Can a composite panel be modeled in SAP2000??

[aubrey7978]

Hello to all experts out there,

i understand that SAP2000 is a non-composite modeling software. I'm currently trying to model a sandwich panel in SAP2000. To model as a single material panel, i found an equivalent young's modulus using EI (flexural rigidity) so as to model the flexural behaviour of the panel only. However, in doing this i'm assuming the axial stress to be negligible which in actual fact not true. Because of this problem, the stress given by SAP2000 will no longer be reliable, am i right?

So my question .... is there a way to go around this problem, maybe playing around with the input parameters so as to separate the axial and bending stresses or some other solutions?

thanks a million in advance.....

aubrey

 

[Qshake]

I would not use SAP to model a composite material application. I would only use SAP if the subject panel were, in fact, a rigid diaphragm in a structural frame application.

 

Instead on 1 equivalent property, you have the option to define each section of the panel separately and rigidly link them together with Joint > constraints > Rigid body type

 

[aubrey7978]

thanks for the reply,

could you kindly elaborate on how to link the separate panels one on top of the other? seems to me SAP2000 allow me to specify a shell at one spatial location only (by specifying a shell element by clicking on the grid), pls correct me if i'm wrong.

thank you once again.....

aubrey

 

You link them at joint locations using Assign > Joint >constraint. Double click the grid to add new planes/gridlines in any direction.

Keep in mind the thickness assigned to your shell elements when creating new gridlines and drawing new shells since you're working on centerline.

For example, if you had a 2 foot thick plate on top of a 1 foot thick plate, you would need to draw the shell elements 1.5 feet away from each other. Must constrain 1 pair of joints at a time using Rigid body type constraint.

I find using the Extruded view (use the 'Set Elements' icon) is useful when visually checking my models when drawing shells sandwiched together

 

[aubrey7978]

thank you very much barefoot_hillbilly,

one more question, u mentioned using rigid body type constraint, which kind of constraint are u recommending, for instance, Equal, Body constraint etc? How to ensure debonding does not occur at other regions of the panel besides the nodes?

really appreciate ur wonderful help rendered. million thanks again....

regards
aubrey

 

From what you have described, sounds like Constraint >Add Body type, in which constrained joints are connected to each other by rigid links.

You want to make sure your shells that are to be bonded together have meshes which are as identical as is reasonably possible. Assign constraints to "corresponding" joints where it makes sense to rigidly link them...not unusual to have many Body type constraints in 1 model. Use Edit/Mesh shells to modify shell meshes.

Example - if you had separate horizontal layers(shells) of a composite material stacked vertically on top of each other, you would want to apply same Body constraint name to joints which have same approximate X,Y coordinates at different Z elevations. Same Rigid Body name can be applied to several joints, usually to a corresponding joint in each layer.

Use animated deflection graphics and Select >Constraints to visually check whether you have constrained joints as intended

 

[aubrey7978]

thanks barefoot_hillbilly

i have tried modeling it with various mesh intensity. for a panel of 1m by 2.15m, i used a 8x8 mesh. the strain calculated at the interface of the sandwich panel still differed by about 50% (but has improved quite a lot compared to a 4x6 mesh initially). Actually did the same way as u mentioned above, but to assign the constraints seemed kinda tedious for the 8x8 one already.

anyway, million thanks for the help, it is truly a boost to my project.

 

Last comment/suggestions, since you mentioned possible strain error. Assuming you want both in-plane and out of plane stiffness in your shell elements, check to make sure the Shell section is "Shell" type, not membrane or plate.

Use rectangular elements whenever possible, avoiding the use of quadrilaterals of arbitrary shape which are less accurate.

Don't overlook the mesh by gridlines and mesh by points on edges options. If meshing by gridlines, it makes it easier to constrain joints.

Good luck

 

[aubrey7978]

hi Barefoot_hillbilly,

just pondering if, say a pressure load, acting on one surface of the composite panel, is it true that only the first layer (the layer on the side where the load is acting) is resisting the load and not all 3 layers? pls correct me if im wrong, cos constraint only causes the subsequent 2 layers to take a deformation similar to the first layer(to act as a rigid body), and it does not transfer the force to the other 2 layers. im afraid that the displacement given will be larger than what it actually should be.

pardon me asking, is there a way that i can verify this approach, or do u know of any journals that i can compare results with?

hope that u will see my question.......and appreciate if u could reply again. thank you very very much!

 

Not true. Using rigid "Body" type constraint, displacements are related, but not necessarily identical. If they are rigidly linked, all 3 layers should be resisting load, not just 1st layer.

Think of rigid Body constraint as similar to linking joints using a very stiff beam with zero weight and zero mass...but without the numerical instabilities introduced by using such a beam. SAP Body constraint, in my opinion, is a very useful feature within SAP.

Try this - Draw 2 joints (Draw > Special joint) in space by themselves 5 ft. away from each other in the X direction - doesn't matter whether they have same Z elevation or not. Constrain them together using Body type. Add very stiff springs (Assign>Joint>springs)something like 1E+8 in all 6 DOF to only one of the joints ...you cannot have a restraint and a constraint on the same joint. On the same joint with the springs, assign a joint load displacement rotation - rotating it about the Z axis some amount, say 15.

After analysis, note that the other joint has not only a rotation, but translational displacement as well - displacements of the two joints are related, but different.

Run your own benchmarks comparing Body constraint to results using a dummy beam with a user defined material with high stiffness, zero weight.

Not sure if there are any theoretical comparisons or not.

CSI used to sell a very good book by Ed Wilson, one of their chief consultants, which explains theoretical background and techniques used in SAP. I think it's called '3 dimensional analysis of structures', or a similar name.

 

[aubrey7978]

thank you very much once again,

will try out what u have said and also some other benchmarks to verify this.

regarding the book by Ed Wilson, heard that it is very good too but could not get it from the library in my college. Think the website

http://www.csiberkeley.com

only has excerpts of it. anyway will try the method in SAP2000 first.

thanks again and happy new year to you.

 

[aubrey7978]

sorry hillbilly,

tried out the method and compared with some results calculated from formulae in J.M. Davies' book -'Lightweight sandwich construction'. Seems like there is a optimal mesh density, cos if i use a denser mesh, the displacement became < actual displacement calculated. would a denser mesh make the panel stiffer? should not it be the denser the mesh, the more accurate the answer?

pls advice and million thanks to u again. sorry for the trouble.

 

[aubrey7978]

Hi Hillbilly,

pardon me for imposing on u again, but seems like u r the only one that i can turn to. Really hope u can reply to my thread...thks.

regarding the method u taught me, i'm kinda facing some problem. using the constraint method, seems like i can't get the model to converge, as in can't perform a convergence study on the model since as i make the mesh denser (with constraints applied to all new nodes as well), the whole panel will become stiffer correspondingly, and the difference between the current model (by doubling the mesh density) and that with previous mesh density isn't negligible.

also, i plotted the stress profile across the centreline of the panel, where the panel is a square one with uniform pressure applied. Boundary conditions all pinned at 4 sides. however, i got a stress profile not parabola, but one which is quite 'wrinkled' and the stress aren't zero at the edges.

Apologize for posting such a long thread....eagerly waiting for ur reply and thanks a million. Really hope that i still can use this constraint approach.

 

Aubrey, not sure why your model would not converge - what error message does SAP give? Also, sounds a little fishy, although plausible, that your model became 'significantly' stiffer with finer mesh.

Careful to make sure the joints you constrain together make sense. don't constrain joints together which are in the same plane, for example, if you are modeling a sandwich panel in which each shell/plane has different properties. Constraining joints in the same plane would definitely stiffen your model.

 

[aubrey7978]

donno did i understand ur advice correctly. in my model, there are 3 layers/plane with all different properties but with same dimensions. within each layer/plane, same properties were used throughout. i meshed all 3 planes to the same density. in each of my body constraint, i have 3 nodes which are all on different planes/layers. i dun constrain nodes that are on the same layer. because of this, i ended up with hundreds of body constraints.

Do u think im doing it the correct way? hope you will give me some advice and shed some light if i'm on the wrong track.

thanks billy.

 

If you have 3 layers, all same mesh and same dimensions, each constraint should be assigned to 3 joints, 1 joint on each plane. if this is what you did, you're doing it correctly. With a fine mesh on your panels, it's expected to have many constraints. But with so many constraints, there is a possibility of error in assigning.

You can do a quick visual check by using Select menu>constraints, then try View menu>show selection only. Make sure you haven't assigned multiple constraints to any of the joints. Right mouse click on joints is another way to check if multiple constraints were assigned to a joint. If you verify that constraints were assigned as intended, i'm out of advice -it should work as composite behavior. Also, check to make sure your shell sections were shell type and not membrane or plate if that is your intention.

You can always email your .sdb file to CSI for tech assistance. good luck