×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Honey comb modeling
8

Honey comb modeling

Honey comb modeling

(OP)
Hello everyone, I am new to NE nastran and i want to analyse a honeycomb structure with aluminum facings and a honeycomb core. Could anyone guide me as to how to assign the material properties and is there any example which would be useful. I would really appreciate any kind of help. Thanks
                                     Sakota

RE: Honey comb modeling

2
Sakota,

You are trying to enter a "sandwich" composite.  You will first want to define othotropic materials for your honeycomb and, although it is isotropic, it is easier to define an "orthrotropic aluminum".  "orthotropic aluminum" has the same material properties in all directions, but it allows you to select it when defining your property.  Honeycomb cores have known directional properties...you can get them from the manufacturer.  Enter the two different materials (aluminum and honeycomb) so that you can select them when you are defining your thick (sandwich) composite property.  This should get you started.

Garland

Garland E. Borowski, PE

RE: Honey comb modeling

Look in the NEiNastran User's Manual, Special Topics section.  There is a sandwich example there.  

There are 2 ways you can do this:

1.  Use a composite laminate property and define 3 layers.  Layer 1 is the bottom facesheet, layer 2 the core, and layer 3 is the top face sheet.  In the Reference Manual under PCOMP you will see some other settings field 9 (LAM) that allow you to specify the core type for facesheet stability index calculations.  You would need to change these in the Editor.  This step is optional.  

2.  Use a single PSHELL property and adjust the bending stiffness parameter, TS/T, etc.  I recommend #1 above because it is easier to set up.  

RE: Honey comb modeling

I would add that Frank's option #1 is likely to be more accurate than option #2.  Laminated plate theory for a sandwich composite is a bit more complicated than just an alteration of the bending stiffness parameter, although bending is the largest impact.  You need to be able to examine your core failure modes.  For an uncored composite, you can use an orthotropic shell element if you know the "smeared" properties of your composite, which, personally, I prefer to calculate outside of the software as a check on how I entered the information.

Garland E. Borowski, PE

RE: Honey comb modeling

(OP)
thanks everyone. i really appreciate your time and patience. Meyers,I have still not looked into the manual but would do so now.If i have any problems shall post the problem here..thanks  once again.
           Sakota

RE: Honey comb modeling

(OP)
ok, i have a question. I am modeling my core using 3d orthotropic properies but whn i run it its converting the material properties  to 2d orthotropic because of the quad elements used to model the shell. What i am concerned about is the how do i give the compressive modulus if i can define the 3rd direction properties.do i juss leave it?

RE: Honey comb modeling

(OP)
ooopss one more question.. the core is aluminum honeycomb. so,it has no elastic modlus and poisson ratio. so how do i define the material property? i used orthotropic but then it needs a E and a possion ratio.Thanks

RE: Honey comb modeling

Let's try to answer your first question:

3-D orthotropic properties are for orthrotropic brick elements, not quad elements, so that is why it is reducing the inputs to 2-dimensions.  To have the 3-D properties, you would have an 8 to 20 node, 3-dimensional representation of the skin (including thickness) or core.  As modeled, the thickness is handled by the laminated plate theory that is being used, or, if you are not using one of the composite material element types, then it is not concerned with your third dimension.

As for the Aluminum honeycomb, it still has material properties that should be available from the honeycomb core manufacturer.  They are not 10e6psi and 0.33 like typical aluminum.  Check the web for aluminum honeycomb.

Garland E. Borowski, PE

RE: Honey comb modeling

GBor,
 A star for your patience

www.probasci.com -
Implantable FEA for medical device manufacturers

RE: Honey comb modeling

Much Thanks! :)

Garland E. Borowski, PE

RE: Honey comb modeling

(OP)
GBor, Thanks for your reply..I have some properties for the core but the things is i am trying to figure out where to input it. i am using orthotropic 2d for the core and i have modeled the top face of the upper facing in the 1-2 plane.And from the properties i have a compression modulus which would be E3. But i dn't have option for E3, its only E1 and E2.. so do i have to define a local co-ordinate system to define the compression modulus and the L, W strength? Thanks once again

RE: Honey comb modeling

If I understand correctly, the problem is that you are trying to give 3-D properties to a 2-D element type.  2-D orthrotropic element types will not consider the out of plane compression and, therefore, is not concerned with E3.

OK, time to "knock some cobwebs loose".  You have to define your element type as "Laminate".  You set up two different materials:  one for your aluminum skins and one for your core.  Your aluminum skins can be 2-D orthotropic, but your core would need to be 3-D orthotropic, not 2-D.  When you define the layers in your laminate, select material 1 for the first skin, give it a thickness...you may even be able to use isotropic material properties for this...I haven't really tried it this way.  For the second layer input into the laminate, select material 2, give it a thickness.  Then for the third layer in your laminate, select material 1 again to provide for the other skin.  My only concern is whether you can apply a 3-D orthotropic material to a 2-D representation.  I have to admit that I'm not sure how the processor will handle this.

Garland E. Borowski, PE

RE: Honey comb modeling

(OP)
Gbor, that is eactly how i modeled earlier. But it dsnt take 3d orthotropic properties since the core is a 2d representation and the thickness is given through section properties and not thru the nodes. So, i donno how to assign the material properties that i have for the core. the properties that i have are:
        compression modulus
        Compression strength
        L direction shear modulus
        W direction shear modulus
Any inputs??
        

RE: Honey comb modeling

2
Kotawsu,

You have to tell us how you plan to model the structure and what type of elements you are using.  If you are using 2D shell elements, then the thru-thickness E3 and strength properties are not used.  However, NASTRAN does use the thru-thickenss transverse shear stiffnesses, G13 and G23.  With 2D elements and compositeee/sandwich materials, you define properties for each layer as a Material, then combine the layers in a Property; the core is treated simply as a different layer.  For in-plane properties of the core you enter some small dummy properties (I typically set E1=E2=100, G12=50, nu12=0.0).

If you are using 3D solid elements (where the skins and core could be modeled with separate elements) then the full 3D set of properties is required.  

If you are using 2D elements, then read about the PSHELL, PCOMP, MAT2 and MAT8 cards in the manual; if you are using 3D elements read about the PSOLID and MAT cards in the manual.

RE: Honey comb modeling

(OP)
Thanks SW for your input. But for a honeycomb core E1 and E2 are zero and it has only compression modulus which is E3. But since i have modeled juss the upper facing of the skin and defined the thickness through section properties i am forced to used 2d elements which means that i dnt have an option of entering E3 which is the compression modulus. In order to avoid singularity am entering small values for E1 and E2 even though they are zero. So the compression modulus which is the out of plane modulus is what causing the difficulty here.

RE: Honey comb modeling

OK.  I can't figure out how else to say this other than:  You have to model your situation differently...or at least think of it differently.  Cores generally exist for one purpose...to transfer load from the inner skin to the outer skin.  It does this not by Young's modulus, but by the shear carrying capabilities...in other words:  G13 and G23, as SWComposites has stated.  In NENastran, these values show up in 2D orthotropic materials as G1z and G2z, respectively.  If all you have is E3, but you know that you have aluminum and it is isotropic, estimate G1z and G2z as approximately equal and having a value of E/2(1-v^2) (I think that's the isotropic formula...someone please confirm or I'll look it up later), where v is poisson's ratio (about 0.27 for aluminum, I think).

Garland E. Borowski, PE

RE: Honey comb modeling

(OP)
Gbor, thanks for the patience.. i solved the problem that i had using 2d orthotropic.

RE: Honey comb modeling

The isotropic formula GBor mentioned should probably be:

G=E/2(1+v)

But I'm not so sure that you can simply use your E3 to calculate the G-value for a honeycomb.

I would recommend that you look at the chapter on honeycomb plates in the FEMCI book:

http://femci.gsfc.nasa.gov/femcibook.html

Good Luck

Thomas

RE: Honey comb modeling

Thanks for the correction, Thomas, I should know better than to try and remember an equation...even one as simple as that!  As for the calculation of G from E3, it's an approximation.  Probably not precise, but shouldn't be too far off.  He does still have an isotropic material even if it is in a honeycomb.

Garland E. Borowski, PE

RE: Honey comb modeling

Thomas,

Great Reference!  A quick glance says the following:

"The shear modulus and the poisson's ratio is required on the MATERIAL card for MID3 and is obtained from the HEXEL manuals. You need to know the cell size and gage, or the desired nominal density."

I completely agree with this statement, but again say that an approximation, assuming a fairly small cell size and reasonable gage, is to use the isotropic equation.

Garland E. Borowski, PE

RE: Honey comb modeling

GBor, the isotropic formula for shear modulus DOES NOT APPLY to honeycomb core since the core is not a solid homogeneous material. Core shear moduli are usually available from the core material supplier.

RE: Honey comb modeling

I believe that for a SMALL CELL SIZE/LARGE GAGE, you can reasonably approximate through the isotropic equation.  I agree that the manufacturer is the place to go for the information and would reference my very first post to this thread.  Barring that as a posibility, if you have to make some assumption...

I understand that you have to understand "garbage in...garbage out".

With that, I quit arguing and agree with you...

RE: Honey comb modeling

(OP)
ok, i dnt understand where i could have gone wrong, this is what i have done:
        i have modeled the top face of the skin and have defined 2 materials. one for the facing and the other for the core. and in property i have used laminate and have defined isotropic for the facings and have defined laminate-2d orthotropic for the core. here i have given a small value for E1 and E2 to prevent numerical singularity while i have given the L direction and W direction shear modulus.I have simulated the simply supported beam problem which is there in the hexcel website. But the deflection from fem seem to be nowhere near the theoretical solution.like fem gives 0.0184m while theory gives 0.04m
could u please tell me where i have gone wrong.
the hexcel link for the problem is:
http://www.formulaschools.com/curriculum/7586+HexWeb+Sand+Design.pdf

RE: Honey comb modeling

The difference is probably due to a) boundary conditions, b) loads, c) mesh size.  FE models are often too stiff.  Please describe how you applied the boundary conditions and loads.  Also, how many elements are in your model?  Did you assign the L and W shear moduli to G1z and G2z?

RE: Honey comb modeling

(OP)
i got it to work. i actually had overconstrained the model and i constrained it in the right way later. it matches well wth the theoretical result. Thanks. Is there an example of composite laminate modeling. if there is could u send me the link. Thanks.

RE: Honey comb modeling

  Dear SWComposites, Gbor (sorry don't know your names) and all who shared knowledge in this topic - thank you very much for your patience.
 What you're discussed here was something I was looking for long time and could not find. My problem is that at my time I had no possibility to go to university so my math base is very poor if non existent. Also language limitations don’t help much. But enough of excuses (here we have a joke about bad dancer and balls that hinder him - it might well be international). How ever I'm determinant (i.e. persistent as a donkey) to learn.
 So would someone rise to challenge and summarize what was discussed here? That would make an invaluable source for many IMHO.
 So to model a sandwich structure in NASTRAN (it will apply for most other FEA solvers).
 What is proper way to define material for lamina plies?
1)2D orthotropic
2)3D orthotropic
I was thinking that 3D orthotropic because in case of non unidirectional fabric we may have different Ex,Ey,Ez etc.
(Note that 3D properties data is rarely available from manufacturers. I guess that there's some way to calculate 3D data from 2D? If so than it will be nice to learn how.
 What is the proper way to define material for core material?
 1) Foam
 2) honeycomb (alu, nomex)
 
 What would be the best choice of elements for complex 3D sandwich structure? I'm very new to NASTRAN? In ANSYS one would simply choose shell91 (composite) with sandwich option and assign material_1 (carbon/epoxy) with appropriate orientation and thickness for face laminates and material_2 (core) for mid layer. My stupidity prevented me from being able to define core material properly as usually only compression modulus
                          Compression strength
                          G13
                          G23
And ANSYS requires full set(9) for E,G and Nu.

 What would be best approach to model complex sandwich structure from geometric point?
 Import it as surfaces and than mesh it with shell elements?
 SWComposites, you mentioned "If you are using 3D solid elements (where the skins and core could be modeled with separate elements) then the full 3D set of properties is required."
 Would you (please! please!) explain a bit more thoroughly how one should do it - from geometry till meshing and material.

 I'm not asking about modeling hard points, bolted and adhesive joints etc. as this is out of topic or is it? ;)

 If there are some dumb mistakes in this post please excuse and correct me.

Kotawsu – would you please share how you finally modeled your case and it correlated well with theoretical results?

 Thank you all so much!
 Adrian  


 




 

RE: Honey comb modeling

(OP)
if i have the midsurface can i still use pcomp method to idelaise a sandwich panel or should i use pshell method.and if i have to use pshell method do i have to give only the facing thickness as the Taverage. thanks.

RE: Honey comb modeling

I have modeled Aramid honeycomb core with solid elements (CHEXA) using anisotropic material cards (MAT9).  I specified appropriate values for G33 (Ezz), G55 (Gyz), and G66 (Gzx), and entered small values for G11 (Exx), G22 (Eyy), and G44 (Gxy).  Please make sure that the material orientation is correct for the solids and plate elements, and the same for all the elements.

RE: Honey comb modeling

Tstanley,
 Thanks for the link!

RE: Honey comb modeling

(OP)
how do we go about modeling a complicated honeycomb design using pcomp.suppose there are multiple parts connected to one another . do we have to assign local orientation to see that the face of each part falls on the x-y plane.

RE: Honey comb modeling

Non planar surfaces are approximated as small planes.  The important thing is to make sure the material direction is correct.  In FEMAP, read the help section for "Modify, Update Elements, Material Angle."  You can view the material angle using view/options; labels, entities and colors; element - orientation/shape.  To see the material angle for 3-d elements, you have to turn off hidden line.  

You can update the material angle for a group of elements using modify / update / material angle.  I don't recall if this works for 3-d elements.  

To get the x/y/z stresses/strains to come out in the right planes, you may have to modify the element orientation.  Just remember to update the material angle after any modifications to the element orientation since the angle is relative to sides one/two of the element.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


Resources

eBook - The Future of Product Development is Here
Looking to make the design and manufacturing of your products more agile? For engineering and manufacturing organizations, the need for digital transformation of product development processes just became more urgent than ever so we wanted to share an eBook that will help you build a practical roadmap for your journey. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close