Discussion Forum

Hello

For the anisotropy of Silicon you need to define for your volume/subdomain Material properties:
Model properties: Anisotropic
and then fill in the D Elasticity matrix, at least the essential Dij (D11, D12, D33) elements and then apply Si lattice symmetry rules (depending on the litteature you have: D11 around 169, D12 around 65 and D33 around 80[GPa]). This is for <100> along x, <010> along y and <001> along z. If you have the material library there are a few examples there too

Then you need to define your coordinate system: "Options - Coordinate systems New ...", I end up using often the "General" tab and define the new x',y',z' w.r.t the original x,y,z. Unfortunately COMSOL does not show the new coordinate system, so I use the trick to apply a Force load on a point and select the new coordinate system, and then check systematically the direction of Fx, Fy Fz w.r.t. the new coordinate system, by using the "show" bundary load option (do not forget to remove the load when you have finished).

For the bending moment you need a little "trick", the best i to study and reproduce the example in the doc:

EXAMPLE: TORSIONAL MOMENT ON A CYLINDER page 69 § Loads of the SMEUG.pdf (SME User Guide)

Good luck
Ivar

Thank you for your kind reply

I found that we can choose <110>axis in the material library for the case of Silicon in the column Oritation/Condition.

Whether there is direct method to assign the direction (coordination system) according to this <110> axis. And whether the material properties are anisotropic automatically changed according our setting.

Best wishes.

Hi

Well pls check carefully how you work and the results, as the Silicon in the specific orientation is valid for an isotropic analysis, if you select anisotropic the data is NOT highlighted hence you have default steel (if you havnt loaded something else before).

The library is very good and handy, but I alsways cross check, and if you want correctly to model crystalline materials, you really need to take care that the orientations correspond.

I.E: if you start to simulate piezo materials, do not forget that the convetion for the stress tensor and Young modulus tensor follows a different order than the classical structural method. There are good reasons, but it's often a headache for the user to get it 100% right

Good luck
Ivar

Thank you very much.

You means we can't use the material library orientation for anistropic crystal and the properties will not change correspondingly?

So, how to choose the material library and set the coordination system to realise the anisotropic (as well, in my case the cross section of the single crystal beam is triangle and there are different directions ).

In fact, the material library is very useful. As well, to set the elasticity matrix seems complex and less accurate.

Thanks again for your kind reply.

Hi

No I did not say you cant use the material library.

Yes you can, definitively.

But you must understand what it is updating in the material selection you have made, they might not match, or the number of DoF (degrees of freed) do not match. And is the material data depending on "T" and "p" and have you defined these ? etc.

If you select anisotropy, because you are working in true 2D or 3D then I would uggest to use the crystalline Si.

0) you create or import your geometry, how it seems logical for you,
1) select your material, select anistropic,
2) and then go into the Mat library, select MEMS and Semicnductor then "Silicon (single-crystal)" (by the way it does not show up in the "search" list that seems to be limited to the main library, hadnt noticed that before)
3) OK (Then you can take a look at the "D" tensor)
5 you create a (or several) local coordinate aligned x' == <100>, y'==<010> and z'==<001>, i.e. by using coordinates, or rotations of the defult one, or edges or a workplane to align it
6) you go to the subdomain material tab and you select the coordinate system that applies for the diffeent Si domains

Then you cross check the values, the easiest is probably to do a quick modal analysis an compare the first beam modes with hand calcualted values, you might also visualise the coordinate system by applying a temprary load to a point and define it in the different coordiante system directions, turn ON the "Options - show symbols" to visualise, and do not forget to remove the load thereafter ;)

On thing to know is that the E10=E01 is around 130GPa, the E11 around 169GPa and that if you are in the perpendicular plane to <001>==z then your approximate bulk modulus can be expressed in cylindrical coordinates theta-z as E_theta[gPA]=130/(1-0.23*(sin(2*theta))^2), it makes a nice polar plot, and the anisotropic factor in the <001> plane is quite large, see attachment (scaled by 100GPa).

Good luck
Ivar

Thank you very much for you kind reply.

I already assign the anisotropic silicon to the beam.

For the bending moment on the beam both side surface(both cross sections are triangle), I still don't clear how to assign the bending moment according the reference (EXAMPLE:TORSIONAL MOMENT ON A CYLINDER).

Since the profile of the stress on the beam is not asymmetry. As well, the stress distribution is complex due to the anisotropic beam. Is there any method to assign bending moment to this beam. In fact, I want to get the stress distribution from this simulation and check how large bending will make this silicon beam break down.

Thank you very much.

Hi,

indeed bending moments are more trickier, probably that is why they are not implemented as such in COMSOL, they are less generalised and as they depend on a point / axis, not conceptually so simple.

but if you have a bending moment to apply to a surface/boundary (assumed x,y) you need "only" to distribute the local pressure:

p(x,y)[N/m^2]=F(x,y)[N]/(dx[m]*dy[m]) correctly, as COMSOL works with pressure for the dependent variable.

If you are in 2D you can drop the "y" and replace it by the normalised depth y=dy=1[m] and correct the units correspondingly, or in axisymmetry replace x=2*pi*r the loop length

The crude way is to apply edge forces and have the material stiffness to mean out the moment over the adjacent surface/boundary, with the drawback of stress concentrations, and some imperfections therearound.

If you have a constrained surface you can define an axis and a cylindrical coordinate along this axis, and develop the pressure over the boundary w.r.t this cylindrical coordinate (i.e. the "torsional" example adapted to your case)

The last I can think of is something we made/build actually some years ago, by adding some "rigid" structure with a shape such that you apply a pure force on this new part to obtain a bending moment on the item of interest, but this is not the way I would start in COMSOL.

A variant but same principle of the doc torsional example is to link the surface where to apply the moment to a point in space and apply a force on this point related to the moment (and its centre/axis of rotation). The point must be linked through "RBE" Rigid Body Elements (for NASTRAN or ANSYS fans) to the surface. COMSOLs way is to use the weak form, but you must write your equations yourself. The trick is to not influence the stiffness of the structure to study, just add a pure pressure gradient. This is also a subject I would like to put up on the model library, have bits and pieces somewhere, but I do really not have time enough.

Hope this helps
Good luck
Ivar