Learning Forum

[JHPontes]

Hello all

I would like to perform an harmonic analysis usin viscoelastic materials in WorkBench.

First I was having some problems to define viscoelastic properties, but was able to manage it using command snippets. However the results I have don't match with my experimental data:

[JHPontes]

n

[peteroznewman]

nThe model results seem to be reasonably close to the experimental values. How close did you expect the agreement to be?n

[JHPontes]

nThe results shown in the figure are obtained via APDL, as yes they are pretty close to experimental values. nHowever I try to make the same analysis using WorkBench and the results are totally different. I suspect its something wrong with the viscoelastic properties since WB resulsts file says something about poisson ration being unused when I expected it to be used to determine Young modulus based on complex values from Prony series.nNot really sure if that's really the case, however the point is I can't make the same analysis in WB.n

[peteroznewman]

nRead this comment. /forum/discussion/comment/15103#Comment_15103nYou can perform a full harmonic analysis on viscoelastic materials by defining frequency dependent elastic modulus, Poisson's ratio and damping using TB,ELASTIC and TB,DAMP commands (WB does not support this in GUI, so you'll need to use command snippets). It still assumes linear response so large-deformation effects are not included.n

[JHPontes]

Hello Array, I understand it, however I don't have those properties.nthe procedure I've used is to introduce shear complex modulus via TB,PRONY,,,EXPE according to item 4.7.3 in https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_mat/evis.html?q=Gmodulus. In the same page you can find the statement Two elastic constants are required to define the complex constitutive model. If only one set of experimental data for a complex modulus is defined, the Poisson's ratio (defined via MP or by elastic data table) is used as the second elastic constant. That is exactly what is going on my APDL file. I introduce only one complex data (complex shear modulus) and expect it to use poisson ratio (defined as MP,PRXY,2,0.499) as the second elastic constant. Using this two elastic properties (nu and complex G) the material model is fully determined (hence you need two properties to determine the others via constitutive equations). nThe point is it works perfectly fine when performing the whole analysis via APDL interface (check Validação_absorvedor.txt).nWhen I try to make the same analysis in WB, everything is the same (appart from the mesh), or at least I expect it to be the same. Except the results aren't even close. nI suspect there's something wrong with the properties. When performing the analysis in APDL, even thought young Modulus is defined, it doesn't make any difference since the two properties used to define the material are poisson and complex shear modulus, not young modulus. When performing the analysis in WB (using command snippets to introduce viscoelastic material properties, which are the same commands in APDL by the way) it doesn't happen. Not really sure about it, but it seems to be using Young modulus and complex shear to determine the others.nWould be really gratefull if you could take a look at the files I've attached.n

[peteroznewman]

nSorry, this is beyond my understanding. Maybe can take a look.n

[BenjaminStarling]

and nThe first thing I noticed is that the force is not applied to the same node/location, as per the image below, in APDL it is offset from the edge, in Mechanical it is on the outer edge. This doesn't drastically change the results but it should be kept consistent. The second thing I noticed is that there is a density assignment in engineering data of the VAMAC material, this should be set to zero, as in the input file you have not specified a density and this is read by APDL as 0. The density and youngs modulus of Aco is also different from your input file, 7850 vs. 7860, 2.1E11 vs. 2.078E11.nThe actual issue is the mesh though. The following results are from the exact same models as per your MAPDL input file. One has the auto-generated mesh from Mechanical, the other uses an identical mesh to the plot above. You can see that there is some observable light blue contour on the inside disk for the model on the left. This is caused by only having one element through the thickness of the viscoelastic material. The number of divisions through the thickness here has a direct influence on the stiffness of your model. To help with meshing in Mechanical, you should divide your geometry into quarters. This will create 6 sided volumes that can be swept/multizoned much easier, and creates the edge divisions required to specify sizings.nThe model on the right gives me this frequency response in the z directionnn