September 6, 2018 at 3:20 pmItalicBikeSubscriber
I'm trying to model a 100x100 mm sandwich composed by 3 layer:
1. Steel sheet, 3 mm thick
2. Viscoelastic polymer, 1 mm thick
3. Steel sheet, 3 mm thick
I need to evaluate the damping effect of the application of 3 mm thick steel sheet with polymer on the FRF of the 3 mm plate. The surfaces are sticked togheter.
I got the complex modulus G' and loss factor from DMA experimental analysis. I try to follow the help, ANSYS Documentation -> Mech APDL -> Material Reference -> Non Linear Material Properties -> Viscoelasticity, in particular from 4.7.3 paragraph. Unfortunately, i don't see any change on the model results.. Could someone help me?
This is the command (APDL) that I used to define the material. Polymer is the name selection.
MP, EX, mat_num, 0.5E+05
MP, NUXY, mat_num, 0.49
MP, DENS, mat_num, 1E-09
TB, EXPE, mat_num, 1, 10, GMODULUS
TBPT, DEFI, 0.1, 70000, 34300, 0
TBPT, DEFI, 0.2, 90000, 53100, 0
TBPT, DEFI, 0.5, 110000, 75900, 0
TBPT, DEFI, 1.0, 150000, 119000, 0
TBPT, DEFI, 2.0, 200000, 170000, 0
TBPT, DEFI, 3.0, 225000, 207000, 0
TBPT, DEFI, 10, 400000, 396000, 0
TBPT, DEFI, 100, 1700000, 1700000, 0
TBPT, DEFI, 500, 4000000, 3600000, 0
TBPT, DEFI, 9000, 20000000, 14000000, 0
TB, PRONY, mat_num, , EXPERIMENTAL
CMSEL, S, Polymer, ELEM
EMODIF, ALL, MAT, 2
September 6, 2018 at 4:44 pmJohn DoyleAnsys Employee
Are you missing a comma on the TB,prony,,, command?
Shouldn't it be: "TB,prony,mat_num,,,Experimental" ?
Also, the sample APDL input I am looking at has the commands ordered:
TB,PRONY,1, , ,EXPE
TB,EXPE,1, , ,EMOD
September 6, 2018 at 6:04 pmItalicBikeSubscriber
thanks for answering. Yes, I was missing a comme on TB, PRONY, , , command. Now he doesn't give any error, but he's not sensitive to modulus variation. In help documentation descripted in my previous post, it's written:
"Using experimental data to define the complex constitutive model requires elastic constants (defined via MP or by an elastic data table [TB,ELASTIC]). The elastic constants are unused if two sets of complex modulus experimental data are defined. This model also requires an empty Prony data table (TB,PRONY) with
So I have the command:
September 7, 2018 at 12:32 pmJohn DoyleAnsys Employee
The need for "... empty Prony data table (TB,PRONY) with TBOPT = EXPERIMENTAL." is just the way it was programmed to receive the input data.
When you say there is "...no change in the results", what result are you referring to?
I would recommend plotting max amplitude vs frequency. The harmonic viscoelasticity mat'l is intended to enable you to define frequency dependent stiffness and damping, so amplitude vs frequency curve should change as you add more stiffness and/or damping, but perhaps a particular result at a particular location and frequency will not change much or at all or perhaps the damping is too small to make any difference.
Alternatively, as a test, you could also try to define the equivalent the Prony Series alpha and tau values in frequency domain (as a test).
September 7, 2018 at 1:07 pmItalicBikeSubscriber
I'm referring the frequency response graph, acceleration vs. frequency.
Howerer, I think that I solved the problem, now it seems to works, but I don't know if it's good.
jjdoyle, you wrote: "Alternatively, as a test, you could also try to define the equivalent the Prony Series alpha and tau values in frequency domain (as a test)."
But I got only experimental results about G' Modulus and Loss Factor, I don't have the shear vs. time relaxation graph. Considering the experimental data the i got, the command that i used it's the correct procedure?
I want to be sure that the procedure is correct, than i try to change the values!
Thank you very much.
September 8, 2018 at 9:25 amJohn DoyleAnsys Employee
You can use our curve fitting tool to calculate alpha and tau from experimental data in frequency domain for use in a prony series expression for harmonic viscoelasticity. Do you have access to the ANSYS customer portal? There is a KM Solution (#2036139) on the customer portal illustrating how to do this.
September 8, 2018 at 12:53 pmItalicBikeSubscriber
I don't have the access to customer portal, how can i do it? Could you bring be the solution in another way?
September 8, 2018 at 2:01 pmSandeep MedikondaAnsys Employee
Here is the APDL input script to generate the curve fit.
/com,Curve Fitting Experimental Data Written To sample.exp
Which contains a storage and loss modulus vs frequency data and is named as 'sample.exp':
20 2.19E+04 8.44E+03
30 2.58E+04 9.26E+03
40 2.87E+04 9.78E+03
50 3.09E+04 1.01E+04
60 3.28E+04 1.05E+04
70 3.44E+04 1.07E+04
80 3.56E+04 1.08E+04
90 3.68E+04 1.09E+04
100 3.79E+04 1.10E+04
200 4.44E+04 1.13E+04
300 4.80E+04 1.14E+04
400 5.04E+04 1.12E+04
500 5.17E+04 1.11E+04
600 5.30E+04 1.09E+04
700 5.40E+04 1.08E+04
800 5.49E+04 1.08E+04
900 5.53E+04 1.06E+04
1000 5.61E+04 1.06E+04
2000 5.99E+04 9.84E+03
3000 6.15E+04 9.31E+03
4000 6.26E+04 8.97E+03
5000 6.33E+04 8.75E+03
Note: The values for Tau are still TIME.
The values are initialized and fixed based on values inversely proportional to frequency and are fixed.
Note: The best curve fit for this particular case is achieved by using an absolute error calculation.
September 10, 2018 at 1:33 pmItalicBikeSubscriber
Thanks for your help, Sandeep.
I wrote into the file sample.exp my experimental data (frequency, storage modulus and loss modulus @22°C) and ran the analysis. 2 questions:
1. In solution information panel, i read "successfully saved the calculated coefficients to ANSYS database 1: test". Where can i find it? I want to plot the graph relative moduli vs. time founded with the curve fitting..
2. In analysis settings, solver control, do i switch on the damped option?
September 14, 2018 at 4:13 pmItalicBikeSubscriber
Nobody could help me?
September 14, 2018 at 4:54 pmJohn DoyleAnsys Employee
Assuming you are in MAPDL, after you read in the curve fitting commands above, (make sure you are in the same directory that the file sample.exp is located in) you can open the curve fitter:
Main Menu=>Preprocessor=>Mat'l Properties=>Matl Models=>Structural=>Nonlinear=>Viscoelastic=>Prony Curve Fitting...
..and from there, choose the Curve fit labeled "test" (there is only one). Then click "Plot" to generate the resulting curve fit.
I cannot answer your second question.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.