Author 
Message 
ilhan.tuncoz User
Joined: 23 Nov 2013 Posts: 33

Posted: Fri Jun 20, 2014 1:39 am 


Dear All,
I am using ANSYS Workbench v14 as a finite element solver. I am given a set of material properties to model a composite material.
Properties that I have are:
E11, E22, NU12, G12, G13, G23 and density.
When I try to model this material in ANSYS, I go to engineering data and create a new material with linear orthotropic elastic model. However, It requires 9 material parameters, yet, I only have 6 parameter.
How can I model my material properly with my given 6 parameters. I will use the material in shell elements.
Thanks in advance, _________________ Ilhan Ozan Tuncoz
Aerospace Engineer, M. Sc.
Middle East Technical University  Turkey 

Back to top 


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

Posted: Fri Jun 20, 2014 4:13 am 


Dear Mr. Tuncoz,
Each layer of a composite laminate is transversely isotropic (5
independent material constants) rather than orthotropic (9 independent
material constants). However, in ansys you only have the option of
defining orthotropic materiales. Therefore, you have to calculate the
remaining 4 dependent constants from your 5 independent constants.
In the ansys help () you can find the following information about
orthotropic material constants:
"If the material is orthotropic:
EX, EY, EZ, (PRXY, PRYZ, PRXZ, or NUXY, NUYZ, NUXZ), GXY, GYZ, and GXZ
must all be input if the element type uses the material property. There
are no defaults. For example, if only EX and EY are input (with
different values) to a plane stress element, The program generates an
error message indicating that the material is orthotropic and that GXY
and NUXY are also needed."
That means that Ansys requires you to define 9 constants, as I mentioned
above.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 10:39, ilhan.tuncoz escribió:
Quote:  Dear All,
I am using ANSYS Workbench v14 as a finite element solver. I am given a set of material properties to model a composite material.
Properties that I have are:
E11, E22, NU12, G12, G13, G23 and density.
When I try to model this material in ANSYS, I go to engineering data and create a new material with linear orthotropic elastic model. However, It requires 9 material parameters, yet, I only have 6 parameter.
How can I model my material properly with my given 6 parameters. I will use the material in shell elements.
Thanks in advance,

Ilhan Ozan Tuncoz
Aerospace Engineer
Middle East Technical University  Turkey
++
 XANSYS web  www.xansys.org/forum [3] 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com [4] 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++

Links:

[1] http://www.mail2forum.com
[2] http://xansys.org/forum/viewtopic.php?p=94575#94575
[3] http://www.xansys.org/forum
[4] http://www.padtinc.com
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


p.barrett User
Joined: 07 Oct 2013 Posts: 41

Posted: Fri Jun 20, 2014 4:14 am 


Ilhan,
You will have to make some assumptions for the missing data such as a
similar Poisson's ratio in 2 directions, but given the data you have you can
compute the other terms using a form of the following equation (isotropic
formula):
E=G*2*(1+NU)
Take a look at any solid mechanics text book for the full set of equations
for orthotropic properties.
Peter Barrett, P.E.
CAE Associates, Inc.
www.caeai.com
Original Message
From: Xansys [mailto:xansysbounces@xansys.org] On Behalf Of ilhan.tuncoz
Sent: Friday, June 20, 2014 4:39 AM
To: xansys@xansys.org
Subject: [Xansys] 2D Orthotropic Material Workbench
Dear All,
I am using ANSYS Workbench v14 as a finite element solver. I am given a set
of material properties to model a composite material.
Properties that I have are:
E11, E22, NU12, G12, G13, G23 and density.
When I try to model this material in ANSYS, I go to engineering data and
create a new material with linear orthotropic elastic model. However, It
requires 9 material parameters, yet, I only have 6 parameter.
How can I model my material properly with my given 6 parameters. I will use
the material in shell elements.
Thanks in advance,

Ilhan Ozan Tuncoz
Aerospace Engineer
Middle East Technical University  Turkey
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This email is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this email, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this email and any of its attachments is strictly prohibited and may be unlawful. If you have received this email in error, please notify the sender immediately and permanently delete the original email and destroy any copies or printouts of this email as well as any attachments.
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


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

Posted: Fri Jun 20, 2014 6:13 am 


In my previous meail I meant 5 independent ELASTIC constants and 9
independent ELASTIC constants.
Density must be defined additionally, but it does not influence the
constitutive matrix of the material.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 13:13, mfernan@us.es escribió:
Quote:  Dear Mr. Tuncoz,
Each layer of a composite laminate is transversely isotropic (5
independent material constants) rather than orthotropic (9 independent
material constants). However, in ansys you only have the option of
defining orthotropic materiales. Therefore, you have to calculate the
remaining 4 dependent constants from your 5 independent constants.
In the ansys help () you can find the following information about
orthotropic material constants:
"If the material is orthotropic:
EX, EY, EZ, (PRXY, PRYZ, PRXZ, or NUXY, NUYZ, NUXZ), GXY, GYZ, and GXZ
must all be input if the element type uses the material property. There
are no defaults. For example, if only EX and EY are input (with
different values) to a plane stress element, The program generates an
error message indicating that the material is orthotropic and that GXY
and NUXY are also needed."
That means that Ansys requires you to define 9 constants, as I mentioned
above.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 10:39, ilhan.tuncoz escribió:
Quote:  Dear All, I am using ANSYS Workbench v14 as a finite element solver. I am given a set of material properties to model a composite material. Properties that I have are: E11, E22, NU12, G12, G13, G23 and density. When I try to model this material in ANSYS, I go to engineering data and create a new material with linear orthotropic elastic model. However, It requires 9 material parameters, yet, I only have 6 parameter. How can I model my material properly with my given 6 parameters. I will use the material in shell elements. Thanks in advance,  Ilhan Ozan Tuncoz Aerospace Engineer Middle East Technical University  Turkey  m2f  Sent using Mail2Forum (http://www.mail2forum.com [1] [1]). Read this topic online here: http://xansys.org/forum/viewtopic.php?p=94575#94575 [2] [2]  m2f  ++  XANSYS web  www.xansys.org/forum [3]

 [3]   The Online Community for users of ANSYS, Inc. Software   Hosted by PADT  www.padtinc.com [4] [4]   Send administrative requests to xansysmod@tynecomp.co.uk  ++
Links:

[1] http://www.mail2forum.com
[2] http://xansys.org/forum/viewtopic.php?p=94575#94575
[3] http://www.xansys.org/forum
[4] http://www.padtinc.com
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


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

Posted: Fri Jun 20, 2014 8:13 am 


Dear Mr. Tuncoz:
if your material is fully orthotropic, you should also know E33, nu13
and nu32.
However, I would like to ask you about the known values of the three
shear modulus of your material, G12, G13, G23. Are they all three
different from each other? If two of them have the same value, then you
have a transversely isotropic material, not a fully orthotropic one. As
I mentioned previously, you have the 5 independent elastic constants
that define the material completely.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 15:13, mfernan@us.es escribió:
Quote:  In my previous meail I meant 5 independent ELASTIC constants and 9
independent ELASTIC constants.
Density must be defined additionally, but it does not influence the
constitutive matrix of the material.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 13:13, mfernan@us.esescribió:
Dear Mr. Tuncoz, Each layer of a composite laminate is transversely isotropic (5 independent material constants) rather than orthotropic (9 independent material constants). However, in ansys you only have the option of defining orthotropic materiales. Therefore, you have to calculate the remaining 4 dependent constants from your 5 independent constants. In the ansys help () you can find the following information about orthotropic material constants: "If the material is orthotropic: EX, EY, EZ, (PRXY, PRYZ, PRXZ, or NUXY, NUYZ, NUXZ), GXY, GYZ, and GXZ must all be input if the element type uses the material property. There are no defaults. For example, if only EX and EY are input (with different values) to a plane stress element, The program generates an error message indicating that the material is orthotropic and that GXY and NUXY are also needed." That means that Ansys requires you to define 9 constants, as I mentioned above. Best regards, Jose M. Galan Constr. Engin. Dept. Univ.
 Sevilla Spain El 20/06/2014 10:39, ilhan.tuncoz escribió: Dear All, I am using ANSYS Workbench v14 as a finite element solver. I am given a set of material properties to model a composite material. Properties that I have are: E11, E22, NU12, G12, G13, G23 and density. When I try to model this material in ANSYS, I go to engineering data and create a new material with linear orthotropic elastic model. However, It requires 9 material parameters, yet, I only have 6 parameter. How can I model my material properly with my given 6 parameters. I will use the material in shell elements. Thanks in advance,  Ilhan Ozan Tuncoz Aerospace Engineer Middle East Technical University  Turkey  m2f  Sent using Mail2Forum
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


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

Posted: Fri Jun 20, 2014 8:30 am 


If the plane x2x3 is a plane of isotropy, there are four relationships
between the 9 orthotropic constants:
E2=E3
G12=G13
nu12=nu13
G23=E2/(2*(1+nu23))
Please, read carefully how these elastic constants for orthotropic
materials are introduced in ansys. Be careful with Poisson's ratios;
there are only 3 independent values that need to be input from the 6
possible ratios (that ansys denotes as "major" Poisson's ratios, PRXY,
PRYZ AND PRXZ, and "minor" Poisson's ratios, NUXY,NUYZ,NUXZ). Also be
careful with the order of the tangential stress and strain components in
the stress and strain vectors; in ansys they are stored as
[sigmax, sigmay, sigmaz, sigmaxy, sigmayz, sigmazz]^T
while in the literature they are usually stored as
[sigma1, sigma2, sigma3, sigma23, sigma31, sigma12]^T
Notice that shear stresses are ordered differently.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 17:13, mfernan@us.es escribió:
Quote:  Dear Mr. Tuncoz:
if your material is fully orthotropic, you should also know E33, nu13
and nu32.
However, I would like to ask you about the known values of the three
shear modulus of your material, G12, G13, G23. Are they all three
different from each other? If two of them have the same value, then you
have a transversely isotropic material, not a fully orthotropic one. As
I mentioned previously, you have the 5 independent elastic constants
that define the material completely.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
El 20/06/2014 15:13, mfernan@us.esescribió:
Quote:  In my previous meail I meant 5 independent ELASTIC constants and 9 independent ELASTIC constants. Density must be defined additionally, but it does not influence the constitutive matrix of the material. Best regards, Jose M. Galan Constr. Engin. Dept. Univ. Sevilla Spain El 20/06/2014 13:13, mfernan@us.esescribió: Dear Mr. Tuncoz, Each layer of a composite laminate is transversely isotropic (5 independent material constants) rather than orthotropic (9 independent material constants). However, in ansys you only have the option of defining orthotropic materiales. Therefore, you have to calculate the remaining 4 dependent constants from your 5 independent constants. In the ansys help () you can find the following information about orthotropic material constants: "If the material is orthotropic: EX, EY, EZ, (PRXY, PRYZ, PRXZ, or NUXY, NUYZ, NUXZ), GXY, GYZ, and GXZ must all be input if the element type uses the material property. There are no defaults. For example, if only EX and EY

 are input (with different values) to a plane stress element, The program generates an error message indicating that the material is orthotropic and that GXY and NUXY are also needed." That means that Ansys requires you to define 9 constants, as I mentioned above. Best regards, Jose M. Galan Constr. Engin. Dept. Univ.
Quote: 
Sevilla Spain El 20/06/2014 10:39, ilhan.tuncoz escribió: Dear All, I am using ANSYS Workbench v14 as a finite element solver. I am given a set of material properties to model a composite material. Properties that I have are: E11, E22, NU12, G12, G13, G23 and density. When I try to model this material in ANSYS, I go to engineering data and create a new material with linear orthotropic elastic model. However, It requires 9 material parameters, yet, I only have 6 parameter. How can I model my material properly with my given 6 parameters. I will use the material in shell elements. Thanks in advance,  Ilhan Ozan Tuncoz Aerospace Engineer Middle East Technical University  Turkey  m2f  Sent using Mail2Forum
++
 XANSYS web  www.xansys.org/forum [1] 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com [2] 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++

Links:

[1] http://www.xansys.org/forum
[2] http://www.padtinc.com
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


ilhan.tuncoz User
Joined: 23 Nov 2013 Posts: 33

Posted: Wed Jul 02, 2014 12:41 am 


Dear all,
I apologize for giving such a late response. I thank to all who answered.
Unfortunately, my G12, G13, G23 have different values from each other.
When I assume a transversely isotropic properties and calculate the nu23 accordingly (assuming E33 = E22);
I end up with a poisson ratio which is greater than 3, while others are around 0.2.
I know that PATRAN has 2D orthotropic entry option, but ANSYS do not allow such input... _________________ Ilhan Ozan Tuncoz
Aerospace Engineer, M. Sc.
Middle East Technical University  Turkey 

Back to top 


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

Posted: Wed Jul 02, 2014 4:23 am 


Dear Mr. Tuncoz,
From your comments, it is clear that your material is not transversely
isotropic.
In the MSC Nastran 2004 Reference Manual
(http://simcompanion.mscsoftware.com/infocenter/index?page=content&id=DOC9188),
page 276, you can find the stressstrain constitutive matrix of a 2D
orthotropic material:
eps=C*sigma
which has 6 independent material constants.
By comparing it with the constitutive matrix of a 3D orthotropic
material with 9 independent material constants (for example, in the
Ansys manual, equation (24), Mechanical APDL>Theory
Reference>2.Structures >2.1 Structural Fundamentals), you can see that
the only difference is that in the 2D orthotropic material it is assumed
that sigma_z is zero. This is the assumption used for the formulation of
shell elements (with z being the direction normal to the shell
midplane). In that case, three material constants (Ez, nuxz and nuyz)
are multiplied by zero, and they do not have any influence on the
results (which may be the reason behind the the Nastran 2d orthotropic
material model).
If you want to use the Ansys 3D orthotropic material, you will need to
introduce those three material constants. You should calculate them by
making some assumption.
If the 3d orthotropic material is used on a shell element, the normal
stresses sigma_z (stress component normal to the shell mid surface;
a.k.a. throughthickness stress) that will multiply the assumed
constants (Ez, nuxz, nuyz) will be zero (see SHELL181 assumptions and
restrictions), and thus the assummed constants will not have any
influence on your results.
A possible assumption would be that the deformations in the xz plane of
the material under uniaxial traction in z direction are the same as the
deformations in the xy plane under uniaxial traction in the y direction.
This assumption provides two equations:
Ez=Ey (with Ey<Ex, where Ey and Ex are the two young Modulus of the 2d
orthotropic material)
nuxz=nuxy
You still need the poisson ratio in the plane yz, nuyz. You could make
the assumption of an isotropic that under shear deformation in the yz
plane, :
Gyz=Ey/(2*(1+nuyz))
Thus, you can calculate nuyz as nuyz=Ey/(2*Gyz)1
The abovementioned assumptions are almost the same as for a transversely
isotropic material, but with only one difference: the shear moduli in
the planes xy and xz are different in this case (while in the
transversely isotropic material they are equal).
Remember that you may obtain negative values for nuyz, or values above
0.5.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Univ. Sevilla
Spain
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


ilhan.tuncoz User
Joined: 23 Nov 2013 Posts: 33

Posted: Wed Jul 02, 2014 5:36 am 


Dear Mr. Galan,
Thank you for your extensive and comprehensive answer. The references that you give worked perfectly fine.
I also checked the SHELL181 Assumptions and Restrictions. You are right that throughthickness, SZ, is always zero. However, you should note that there is no assumption regarding strain in Z direction. Therefore, SHELL181 element produces strain in Z direction.
If you look at Equation 2.4, you will note that due the assumption, third column of the constitutive matrix will be zero column. However, third row of the matrix, will not be zero since first two terms in the third row will be multiplied with sigmaX and sigmaY in order to calculate epsilonZ.
However, please note that, my unknown constants will only affect the results in epsilonZ and other parameters will be calculated exactly. In other words, in PATRAN 2D orthotropic constitutive matrix is 5x5 (eliminating epsZ and sigmaZ) while in ANSYS for SHELL181 element orthotopic constitutive matrix is 6x5 (eliminating sigmaZ but retaining epsZ).
In our case, epsilonZ is not an important parameter for the analysis so it works perfectly well.
I again would like to present my profound thanks to you. _________________ Ilhan Ozan Tuncoz
Aerospace Engineer, M. Sc.
Middle East Technical University  Turkey 

Back to top 


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

Posted: Wed Jul 02, 2014 5:40 am 


Thank you for the feedback.
Best regards,
Jose M. Galan
Constr. Eng. Dept.
Univ. Sevilla
Spain
El 02/07/2014 14:36, ilhan.tuncoz escribió:
Quote:  Dear Mr. Galan,
Thank you for your extensive and comprehensive answer. The references that you give worked perfectly fine.
I also checked the SHELL181 Assumptions and Restrictions. You are right that throughthickness, SZ, is always zero. However, you should note that there is no assumption regarding strain in Z direction. Therefore, SHELL181 element produces strain in Z direction.
If you look at Equation 2.4, you will note that due the assumption, third column of the constitutive matrix will be zero column. However, third row of the matrix, will not be zero since first two terms in the third row will be multiplied with sigmaX and sigmaY in order to calculate epsilonZ.
However, please note that, my unknown constants will only affect the results in epsilonZ and other parameters will be calculated exactly. In other words, in PATRAN 2D orthotropic constitutive matrix is 5x5 (eliminating epsZ and sigmaZ) while in ANSYS for SHELL181 element orthotopic constitutive matrix is 6x5 (eliminating sigmaZ but retaining epsZ).
In our case, epsilonZ is not an important parameter for the analysis so it works perfectly well.
I again would like to present my profound thanks to you.

Ilhan Ozan Tuncoz
Aerospace Engineer
Middle East Technical University  Turkey
++
 XANSYS web  www.xansys.org/forum [3] 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com [4] 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++

Links:

[1] http://www.mail2forum.com
[2] http://xansys.org/forum/viewtopic.php?p=94703#94703
[3] http://www.xansys.org/forum
[4] http://www.padtinc.com
++
 XANSYS web  www.xansys.org/forum 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++
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

