Discussion Forum

Hi

unfortunately I cannot see your image (normally you can attach jpg files or png files easily to the forum sections, its better than having ecxternal links that dissapear after some time

for me if you make a very long beam, and segment it in smaller parts then you should have a continuity link at the interfaces and they will tip over, one linked to the other, see the lare displacement example of the doc (at leas in 3.5 ;)

--
Good luck
Ivar

Hi

I finally got to the file (have addd it via "snippit" to this reply)

What I do not understand is the way you expect to get the beams to bend by shortening the right vertical side ?

If you say you have two strait horizontal beams and then weld them onto the long one to the left and the shorter one on the right you stress the beams, and all will deform.

You can do this via a few "tricks" such as (traditionally) use a temperature dependace with a anistropic thermperature expansion coefficient on the right vertical beqam, starting with two equally long vertical beams

Or via the contact physics (could be tricky to get to converge) by appying a force to get the beams to the right to come in contact.

or set up the equations to run an optimsation such that the distance of the two beams (if you connect the four over common borders except for the last region) tend to "0"

--
Good luck
Ivar

Hi Ivar,

Thanks for the reply,

Hopefully i can be more clear now as i have the full model done, I'm actually trying to optimize a 'Butterfly' MEMS coupling spring, and have therefore parametrized certain parts of the structure.

I wasn't try to move either beam by some force, what i was trying to illustrate was that i can't seem to get two beams to be fixed to each other and when one beams length is increased (creating a new model) this causes the other to alter its shape in accordance.

For example in the picture attached, I have the whole coupling spring structure. Now for example I have on parameterized beam "Truss Beam 1" in which i can alter its length, either increase or decrease.

Now truss beam 1 is attached to the outer flexure beam 1 at its top. If i increase the truss beam length upwards, I want the outer flexure beam end point to still be attached to the truss beam, as in the bottom picture.

Now this obviously results in the outer flexure beam changing its length and angle.

Currently if i change the truss length, i have to change the outer flexure beam length and angle automatically.

If i don't then it basically looks like the picture i gave in the first post where the flexure beam remains the same, while the new longer truss beam pokes out above, as in the second part of the first picture in my first post :)

Is there any way to clamp various points, in my case the beam end points together?

Regards Mike F

Hi

Now I believe I catch better what you are looking for, the issue is then how to make a clean geometry (as you start with a model without stress, deformations is second step).

Well I would have done it in SolidWorks CAD (parametrised via the "Equations") and linked it via Livelink (in V4) such that I could rerun the hole with the new geometry.

In 3.5 one could try to make the geoemtry via matlab, should work but is (in my view) far more tedious. Then not to forget to make an union or composite entity, and remove unwanted internal boundaries.

One trick if you work with very different thickness of beams and fixed regions (not really your case just there) I mostly split my thin beams in the middle to force a more detailed mesh and at least two elements per beam width, and I cut the beam with an interiour boundary slightly inside the fixed side, such to force high mesh density at the attachments.

Anyhow you have the issue of stress concetration (numerical as well as real) with right edge flexure beams particular of mems size items (if you use wet-etching or other techniques) here its difficult to be fully representative

--
Good luck
Ivar

Hi,

Yes, at the moment it is just a static model, what i want to do is perform stress analysis on the model, by applying a force at the top, not sure what to use though, point or edge force.

This is all part of an optimization routine, so at best all i would like to do is simply pass a 'parameter' array of values which change the default shape, and then perform stress analysis.

My objectives are to simply have the spring match a certain stiffness value (X direction) and to reduce stress in the model.

Also as a constraint to make sure no stress point exceeds the maximum of polysilicon, (which btw I'm not sure what it actually is :D ).

I have built the model in a separate analysis tool SUGAR, which is a MEMS Nodal simulator, attached as a picture. This model being Nodal, and hence works by connecting beam end points does allow my the functionality of simply altering the truss beam length and then it automatically corrects the length of the outer flexure.

I just wish there was a way to do it in COMSOL.

I'm new to this side of modeling and analysis, so it can be a bit dangerous for me in making sure I'm doing everything as correctly as possible,

For example what is the best method for analysing stress of the spring model, do I have to anchor some points to the 'floor' at the moment i have 4 anchors but they don't do anything, also do you think it matters if I have no boundaries, as it is only stress analysis.

How important is it to break up long 'beams' into sections or not?

Also do you know of a method to work out stiffness, I believe i can work it out analytically by using the displacement and the input Force but I'm not sure.

Kind Regards Mike F

Well, I think i managed to get something working :D

This is a displacement of the spring of -100 N along y axis, using a coarse mesh.

For some reason in COMSOL it shows up wrong, the only colours are dark blue over the top plane, and then the maximum stress red along the side plane as somewhat shown in the attached picture.

Still exporting it seems to give the correct von mises stress picture, i hope :).

Regards Mike

Hi

a few comments:

1) with respect to stress, do expect very high values in the corners where you have stress concetration, there you would probably also get numerical issues so one can never 100% trust thos values, very locally. You can still plot the overall stress distribution by detecting these spikes and clip the color range. But still, what is the true value in these corner ? >>1GPa is not really survivable for your system, be aware.
Your issue with the colors could be, try a 3D plot and see if you do not have somevery "high" spikes (orders of magnitude" then tweak the color range.

2) In general try to avoid point loads, in 2D it corresponds to edge loads so could be considered, but the best is surface loads over at least a few elements (but you need to normalise your force to pressure over the load surface (can be done internally by the load options in V4, must be done manually ie.e integration coupling variables in v3.5a

3) check carefully your meshing, in V4 you can run your model with a parameter to increase the meshing, run for n, 2*n 4*n anf if possible 8*n elements just to see the sensitivity of your model to the expected results (again singular points may give you some surprises, think over what kin of criteria to use, displacement, stress, total energy ...

4) I normally say 3-4 elements across a beam as absolute minimum, therefore often starting in 2D helps to set up the model because its so much faster, using symmetry is also a nice way around, but note that for eigenmodes you must combine symmetric and antisymmetric BC's to get all modes out, and often the loads you apply are not really symmetric, hence you must use the full model.

Unfortunately COMSOL V4 does not (yet ?) have the facility to make mesh mirroring i.e. you have a symmetric geometry defined, you mesh only 1/2 or 1/4 or even less and then ask the mesher to distribute the mesh symmetrically on the rest of the geometry.
You could ask why, but often for complex geometries you have to do a lot of mesh fiddeling, it divides the work by 2, 4 8 or even more, this is important when you need to sell the purchase and mainetnance costs of a software to your boss, and then when you want to do very precise analysis (opto-mechanics or interferometry) the assymetric meshing you get by full "free-mesh" is enough to give large errors compared to the scale you are looking for, all this is probably not fully relevant for you as is, but if you go into opto-mems it will be.

5) check your forces, take the reaction forces on the fixed points and compare them to the load forces should be the same.
This is another slight weakness in COMSOL structural, it does NOT propose any simple validation/verification scripts, such as comparing the reaction forces to external forces, the total stress energy to the input energy ... But I'm sure these things will come, one could imagine a series of scripts to do this. Typically a good "student job" unfortunately I have none at hand ;)

--
Good luck
Ivar

Hi Ivar,

Once again thanks for the comments.

I thought i should give some background on what I'm trying to do. I'm a PhD student, shocking I know, and I mainly work on the design and optimisation of MEMS. Now from my understanding MEMS design and it's optimisation is 'generally' of a build and break iterative, a designer builds the device tests it to oblivion and then redesigns it. With the advent of COMSOL and other FEA / Solid modeling tools, this has somewhat migrated to building and evolving designs using these tools + (Analytical models). Now this is still time consuming to do, and optimisation by hand or somewhat better using gradient based local search optimisation techniques isn't always the best approach due to the non-linear relationship of design variables to device response. Also from what I understand there is really no general methodology towards MEMS design, some designers solely use FEA tools, others use analytical models, others perhaps lumped circuit models or perhaps a combination but it is to me still unclear.

So this is where i come in :), To begin with I've taken an decomposition created by a man named Senturia for MEMS design, which looks at the whole process and breaks it down into a set of hierarchical levels, these being System, Device, Physical and Process. The system level deals with generally the circuitry and therefore utilizes lumped circuit models or block diagrams for its design. The device level is generally an abstract representation of the MEMS device, either through the use of Nodal 2.5D simulators such as SUGAR, or analytical models. The physical level uses FEA and BEA tools such as COMSOL or ANSYS to design the solid 3D model of the device. The process level deals with the design of process and fabrication and as such I ignore in terms of design optimisation.

Now what I'm trying to do is see whether it is beneficial to link the various levels together in what can be called a Multi-Level approach, for improved design optimisation. For example an analytical model is orders of magnitude faster then a representative FEA model, and perhaps it might be better to evolve new designs using the analytical model first before passes good designs up to FEA analysis, thus reducing computation time spent on poor designs. Also perhaps you would like to perform some Shape optimisation, something which can't be done on an analytical model generally. This is an example of a Device - Physical coupling.

Now currently I have been working on the design optimisation of a MEMS bandpass filter, which consists of joining / coupling together a number of folded flexure resonators using a 'coupling spring. This work, as shown in the attached paper uses an equivalent lumped circuit model of a bandpass filter, (Spring Mass system - RCL Tank) which is design to match a certain filter response. I can then extract the values for good filter designs and convert them into target values of 'Mass' and Stiffness and then look to evolve a simple 2.5D SUGAR Nodal model to match my mass and stiffness target values. This is basically a System - Device coupling.

Now I wanted to move into some Physical design optimisation so considering in the last example I actually did not design the coupling springs, I though I could do it here. For this all I need to do is really design the coupling spring to match a certain stiffness value (Taken from the previous circuit model and converted). I also thought it best to utilise something only COMSOL or FEA tools could do which is perform stress analysis.

So using a supplied Force I can then compute the stress and stiffness and hopefully evolve the design to match my targets / reduce stress.

Can I ask for your opinion, I'm not sure how much you work with MEMS, probably a darn sight more then I do :D.

Also on a side note, one of my objectives as I said before was to also optimise design to reduce the stress levels within the spring. I originally thought that this design would give stress levels close to that of the maximum load for polysilicon, however if it is 1000MPa, then it seems to be nowhere close (I get 17MPa), which kind of makes the objective redundant.

2) With regards to your second point, what do you feel would best represent a force applied to the coupling spring from one of the coupled resonators, currently I'm just putting a face load across the top anchored beam of -100 N (Which is probably way to large for my resonator displacement) along the Y axis.

3) Meshing is an interesting issue for me, you see my work looks at multi-level design, one approach is to optimise two sets of design using two different optimisers with differant levels of evaluation / accuracy, so for example I have one coarse mesh which takes 5 seconds to analyse and one highly dense mesh which takes 30 seconds to analyse. Naturally you hope the higher density mesh is more accurate, however it has a computational cost. So what you might look to do is evolve new designs at the course model level, and then on occasion pass good designs for evaluation at the higher level, this is of course a crude explanation :D .

4) Funnily enough I'm not to bothered about speed, as long as I have one fast but inaccurate and one slow and accurate model I will be happy.

5) How exactly do you check the forces?

Thanks for the help, and sorry for giving you a tome to read

Kind Regards Mike F

Hi again

Nothing shocking about doing a PhD, I know others having spent ages on that, OK for me its gettig rather a long time ago ;)
You have attacked an very interesting approach there, I agree MEMS design is (like meshing) for me an "art" before a science you need quite some experience, and in many domains with tests and failures, but often too success.
I have been working with flexures for soon 25 years, mainly by analytical means for gross dimensioning, simple numerical and then FEM for last (almost final) models, with COMSOL and a good CAD tool I can make 10 models in the time of 1 from our previous software (and a decade ago) which helps for the experiment domain you can cover. But in our team we still have a good "analyst" because he can sort out concepts much quicker than only via numerical methods. Then if these are for MEMS concepts (we still do many thing flexures / compliant mechanisms in classical fine-mechanics and metal) you need the good, experienced "Silicon chemists". Personally I like wet etching for "mechanical parts", it's more limited in shapes, and you need technology tricks to avoid stress concetrations but you can get cleaner items, DRIE allows you about any shape, but no perfect parallelism. Anyhow very thin features have a stiffness issue in the out of plane direction, not obvious how to get around. Perhaps that's why its fun. My first scan of your article, reminds me about the time we did most mechanical via electric equivalence, but also some of the optimisation approaches used for optical thin film design (stack of dielectrcs and sometimes metals to get a given reflectance, transmission and polarisation dependence).
I believe you could do/port most of it fully in COMSOL, you have the matrix handling, the PDE and the optimsation included, no ?

Back to Si failure in MEMS, I believe its mostly happening due to stress concetration designs, and to technology issues, such as the generation of small spikes (typically in wet etching) or fracture initiating not passivated well enough (typically resulting from the DRIE) and a crystal (such as Si) has no fracture stopping elements such as material grains in metal. I believe only micro-spot X ray spectroscopy can show you truely the culprits, but experience is another way to avoid them (as you say build and brake ;)

2) For me forces (or fixations) should apply to surfaces of several mesh elements sizes. Applying 1 or 100 N in a linear analysis doesnt really matter (apart if its to get out of numerically small issues). For large deformation approaches it's aquestion of convergence and time to wait.

3) for you I believe you must also use some sort of gradient steepness criteria too, just the coarse or fine mesh is not enough, as you can get numerical run-offs on a few points that might guide ou away from interesting optimums. Perhaps some tests when taking out the n highest and lowest values could be a way (to be tested carefully). It's slightly too quick just to say higer mesh density is better, even if I agree it mostly is.

4) that depends on the level of "super cluster" you have to play with I agree, I have to stay within the RAM of my single workstation (but its a rather new good one ;) Now analytical approaches such as MapleSim or Modelica can be quicker and give some interesting trends to use further for detailed FEM, how to link it into your case is not obvious.

5) I usually say 5-10% is "good" (for force balance, as well as for maximum model values change for impoved meshing density limits). But for i.e. optomechanical designs, such as for astronomy adaptive optics you need several orders of magnitude better, which remains for me, outside of numerical FEM modelling reach, today.
And still, you can get very interesting information on how you should go about your design with the FEM, and then you must "try" as in real life there are many items that is not in our models. For MEMS typically the thin film damping effects can often be to our benefice, by damping several parasitic structural modes, while contact and "sticking" not yet well modelled can be fatal for the functionality.

My PhD time was when I started to learn "systems engineering" it looks like your in the middle of that just there

--
Good luck and have fun Comsoling
Ivar

Hi Ivar,

2) Does the level of Force (1 - 100 N) really no matter?, I believe for calculating stiffness it doesn't because it is simply a function of displacement and force, though i could be wrong, however when looking at stress levels, a greater force will give a larger displacement which itself will lead to increased stress.

3) I won't be using any gradient based local search optimization techniques, but rather a population based stochastic approach called Evolutionary Algorithms, more specifically multi-objective genetic algorithms, so hopefully the approach will handle the problem as it does not use gradients of any kind to improve the design.

4) Ahh, I should have said that I as well am stuck using my local computer, with only 4gb and windows vista, so far the coupling spring calculations require about 1gb of RAM to run, though I don't think I used the highest density mesh so it could be a problem :).

5) For me I can't actually fabricate any of the designed devices so in this case it is one of many limitations, I would like to but its a no go.

Kind Regards Mike F

Hi

What I was saying is that if you apply 1N you have the displacements and stress level aready scaled "per 1N applied force". If you use 100[N] you must divide by 100 and multiply by the force in N you want to compare to.
This is if you are in linear (small deformation mode).
If you turn on large deformation (non-linear analysis) it's easier to analyse by running a parametric sweep with several force values between 1 to 100[N] (or whatever reasonable min/max load forces you expect to have) then you can better see when (if present) the non linear behaviour becomes dominant. An to decide if te time consuming non-linear calculations are worth it

4GB is already interesting, by using symmetry you could even gain RAM versus mesh density ratio too, it's a good starting point. Running 2D could also help, at least to begin with.

If you have no way to build anything, I would say that finding some similar structures in the litterature with measured stiffness, forces and general beahviour are already a good starting point. Not taking some time to calibrate (or at least attempt to, as often in articles you lack the full information so you might need to do some hypothesis) is in my view not a professional approach. Because it's so easy to get nice but unrealisitc results. Even a few analytical points in the experience space is better than blind trusting your FEM results

--
Good luck
Ivar

Hi Ivar,

I agree that it seems to be the best approach to validate the FEA with some kind of analytical model, sadly I don't have nor know how to make one for this spring. It is basically a copy of one from the literature, paper attached.

I will probably have designs which take as input different force levels N, as the spring will be essentially coupled to a folded flexure resonator, and I imagine its stiffness and input force will have an effect on the force applied to the spring.

Will this be really a bad thing?, if I have one design and apply one two differant sets of force N, I imagine the springs stiffness will remain the same, but the stress over the spring will be different, logically higher over the spring which has a larger force applied to it.

Regards Mike F

Hi
If you are in a linear regime (typically no stress stiffening, "low" stress and small displacements) you should expet little/negligible effects on spring constants versus load, then its a question how the springs are linked together, forces remain.

But you should have clearly in mind the differences and relations between strength, strain, stress, and stiffness (all the ones with s').

These topics are typically well covered in the bookson "compliant mechanisms or on Flexures"

stress and strain are related to the young modulus (that might be non linear related back to the total stress present), and stiffness is related to the young modulus and the inertia (a geometrical property that can again be influenced by the total integrated strain = deflection).
While strength if finally a meaterial property, specifying the stress compliance before failure (up t you to define "failure" linked to your limit of resilience or toughness) ...

--
Good luck
Ivar