Learning Forum

[ItalicBike]

Hi everybody,

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.

mat_num=2

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

TBTEMP, 22

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

 

ALLSEL

/solu

[John Doyle]

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

TBPT, ,

.....

• TB,EXPE,1, , ,GMOD


• TBPT,,,


• ....




• I am not sure the order matters, but you could test it.




• Regards,


• John


• 
  26 


• 26 


•  

[ItalicBike]

 Hi jjdoyle,

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 TBOPT = EXPERIMENTAL."

 

So I have the command:

TB, EXPE, mat_num, 1, 10, GMODULUS

TBTEMP, 22

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

To define FREQUENCY, G' , G'', Loss Factor (zero because he want just 2 constant, I think the third is calculated). Why he need the empty prony series? I do not understand. Into the solution information, he write:

 

***** ANSYS ANALYSIS DEFINITION (PREP7) *****

 PARAMETER MAT_NUM =     2.000000000   

 MATERIAL          2     EX   =   50000.00     

 MATERIAL          2     NUXY =  0.4900000     

 MATERIAL          2     DENS =  0.1000000E-08 

   Complex elastic constants input with TB,EXPE                                   
   WITH A MAXIMUM OF  1 TEMPERATURES AND    0 DATA POINTS

   SHEAR MODULUS OPTION FOR MATERIAL 2
   WITH A MAXIMUM OF  1 TEMPERATURES AND    10 DATA POINTS

 TEMPERATURE TO BE USED FOR THE NEXT TBDAT COMMAND=  22.0000
    TEMPERATURE SPECIFICATION=  1

 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     0.10000   Y=700000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     0.20000   Y=900000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     0.50000   Y=1100000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     1.00000   Y=1500000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     2.00000   Y=2000000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=     3.00000   Y=2250000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=    10.00000   Y=4000000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=   100.00000   Y=17000000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=   500.00000   Y=40000000.00000
 POINT INSERTED IN THE  EXPE  TABLE FOR MATERIAL     2
    X=  9000.00000   Y=200000000.00000

 SELECT      COMPONENT POLYMER                        

 MODIFY ALL SELECTED ELEMENTS TO HAVE  MAT  =         2

 SELECT ALL ENTITIES OF TYPE= ALL  AND BELOW


 ***** ROUTINE COMPLETED *****  CP =         0.469

 

But no change in the results..

[John Doyle]

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).

Regards,

John

[ItalicBike]

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.

 

 

 

[John Doyle]

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.

[ItalicBike]

I don't have the access to customer portal, how can i do it? Could you bring be the solution in another way?

 

Thank you

 

A.

[Sandeep Medikonda]

Hi,

 Here is the APDL input script to generate the curve fit. 

fini

/clear



/PREP7

!*

/com,Curve Fitting Experimental Data Written To sample.exp

TBFT,EADD,1,SDEC,sample.exp

TBFT,FCASE,1,NEW,PVHE,test

TBFT,FADD,1,VISCO,PSHEAR,5

TBFT,FADD,1,VISCO,PBULK,NONE

TBFT,FADD,1,VISCO,SHIFT,NONE

TBFT,FCASE,1,FINI

TBFT,SET,1,CASE,test,,1,1

TBFT,SET,1,CASE,test,,2,1

TBFT,SET,1,CASE,test,,3,1e-5

TBFT,SET,1,CASE,test,,4,1

TBFT,SET,1,CASE,test,,5,1e-4

TBFT,SET,1,CASE,test,,6,1

TBFT,SET,1,CASE,test,,7,1e-3

TBFT,SET,1,CASE,test,,8,1

TBFT,SET,1,CASE,test,,9,1e-2

TBFT,SET,1,CASE,test,,10,1

TBFT,SET,1,CASE,test,,11,1e-1

TBFT,SET,1,CASE,test,,comp,pvhe

TBFT,FIX,1,CASE,test,,1,0

TBFT,FIX,1,CASE,test,,2,0

TBFT,FIX,1,CASE,test,,3,1

TBFT,FIX,1,CASE,test,,4,0

TBFT,FIX,1,CASE,test,,5,1

TBFT,FIX,1,CASE,test,,6,0

TBFT,FIX,1,CASE,test,,7,1

TBFT,FIX,1,CASE,test,,8,0

TBFT,FIX,1,CASE,test,,9,1

TBFT,FIX,1,CASE,test,,10,0

TBFT,FIX,1,CASE,test,,11,1

TBFT,SOLVE,1,CASE,test,,0,1000,0,0

TBFT,FSET,1,CASE,test

Which contains a storage and loss modulus vs frequency data and is named as 'sample.exp':

/1,freq
/temp,75
 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.

Regards,

Sandeep

[ItalicBike]

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?

 

Thanks

Regards.

[ItalicBike]

Nobody could help me?

[John Doyle]

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.