ANSYS Composite Material Design

Discussion in 'Software' started by Yousra Anwar, Feb 25, 2013.

  1. Yousra Anwar
    Joined: Oct 2012
    Posts: 7
    Likes: 0, Points: 1, Legacy Rep: 10
    Location: Alexandria,Egypt

    Yousra Anwar Junior Member

    Hi,
    I am Preparing a midship section by using the Ansys for a composite material boat, I am using Shell 181 for & Solid 185 for the foam core stiffeners , shall I used a contact between the hull shell 181 & Solid185 or there is a way to glue them together?
    Thanks
     
  2. Ad Hoc
    Joined: Oct 2008
    Posts: 7,077
    Likes: 1,009, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Yousra

    You need to be careful here. Do you have any data to validate the elements and their build up and the final properties post layup? Otherwise you're focusing on getting a model that in the FE is "correct" but does not reflect reality. Getting meaningful data from FEA when using composites is not as straight fwd as it is with typical isotropic materials.
     
  3. Yousra Anwar
    Joined: Oct 2012
    Posts: 7
    Likes: 0, Points: 1, Legacy Rep: 10
    Location: Alexandria,Egypt

    Yousra Anwar Junior Member

    Thank you for the advise..I am Preparing my master degree in conposite material optimisation.. I have already prepared all the calculations for the conposite.. I have treated it as orthotropic material.. I have also chosrn shell 181 in order to enter layer by layer..the only problem I have so far is the Ansys...I really dont know is there a way to glue shell 181 to solid 185.. Is there another way to prepare the stiffeners and in the mean time shows the unidirectional fiber on th crown only and the different layers that covers the whole section
     
  4. rxcomposite
    Joined: Jan 2005
    Posts: 2,402
    Likes: 394, Points: 83, Legacy Rep: 1110
    Location: Philippines

    rxcomposite Senior Member

    What is shell 181 and solid 185? Product code?
     
  5. Yousra Anwar
    Joined: Oct 2012
    Posts: 7
    Likes: 0, Points: 1, Legacy Rep: 10
    Location: Alexandria,Egypt

    Yousra Anwar Junior Member

    Shell 181 & Solid 185 elements of Ansys, Sorry I really don't know what you mean by product code. please advise
     
  6. rxcomposite
    Joined: Jan 2005
    Posts: 2,402
    Likes: 394, Points: 83, Legacy Rep: 1110
    Location: Philippines

    rxcomposite Senior Member

    I thought you were referring to a Shell composite product.

    You are mixing up the analysis method. In aerospace technology, laminates consist typically of a large number of thin plies of the same material of (about 0.010”) ply thickness. The multiple plies are arranged in a progressive angle orientation (0, 30, 45, 60, 90 degree) to achieve a balanced laminate where it yields an isotropic property in in-plane loads. The laminate is treated as a homogenous material with a degraded material property to take care of out of plane loads. In short, the material is treated as a dense material with an isotropic material property like metal. Preliminary design analysis can therefore establish the baseline for optimization before fine tuning with FEA.

    In marine structures, laminate consists of much fewer but thicker plies. Varying materials are also used other than UD fiber. This makes it sensitive to out of plane loads, ply angle, distance to neutral axis, tensile/compressive strength, fiber volume ratio, ect. For significant out of plane loads, the “homogenous material” treatment renders the results somewhat impractical and meaningless for marine structures. For multiple layers of varying materials and layer by layer analysis the “maximum strain theory” is a better method. The method becomes more practical when the need for stiffener/plate combination is analyzed.

    Attached is the tabulation of maximum strain theory (by M. Hollmann) as applied to complex aircraft structures. This method is also used with slight variations, by Lloyds, ABS, BV, and ISO, to name a few.
     

    Attached Files:

  7. Red Dwarf
    Joined: Jun 2012
    Posts: 234
    Likes: 6, Points: 0, Legacy Rep: 61
    Location: USA California

    Red Dwarf Senior Member

    Just a bit of advice, throw away the M. Hollmann books. There are dozens of reputable books on laminate analysis that will give you better information. I'm not going into Hollmann's issues, let's just say he is infamous within the aerospace industry.;)
     
  8. rxcomposite
    Joined: Jan 2005
    Posts: 2,402
    Likes: 394, Points: 83, Legacy Rep: 1110
    Location: Philippines

    rxcomposite Senior Member

    RD,
    I have better books and softwares but Hollmann has the basics. Sure there was a lot of typo errors in there and gave me some headaches but since I have straightened it out, I still refer to it from time to time.
     
  9. rxcomposite
    Joined: Jan 2005
    Posts: 2,402
    Likes: 394, Points: 83, Legacy Rep: 1110
    Location: Philippines

    rxcomposite Senior Member

    Just to inform you, M. Hollmann passed away last year. May he rest in peace. In the early days of composite, he was the guy to run to. I share some of his friends.

    For the issue, here is what they say:
    "I was poking around the web and came across this page announcing the death of Martin Hollmann, to cancer, on 12 Oct 2012.

    Hollmann designed the composite 6-place Stallion aircraft and wrote/published many books on amateur/homebuilt composite design. No author receives universal acclaim and I know there has been some critique on this board about some of his design methods, but I think it's fair to say many find his books provide useful references in a field where there's a paucity of information for the non-professional designer.

    Anyway, because he's well known among the "fibers and goo" crowd here, I wanted to pass the word along. To those who knew him, my condolences for your loss.

    Mark" http://www.homebuiltairplanes.com/f...igner-author-martin-hollmann-passes-away.html
     
  10. Ad Hoc
    Joined: Oct 2008
    Posts: 7,077
    Likes: 1,009, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    I am not familiar with Ansys. However in the FEA I use, Cosmos/M, there is a feature where you can "bond" the 2 element types together, and selecting how the translation is to be performed. I am assuming there is a similar feature in Ansys, otherwise you may have to do this manually and iteratively.

    You mat find this forum of use on the subject too:
    http://www.xansys.org/forum/viewtopic.php?p=66010&sid=77aa2f3e068db7808c459cf42cff6199
     
  11. Yousra Anwar
    Joined: Oct 2012
    Posts: 7
    Likes: 0, Points: 1, Legacy Rep: 10
    Location: Alexandria,Egypt

    Yousra Anwar Junior Member

    Thank you very much I will Check it :)
     
  12. petereng
    Joined: Jan 2008
    Posts: 581
    Likes: 22, Points: 28, Legacy Rep: 252
    Location: Gold Coast Australia

    petereng Senior Member

    Hi, I'm not a Ansys user but have used Lusas and Strand. You need to be careful when connecting plate elements to solid elements. You have to check that they are coupled correctly. If you just connect the plate "on edge" it will act as a hinge. You will either need to add some analytical links or some geometry to ensure the local moment is correctly transfered. Ideally you would work in all plate elements or all solid elements. Usually I develop a design in plate elements and if an area is critical then either sub model it as a solid or do the entire thing as a solid. At each step check your assumptions are correct. Firstly in FEA you need to be clear what you are looking for. If you only require a stress plot then use plates all the way. But plates will neglect things like asymetric loading of the skins. So if you are trying to determine if a skin locally buckles then you have to use solids for the core and plates for the skins and ensure you have a contiguous mesh through the whole lot. If you use analytical links to "glue" discontiguous meshes eg a hull to a bulkhead then you ahve to be careful that you iether under constrain it or over constrain the connection. Better to build good mesh from the start. You must know what you are looking for and build a suitable model. What are you actually looking for? Cheers Peter S
     
  13. kvsgkvng
    Joined: Jan 2012
    Posts: 212
    Likes: 8, Points: 18, Legacy Rep: 49
    Location: *

    kvsgkvng Senior Member

    You have to extend plate into solid in order to develop moment connection. Otherwise your shell member will flap like a door hinge with no moment continuity.
     
  14. ESAComp
    Joined: Apr 2013
    Posts: 2
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: France

    ESAComp New Member


  15. petereng
    Joined: Jan 2008
    Posts: 581
    Likes: 22, Points: 28, Legacy Rep: 252
    Location: Gold Coast Australia

    petereng Senior Member

    Hello Yousra - have you resolved your problem yet? My advice would be to model the entire structure in shell elements first. The core then becomes one of the plies in the laminate. As long as you do some basic checks to confirm the sandwich does not wrinkle its skins or delaminates then this is the best starting point. Once the design has been run and you understand its performance then you build the final model with the cores as solids and the skins tesselatted to the core. If you try to use connection type elelents between the solid and the skins (eg bonding or attachments) the solution time will be huge. Tesselation means the skins and the solids share the same nodes. Hope this helps. Plus your material mechanical data needs to be correct.Cheers Peter S
     
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.