Terribly slow computation time for silicon microstructures... 1

[jongyonkim]

Hi, I'm using ABAQUS/Explicit to simulate stretching of a silicon coil that measures 2um~200um (micron) for my lab.

I made the structure with part size "200" for 200um, which translates to 1 unit = 10^(-6)m. I also made appropriate scaling to density and Young's Modulus.

Density : 2.329E3 kg/m^3 -> 2.329E-15 units
Young's Modulus : 1.124E11 Pa -> 1.124E5 units

The computation time turned out to be absurdly slow (Time/LPF Inc is around 10^(-10), which takes "weeks"). My computer has dual 3.2Ghz processors with 2GB RAM, which is sufficient to run ABAQUS.

Has anyone tried running micron-scale simulations with success? Can ABAQUS run such a small-scale simulation in a reasonable time frame (~hours)? If so, what may I be doing wrong? If not, what other FEA tools do you recommend?

Thank you.

 

[bassmanjax]

Hi

Have you tried using mass scaling?

Martin

 

[jongyonkim]

Hi Martin,

My step has this mass scaling option as default ("Use scaled mass and 'throughout step' definitions from the pervious step"). What does this mean, and how can I go about using mass scaling to improve computation time?

Are there any other techniques I should be aware of / can use? I'm new to ABAQUS, and I've only done the tutorial.

Thanks.

 

[bassmanjax]

Hi

Mass scaling can be used to reduce the increment of time required. Basically, the minimum time increment is controlled by the smallest element size and the material density. As you generally don't want to change the mesh, by artificially increasing the model density with mass scaling, you can increase the minimum time increment and thus reduce the solution time.

I tend to do forming analyses where I use *VARIABLE MASS SCALING with the TYPE=BELOW MIN and DT cards set as appropriate. The increase in mass is shown in the .sta file during the analysis - be careful that the increase in mass isn't too great though, or your results will be invalid.

The other way to reduce the solution time is to reduce the step time. You may find that you can safely decrease the total step time without invalidating the results. Most of my forming analyses are run over 0.01 sec with no problems.

Martin

 

[xerf]

I have been running micron size models with ABAQUS/Standard, with the dimensions scaled to (mm).

I am not sure about you scaling, but in general I avoid putting numbers of order of (10^-15) in my models.

(I might be wrong about this, but it seems to me that your lenghts are in microns, while the Young's modulus is in N/(mm^2), also for the density -> 1(m^3)=10^18(micron^3).)

 

[jongyonkim]

I think this is primarity a scaling issue. If I just assume SI units (thereby making a 200um structure 200m! but with unscaled true density and YM), computation time is in the order of mintues!

This is what I do. The conversion will take just a minute.

-> Scale only length: 1 unit = 1E-6 m.

Then,

Density = 2.329E3 kg/m^3 = 2.329E3 x (1E-6)^3 = 2.329E-15

Young's Modulus = 1.124E11 = 1.124E11 x 1E-6 = 1.124E5

where YM's unit Pa has been broken down to N/m^2 = kg*m/(s^2*m^2) = kg/(m*s^2)

I think the orders E-15 and E5 are throwing me off...Time/LPF Inc is around 1E-10...

Please tell me if I've made any mistakes, or if there is a better scaling standard than this.

I greatly appreciate your help.
Thanks.

PS> I think the nature of this problem is also contributing to the high computation cost: It is a "dynamic, explicit" nonlinear analysis of a flat, round silicon cylinder with two thin arms coiling around it. The ends of the two arms are subject to force that stretches the spiral arms and thus uncoils the structure. 15k nodes, 9k elements.

 

[xerf]

I have a problem understanding your scaling approach.

If I had a model with dimensions of about 200um, for the FE model I would convert all the lenghts in (mm). Therefore, I would need to supply the Young's modulus in MPa (i.e. N/mm^2) and the density in Kg/mm^3.

 

[jongyonkim]

Hi xerf, I didn't quite understand what you mean by "convert all the lengths in (mm)" for 200um.

Do you mean,

a) 200um -> 200mm, so use a "factor of 1E-3", which applies to other variables.

b) 200um -> 200mm, just use mm instead of um.

If you were me, how would you scale density and Young's Modulus?

Silicon density : 2.329E3 kg/m^3
Young's Modulus : 1.124E11 Pa

Please take a minute to calculate them for me, as I don't fully understand what you mean by converting lengths.

Thank you for your time

 

[xerf]

I guess we have a different understanding on how to do finite element modeling.

ABAQUS does not use units for various quantities. It is up to the user to be consistent with the units of the quantities he needs in the model.

I meant that
200(um)=0.2(mm)
2.329E3 (kg/m^3)=2.329E-6 (kg/mm^3)
1.124E11 (Pa)=1.124E5 (MPa)

 

[jongyonkim]

Hi Xerf,

I understand what you mean.

The reason why you chose to do in mm scale instead of um scale (what I did) was to choose the units to make sure the extreme values (E-6 to E5) are as close together as possible, right?

So, if I were to follow your method with the mm scale, I would have to create a part size 0.2 units for 200um. (before, with um scale, my part size was 200)

1) I see how density becomes 2.329E-6 kg/mm^3. However, for Young's Modulus, don't you have to take into account the N in Pa = N/mm^2? With the mm scale, N = kg*mm/s^2 , so Pa = N/mm^2 = kg*mm/s^2/mm^2 = kg/(mm*s^2). One of the mm in the denominator cancels out. So it should be 1.124E8 (kPa)?

2) I had actually tried doing the scaling mentioned above and with other values (part size 0.2, 200, 20000). Apparently, for some strange reason, using a part size 20000 (hence 1 unit length = 10^-8 m) is orders of magnitude faster than the previous two (but still taking weeks). Do you have any idea why this might happen? According to ABAQUS, if you scale everything right, this discrepancy shouldn't be there.

Sorry about my obsession with precision in scaling. I have to get this right before I look for other solutions...

Thanks.

 

[xerf]

1) 1Pa=1N/m^2 (not 1N/mm^2)

2)The maximum time increment for explicit scheme is restricted by the stability of the explicit algorithm.
In general, the time increment is limited by the relation:

delta_t<=2/((1-2*theta)*lambda_i),

where lambda_i is the greatest eigenvalue of the system
and 0<theta<1.0 depends on the numerical scheme used, for explicit schemes theta=0.0 (whereas theta=1.0 for implicit->i.e. no restrition on time increment for the implicit schemes).

Therefore:
delta_t<=2/(lambda_i)

However, computing the system eigenvalues can be expensive, thus sometimes the maximum eigenvalue is estimated. Generally the greatest element eigenvalue is used instead of the greatest system eigenvalue.( There is a theorem proving that the system eigenvalues are bounded by the eigenvalues of the individual elements.) The maximum eigenvalue of an element can be related to its dimensions, in such way that delta_t is proportional to a minimum characteristic lenght of the element:

delta_t<=min(L_elem/c)

where c (if I remember well) is the wave speed in the material.

I am not sure exactly on how ABAQUS computes the time increment for the explicit scheme, but I guess this might explain your problem.