Author 
Message 
irantzu.uriarte User
Joined: 21 Oct 2008 Posts: 17

Posted: Thu May 21, 2009 2:19 am 


Hi there,
Here I come once again, now that I know that what I wanted to do is
possible.
I'll insert here the "simple" log file (at the end I used a simple body with
just one element, to see where the problem could be), so maybe you can tell
me where is the problem in my model, if in ansys or in the material model.
/PREP7
ET,1,SOLID185
KEYOPT,1,2,0
KEYOPT,1,3,0
KEYOPT,1,6,0
KEYOPT,1,10,0
!Material 1 > hiperelástico
TB,HYPER,1,,2,YEOH !Yeoh data table
TBDATA,1,0.163498 !Define C1
TBDATA,2,0.125076 !Define C2
TBDATA,3,6.93063E5 !Define first
incompressibility parameter
!Material 2 > viscoelástico
tb,hyper,2,,,moon !elastic properties
tbdata,1,38.462E4,,1.2E6
TB,PRONY,2,1,1,SHEAR
TBTEMP,0
TBDATA,1,0.5,2,
TB,PRONY,2,1,1,BULK
TBTEMP,0
TBDATA,1,0.5,2,
!Material 3 > fricción interna (Von Mises bilineal isotrópico sin
endurecimiento)
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,3,,1
MPDATA,PRXY,3,,.4999
TB,BISO,3,1,2,
TBTEMP,0
TBDATA,,3,0,,,,
BLOCK,0,10,0,50,0,100,
VATT,1,,1
MSHAPE,0,3D
MSHKEY,1
ESIZE,100
VMESH,ALL
EGEN,3,0,ALL,,,1,,,,,
/SHRINK,.001
DA,5,ALL,0
*DEL,_FNCNAME
*DEL,_FNCMTID
*DEL,_FNCCSYS
*SET,_FNCNAME,'proba'
*SET,_FNCCSYS,0
! /INPUT,..\..\LANA\Proba.func,,,1
*DIM,%_FNCNAME%,TABLE,6,8,1,,,,%_FNCCSYS%
!
! Begin of equation: 0.05*sin(1000*3.1416*{TIME})
*SET,%_FNCNAME%(0,0,1), 0.0, 999
*SET,%_FNCNAME%(2,0,1), 0.0
*SET,%_FNCNAME%(3,0,1), 0.0
*SET,%_FNCNAME%(4,0,1), 0.0
*SET,%_FNCNAME%(5,0,1), 0.0
*SET,%_FNCNAME%(6,0,1), 0.0
*SET,%_FNCNAME%(0,1,1), 1.0, 1, 0, 1000, 0, 0, 0
*SET,%_FNCNAME%(0,2,1), 0.0, 2, 0, 3.1416, 0, 0, 1
*SET,%_FNCNAME%(0,3,1), 0, 3, 0, 1, 1, 3, 2
*SET,%_FNCNAME%(0,4,1), 0.0, 1, 0, 1, 3, 3, 1
*SET,%_FNCNAME%(0,5,1), 0.0, 1, 9, 1, 1, 0, 0
*SET,%_FNCNAME%(0,6,1), 0.0, 2, 0, 0.05, 0, 0, 1
*SET,%_FNCNAME%(0,7,1), 0.0, 3, 0, 1, 2, 3, 1
*SET,%_FNCNAME%(0,8,1), 0.0, 99, 0, 1, 3, 0, 0
! End of equation: 0.05*sin(1000*3.1416*{TIME})
!>
DA,6,UZ,%proba%
FINISH
/SOL
ANTYPE,4
SOLCONTROL,ON
NLGEOM,1
TIME,100
NSUBST,20,100,10
!AUTOTS,1
OUTRES,ERASE
OUTRES,ALL,1
SOLVE
Thank you in advance,
Irantzu
______________________________
PhD Student
EHUUPV Spain
Mensaje original
De: email address suppressed [mailto:email address suppressed] En nombre
de Irantzu
Enviado el: miércoles, 06 de mayo de 2009 9:48
Para: 'ANSYS User Discussion List'
Asunto: Re: [Xansys] About viscoelasticity + hyperelasticity
Thank you very much, Paris. I've been in PolymerFEM.com web, reading and I
wrote to Mr. Bergstrom too. Now I'm waiting for his answer...
Mensaje original
De: email address suppressed [mailto:email address suppressed] En nombre
de Altidis, Paraschos C.
Enviado el: martes, 05 de mayo de 2009 22:45
Para: ANSYS User Discussion List
Asunto: Re: [Xansys] About viscoelasticity + hyperelasticity
Irantzu,
As I'm watching the structural mechanics enhancements in v12.0, your
problem is solved with the new BergstromBoyce material model. BTW,
Bergstrom is the person behind PolymerFEM.com that I strongly
recommended you visiting in my first reply.
Along the same lines, FINALLY we can account for the Mullins Effect in
hyperelastic materials. Thanks ANSYS, Loooooong overdue but it's here
now.
Regards,
Paris Altidis
Belcan Corp.
Original Message
From: email address suppressed [mailto:email address suppressed] On
Behalf Of Dave Lindeman
Sent: Thursday, April 30, 2009 12:01 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] About viscoelasticity + hyperelasticity
You can mix linear elastic and hyperelastic chains (e.g., the
ArrudayBoyce viscoplasticity model uses both). However, if your
simulation involves finite strains, then, in general, linear elastic
models shouldn't be used.
It sounds as though you should really be working on a USERMAT. Although
it may be possible to calculate the global force vs. deflection response
with reasonable accuracy using multiple overlayed elements and material
models, you won't be able to calculate the correct strain decomposition.
Regards,
Dave

Dave Lindeman
Lead Research Specialist
3M Company
3M Center 2353F08
St. Paul, MN 55144
6517336383
Irantzu Uriarte Gallastegui wrote:
> Hi Paris,
>
> About your comments, I'll try to explain what I'd like to do with my
model.
>
> The rheological model really consists of 3 chains in parallel (so the
> final stress contribution will be the summ of the 3 chains' stresses):
>  One to model the hyperelastic behaviour (with a spring) > with a
> Yeoh's model with 3 parameters
>  Another one to model the viscoelasticity (with a spring in series
> with a dashpot)> here comes my main doubt
>  Last one to model the plastic effect (with a spring in series with a
> friction element)> with a Von Mises elastoplastic model without
> hardening
>
> When I introduce the viscoelastic model's parameters (and the same
> occurs with the friction part chain), I have to introduce its elastic
> part. And I don't know if I can use linear elastic Ex and Prxy here,
> but maintaining Yeoh's model (nonlinear elastic) in the other chain.
> Maybe all the springs must be of the same kind? (all of them linear or
> all of them non linear...?)
>
> I've got some results from tests (not mine yet, I still am in the
> begining...). But I'm not sure if I understand completely how should I
> model my material...
>
> I'll tell you if I conclude something realistic...
> Best regards,
> Irantzu
>
>
>
>
> "Altidis, Paraschos C." <email address suppressed> ha escrito:
>
>> Hi Irantzu,
>> Questions about materials are more than welcome on this forum.
After
>> all, material nonlinearities are part of the game and we don't get
>> that many threads on materials.
>> To your questions:
>> 1) Overlapping meshes with different materials may not the issue
>> {based on what we know about your problem}. Their interaction and
>> contribution to the results would've been my main concern. I don't
>> quite follow what you're trying to model but it seems like 3 layers
>> of hybrid visco/hyper/?? Elastic material. Is your intent to examine
>> each layer's contribution to the "composite" or as a single 3layer
"composite" ??
>> 2) As far as the hyperelastic mat properties, yes, they can make or
>> break the convergence/accuracy of your model with excessive
>> deformation and hourglassing. Best practices: a) have a hyperelastic
>> material model that is most appropriate for the actual material ; b)
>> Have reliable test data that describe the response of the material at
>> hand (that is, not from a general materials handbook, but ACTUAL
>> test data) 3)what is the hyperelastic material that you are using ?
>> 4) Do you have tested properties for each layer or this is too early
>> to discuss this issue ??
>> 5) Strongly recommend to visit polymerFEM.com. You can browse the
>> site for lots of material and ask Jorgen Bergstrom the same question
>> you posted here.
>>
>> Keep us posted of your findings.
>>
>> Regards,
>> Paris Altidis
>> Belcan Corp.
>>
>>
>>
>> Original Message
>> From: email address suppressed [mailto:email address suppressed] On
>> Behalf Of Irantzu Uriarte Gallastegui
>> Sent: Wednesday, April 29, 2009 4:20 AM
>> To: email address suppressed
>> Subject: [Xansys] About viscoelasticity + hyperelasticity
>>
>> Dear all,
>>
>> Since my last mail asking about 3 superimposed meshes, I've been
>> checking my logfile and now I've got some doubts about material
>> properties. I don't know if it's possible to ask you about it here,
>> but if someone has worked with what I'm going to ask, I'd thank a lot
>> your help.
>>
>> One of my meshes is for a hyperelastic material and another one for a
>> viscoelastic material property. The rheological model would be, for
>> these two, 2 chains in parallel, one with a spring, another one with
>> a spring in series with a dashpot.
>> If the spring I use in the elastic chain is nonlinear
>> (hyperelastic), is it necessary the other spring (in the viscoelastic
>> chain) to be nonlinear? Or could I introduce a linear spring in the
second chain?
>>
>> If the values of the material parameters I introduced weren't
>> realistic, maybe the model distorts a lot too much and is for that
>> that the answer cannot be visualized?
>>
>> Thank you in advance, and excuse me please if such kind of questions
>> are out of this forum.
>>
>> Best regards,
>> Irantzu
>>
>> __________________
>> PhD Student
>>
>> EHUUPV Spain
>>
>>
>> ++
>>  XANSYS web  www.xansys.org/forum 
>>  XANSYS blog  xansys.blogspot.com 
>>  The Online Community for users of ANSYS, Inc. Software 
>>  Hosted by PADT  www.padtinc.com 
>>  Send administrative requests to email address suppressed 
>> ++
>>
>>
>> 29/4/2009This email transmission contains information that is
>> confidential and may be privileged. It is intended only for the
>> addressee(s) named above. If you receive this email in error,
>> please do not read, copy or disseminate it in any manner. If you are
>> not the intended recipient, any disclosure, copying, distribution or
>> use of the contents of this information is prohibited. Please reply
>> to the message immediately by informing the sender that the message
>> was misdirected. After replying, please erase it from your computer
>> system. Your assistance in correcting this error is appreciated.
>>
>>
>> ++
>>  XANSYS web  www.xansys.org/forum 
>>  XANSYS blog  xansys.blogspot.com 
>>  The Online Community for users of ANSYS, Inc. Software 
>>  Hosted by PADT  www.padtinc.com 
>>  Send administrative requests to email address suppressed 
>> ++
>>
>>
>
>
>
>
> ++
>  XANSYS web  www.xansys.org/forum 
>  XANSYS blog  xansys.blogspot.com 
>  The Online Community for users of ANSYS, Inc. Software 
>  Hosted by PADT  www.padtinc.com 
>  Send administrative requests to email address suppressed 
> ++
>
>
>
++
 XANSYS web  www.xansys.org/forum 
 XANSYS blog  xansys.blogspot.com 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to email address suppressed 
++
5/5/2009This email transmission contains information that is confidential
and may be privileged. It is intended only for the addressee(s) named
above. If you receive this email in error, please do not read, copy or
disseminate it in any manner. If you are not the intended recipient, any
disclosure, copying, distribution or use of the contents of this information
is prohibited. Please reply to the message immediately by informing the
sender that the message was misdirected. After replying, please erase it
from your computer system. Your assistance in correcting this error is
appreciated.
++
 XANSYS web  www.xansys.org/forum 
 XANSYS blog  xansys.blogspot.com 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to email address suppressed 
++
++
 XANSYS web  www.xansys.org/forum 
 XANSYS blog  xansys.blogspot.com 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to email address suppressed 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Thu May 21, 2009 6:30 am 


Dear Irantzu,
your third material is nearly incompressible, with a poisson ratio of 0.4999 . The mixed uP formulation is more robust (check Ansys manual) than the displacement formulation.
The variation with time of your prescribed displacement does not correspond with the 0.05*sin(1000*3.1416*{TIME}) that is written in the comment. By looking at the displacements in the /post26 postprocessor (/post26$nsol,2,3,u,z$plvar,2), the prescribed amplitude is 0.05, but the frequency is not 3141.6rad/s (whose period would be 1/500seconds), but 7.306e3 rad/s (period=860 sec).
Instead of solving three overlapped meshes, perhaps it would help you to solve three independent problems with only one mesh in each of them, and check the results of each single model.
You are applying a maximum shear deformation of 0.05/10=0.005=0.5% (maximum UZ displacement/thickness). At time=100 the shear deformation is 0.0335/10=0.00335=0.335%.
For the third material, your shear modulus is G=E/(2*(1+mu))=1/3, therefore your shear stress is tauxz=1.67e3 , well within the linear regime (fy/sqrt(3)=sqrt(3)=1.732>tauxz).
For your first material, the initial shear modulus is G=2*c10=2*0.163498=0.327, and multiplying by the shear deformation at time 100 you obtain the following shear stress 0.327*0.00335=0.0011.
For your second material, the initial shear modulus is G_0=2*(c10+c01)=2*(38.462E4+0)=769240, which is several orders of magnitude bigger than the other two materials. The fraction of shear modulus that is lost is G1=0.5*G_0, with a relaxation time of 2 seconds, therefore, at time t, G(t)=G_0*0.5*(1+exp(t/2)). For t=infinity, the shear modulus is G_inf=0.5*G_0. The relaxation time is much smaller that the period of your excitation, therefore the response will be similar to that of a elastic material with G=G_inf. Multiplying G_inf by the shear deformation at time 100, you obtain the following shear stress: 0.5*769240*0.00335=1288
When solving the three independent problems, the shear stress results are very close to the values given above, except for the second material, where Ansys does not converge. Ansys suggest ramped loading or modify the mesh. I have used ramped loading (KBC,1), and still did not converge. By increasing the relaxation time for bulk modulus (TB,PRONY,2,1,1,BULK$TBTEMP,0$TBDATA,1,0.5,2000) to a large value (2000), Ansys converged and the shear stresses were close to the value calculated above.
When solving the problem with the three overlapped meshes, the same results as for the three independent meshes are obtained. You have applied a prescribed displacement on three "springs" (elements) in parallel.
I hope that this helps.
Best regards,
Jose M. Galan
Dept. Construction Engineering
University of Seville (Spain)
 Mensaje original 
De: Irantzu <email address suppressed>
Fecha: Jueves, Mayo 21, 2009 11:21 ombr
Asunto: Re: [Xansys] About viscoelasticity + hyperelasticity
A: 'ANSYS User Discussion List' <email address suppressed>
> Hi there,
>
> Here I come once again, now that I know that what I wanted to do is
> possible.
>
> I'll insert here the "simple" log file (at the end I used a simple
> body with
> just one element, to see where the problem could be), so maybe you can
> tell
> me where is the problem in my model, if in ansys or in the material model.
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


irantzu.uriarte User
Joined: 21 Oct 2008 Posts: 17

Posted: Fri May 22, 2009 4:41 am 


Dear José Manuel,
First of all, thanks for your answer.
1. I don't know what are you talking about in the 2. paragraph. Where does
appear that period of 860sec...?
2. Why not 3 independent meshes? Because that way I wouldn't be taking into
account the effect between each other, isn't it? I mean, I want the
deformation not to be "free", but related to the whole model.
Nevertheless, model's constants are wrongly introduced, as you have showed
me. (And I also have sent wrong the 2. model's part, because the aim was to
use linear elastic model instead of mooneyrivlin material with the
viscoelasticity...)
Thank you once again,
Irantzu
____________
PhD Student
EHU Spain
Mensaje original
De: email address suppressed [mailto:email address suppressed] En nombre
de email address suppressed
Enviado el: jueves, 21 de mayo de 2009 15:30
Para: ANSYS User Discussion List
Asunto: Re: [Xansys] About viscoelasticity + hyperelasticity
Dear Irantzu,
your third material is nearly incompressible, with a poisson ratio of 0.4999
. The mixed uP formulation is more robust (check Ansys manual) than the
displacement formulation.
The variation with time of your prescribed displacement does not correspond
with the 0.05*sin(1000*3.1416*{TIME}) that is written in the comment. By
looking at the displacements in the /post26 postprocessor
(/post26$nsol,2,3,u,z$plvar,2), the prescribed amplitude is 0.05, but the
frequency is not 3141.6rad/s (whose period would be 1/500seconds), but
7.306e3 rad/s (period=860 sec).
Instead of solving three overlapped meshes, perhaps it would help you to
solve three independent problems with only one mesh in each of them, and
check the results of each single model.
You are applying a maximum shear deformation of 0.05/10=0.005=0.5% (maximum
UZ displacement/thickness). At time=100 the shear deformation is
0.0335/10=0.00335=0.335%.
For the third material, your shear modulus is G=E/(2*(1+mu))=1/3, therefore
your shear stress is tauxz=1.67e3 , well within the linear regime
(fy/sqrt(3)=sqrt(3)=1.732>tauxz).
For your first material, the initial shear modulus is
G=2*c10=2*0.163498=0.327, and multiplying by the shear deformation at time
100 you obtain the following shear stress 0.327*0.00335=0.0011.
For your second material, the initial shear modulus is
G_0=2*(c10+c01)=2*(38.462E4+0)=769240, which is several orders of magnitude
bigger than the other two materials. The fraction of shear modulus that is
lost is G1=0.5*G_0, with a relaxation time of 2 seconds, therefore, at time
t, G(t)=G_0*0.5*(1+exp(t/2)). For t=infinity, the shear modulus is
G_inf=0.5*G_0. The relaxation time is much smaller that the period of your
excitation, therefore the response will be similar to that of a elastic
material with G=G_inf. Multiplying G_inf by the shear deformation at time
100, you obtain the following shear stress: 0.5*769240*0.00335=1288
When solving the three independent problems, the shear stress results are
very close to the values given above, except for the second material, where
Ansys does not converge. Ansys suggest ramped loading or modify the mesh. I
have used ramped loading (KBC,1), and still did not converge. By increasing
the relaxation time for bulk modulus
(TB,PRONY,2,1,1,BULK$TBTEMP,0$TBDATA,1,0.5,2000) to a large value (2000),
Ansys converged and the shear stresses were close to the value calculated
above.
When solving the problem with the three overlapped meshes, the same results
as for the three independent meshes are obtained. You have applied a
prescribed displacement on three "springs" (elements) in parallel.
I hope that this helps.
Best regards,
Jose M. Galan
Dept. Construction Engineering
University of Seville (Spain)
 Mensaje original 
De: Irantzu <email address suppressed>
Fecha: Jueves, Mayo 21, 2009 11:21 ombr
Asunto: Re: [Xansys] About viscoelasticity + hyperelasticity
A: 'ANSYS User Discussion List' <email address suppressed>
> Hi there,
>
> Here I come once again, now that I know that what I wanted to do is
> possible.
>
> I'll insert here the "simple" log file (at the end I used a simple
> body with
> just one element, to see where the problem could be), so maybe you can
> tell
> me where is the problem in my model, if in ansys or in the material model.
++
 XANSYS web  www.xansys.org/forum 
 XANSYS blog  xansys.blogspot.com 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to email address suppressed 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Fri May 22, 2009 10:24 am 


Dear Irantzu,
With respect to the period of the excitation: after executing your macro, I obtained the UZ displacements of node 3 in the timehistory postprocessor (/post26) with the following commands: /post26$nsol,2,3,u,z$prvar,2
Node 3 belongs to area 5, where prescribed UZ displacements were applied using a function. The displacements are listed below:
TIME 3 UZ
uz3
1 3.67E04
2 7.35E04
4 1.47E03
8 2.94E03
16 5.86E03
26 9.49E03
36 1.31E02
46 1.66E02
56 2.00E02
66 2.33E02
76 2.65E02
86 2.95E02
96 3.24E02
100 3.35E02
Is there any difference with what you obtain?
By plotting those results in excel, it seemed the begining of a sine variation, but it did not even reach the first peak (therefore, 100 was less than 0.25*period). I increased the time, until I saw a full cycle; that time, 860, was the period of the excitation.
With respecto to the overlapped meshes: I am not an expert in material models. I guess that the material behaviour that you are trying to model is not simple, and that is why you use three overlapped meshes. I find it easier to understand simpler models, before proceeding to the complex ones, that is why I suggested looking at the independent meshes first (before proceeding to the three overlapped meshes).
With my email I did not mean that the material constans that you used were wrong, I am not an expert on those materials. I just wanted to analyze the results, by checking the shear stresses obtained with Ansys with some simple hand calculated values (I assumed that your plate was approximately under pure constant shear). The agreement was quite good, and I wanted to share it with you.
The analysis did converge when using only one mesh, except for the viscoelastic material (material 2). The analysis did not converge with the three overlapped meshes either. The change that I did in the relaxation time of the bulk modulus wass quite arbitrary and it could even be unrealistic for your material! You should use the material parameters that you have obtained from experiments or from the literature.
I hope that you find it helpful.
Best regards
Jose M. Galan
Dept. Construction Engineering
University of Seville (Spain)
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 




You cannot post new topics in this forum You cannot reply to topics in this forum You cannot edit your posts in this forum You cannot delete your posts in this forum You cannot vote in polls in this forum You cannot attach files in this forum You cannot download files in this forum

