Search
Close this search box.
Notifications
Clear all

Damping in viscoelastic FE model

7 Posts
4 Users
0 Reactions
856 Views
Posts: 4
Topic starter
(@nlynch066)
New Member
Joined: 13 years ago

Hi all,

I am doing harmonic analysis simulation for a structure in Abaqus. I am interested in studying the extent of damping after attaching a tuned viscoelastic damper (or a simple viscoelastic layer to begin with) to the structure.

I entered viscoelastic material (3M ISD 112) parameters in frequency domain (obtained from research literature).

I am not using any other structural or viscous damping for the structure.

Ideally I expected that response peaks of structure with viscoelastic damping to be more wide indicating material damping. But I am finding sharp peaks at resonances for models with and without viscoelastic layer. Only the frequency at which peaks occur shifts due to effect of mass addition. How can we see the effect of damping due to mounting of viscoelastic material? Is there something I am missing to consider ?

Thank you in advance.

Regards

Kiran

6 Replies
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

Your expected observations seam reasonable to me. Are you sure you defined the linear viscoelastic material model properly?

-Jorgen

6 Replies
Posts: 4
Topic starter
(@nlynch066)
New Member
Joined: 13 years ago

Hi Jorgen,

Thank you for the response. Please find attached the viscoelastic data which I am using. I am using Frequency domain data. I guess I can also use time domain data (also included in adjacent sheet) in which case Abaqus may try to convert into frequency domain when I am carrying out harmonic analysis. Also find attached the result in another sheet comparing the harmonic response for damped and undamped condtion.

Thanks again for your support and wonderful website.

Regards

Kiran

Reply
Posts: 4
Topic starter
(@nlynch066)
New Member
Joined: 13 years ago

Hi Jorgen,

Just clarifying one more possibility:As you can see from attachment in previous post, I did not give any damping in usual Edit Material, damping window. I am assuming that G and G of viscoelastic material will automatically contribute to the material damping. Is this right or shall I have to specify Damping (composite) separately for viscoelastic material, for e.g. loss factor (eta = G/G). But problem with this kind of definition would be loss factor or damping cannot be defined as dependent on frequency (as we give in viscoelastic material definition).

Thank you,

Regards
Kiran

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

It should not be necessary to supply additional (composite) damping...

-Jorgen

Reply
Posts: 3
(@sonidos)
New Member
Joined: 12 years ago

Kiran,

Are you sure viscoelasticity is active in the analysis youre running? For material damping to be accounted for in natural frequency extraction you should be using *Frequency Complex. For frequency sweep analysis (e.g. with harmonic excitation) I recommend using direct steady state analysis or subspace steady state (less accurate). Dont use modal analysis because as far as I remember it does not include viscoelasticity, the response is calculated from elastic parameters only.
Than also, the results for analysis with material damping will be expressed in complex numbers and you should carefully interpret the data (real, imaginary components or complex magnitude).

Hope this helps!
Damian

Reply
Posts: 3
(@herbalincen22)
New Member
Joined: 8 years ago

Im gonna resurrect this thread.

I have Prony series parameters for for the dynamic shear modulus of bituminous materials. Usually, people establish a master curve spanning approximately 8 decades of frequency.

Until now a verified that I am using Abaqus correctly by running time domain simulations on a single element (C3D8R) under pure shear and small strains (1%). There, after two cycles, the stress amplitude and phase angle equilibrate and i sample the steady-state response, which is rather precisely what i expect. Nevertheless, this is tedious, since I am not interested in the transient response and I need one simulation for each frequency.

*Material, name=Mortar
*Elastic, moduli=instantaneous
2098.57851, 0.35
*Viscoelastic, time=PRONY
3.7568E-001, 0., 0.000115
2.7276E-001, 0., 0.000787
1.9427E-001, 0., 0.00538
1.0653E-001, 0., 0.0368
3.8469E-002, 0., 0.251
9.1862E-003, 0., 1.72
2.4574E-003, 0., 11.7
4.3744E-004, 0., 80.3
1.6211E-004, 0., 549.
4.4130E-005, 0., 3750.

I figured that it would be advantageous using direct steady state analysis. Unfortunately, there I cannot specify a instantaneous modulus, but ABQ wants me to put in a long term modulus. This does not exist since bitumen is typically modelled as a fluid, so the equilibrium spring in the GenMax model is disregarded.

So when i specify

*Material, name=Mortar
*Density
1E-004
*Elastic, moduli=instantaneous
2098.57851, 0.35
*Viscoelastic, frequency=PRONY
3.7568E-001, 0., 0.000115
2.7276E-001, 0., 0.000787
1.9427E-001, 0., 0.00538
1.0653E-001, 0., 0.0368
3.8469E-002, 0., 0.251
9.1862E-003, 0., 1.72
2.4574E-003, 0., 11.7
4.3744E-004, 0., 80.3
1.6211E-004, 0., 549.
4.4130E-005, 0., 3750.

and define a step with a frequency sweep between 1e-4 and 1e+4 Hz:

*Step, name=sinusoidal_loading, nlgeom=NO, perturbation
*Steady State Dynamics, direct, friction damping=NO
0.0001, 10000., 9, 1.

Abaqus issues a warning:

***WARNING: MODULI=INSTANTANEOUS ON *ELASTIC CANNOT BE USED WITH FREQUENCY
DOMAIN VISCOELASTICITY. THE MODULI ARE CONVERTED TO LONG TERM
MODULI USING THE PRONY SERIES PARAMETERS.

Ok, this sounds like Abaqus would take care of that, although i have no clue how. But more importantly I cannot make any sense of the results. Everything is off. I neglected inertia effects by setting the density to a very low value, which is in accordance with the Abaqus manual. I also tried different densities, but the results are the same.

Any help is appreciated.

Kind regards,
Johannes

Reply
Share: