    Joined: Oct 2008
    Posts: 6,792
    Likes: 741, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Well, you need to understand the basics of springs, what is a spring and what does it do?

    It is a member that obeys Hooke’s law, and only resistance forces in the direction of the spring, which is why you need to be in the placement of springs in the FEM. So the spring itself, as previously noted we can then establish that a prismatic uniaxial bar (a rod if you like) that obeys Hooke’s law has a spring constant k = AE/L where A represents the cross-sectional area of the bar, E is the modulus of elasticity, and L is the bar length.

    So, knowing this, what does the spring(s) do in the FEM?...just as any ‘normal’ spring dopes, it resists forces up to their yield limit. Why is this important?...well, as noted previously, you need to prevent the FEM from rigid body motion. Because if the model has insufficient boundary conditions, in this case – restraints – the model will not behave correctly. This is manifested by the stiffness matrix, inside the computations, as providing incorrect solutions, or no solution at all, as the stiffness matrix is singular! Because each node in the FEM can have up to 6 degree of freedom, depending upon the element type selected for the analysis. And given that each node has up to 6 degrees of freedom, unless all 6 degrees of freedom – anywhere in the model – the model is not fully restrained and thus = free body movement. In simple language it will move when it should not do.

    If you image standing with your feet apart and you are holding a rope. This rope is then pulled, what does it do… it pulls you over and you will possibly fall down or even then be dragged away from your standing position. There will still be a force and hence a ‘stress’ on your body, but your body is no longer in the same position prior to the rope being pulled. It has moved..

    If your foot is strapped in some manner to the ground so your foot cannot move, when the rope is pulled, you rotate about that foot. Your body is still experiencing the force that is applied, via the rope, and thus still under some degree of stress.

    If both your feet are now strapped in, and the rope is pulled, all the force goes directly into your body and the stress is dissipated throughout your whole body. Your feet do not move, ergo your whole body is now under a state of stress. But because your feet are constrained from displacement, this shall attract the stress, owing to its ‘infinite’ stiffness. If the strap is made of thin wire…your feet will most likely bleed and be cut in two…as the force/area of the wire is near infinity...a cheese wire. Whereas, if you are wearing a shoe, and the whole shoe sole is welded or glued to the ground…the stiffness is spread over the whole sole of the shoe…and your feet will no longer hurt or be cut in two!. But will there be “some” discomfort, probably… and this is the whole point…if you analysis is concerned with the stress in the armpits joints and shoulder blades, you do not worry about what the stress is showing in your feet. Because you reduce the stress as much as possible, by spreading out the restraints as much as possible to reduce the stiffness effects, and then you only focus on the stress where you are interested.

    So, the objective is to apply boundary conditions that either, as previously noted, restrain displacement or a by the application of force – a spring – to prevent rigid body motion, but do not influence the results you are seeking.
     
Loading...
Forum posts represent the experience, opinion, and view of individual users. Boat Design Net does not necessarily endorse nor share the view of each individual post.
When making potentially dangerous or financial decisions, always employ and consult appropriate professionals. Your circumstances or experience may be different.