poroelastic material model in ANSYS
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html) and
add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have considered
large displacements in your static analysis, which may distort the
elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the simplest
problem, with an analytical solution that you can find in any Soil
Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2, where
t is in s, and Hdr is the drainage length in meters. In the simple 1D
consolidation case studied by Terzaghi, with permeable top and
impermeable bottom (same as VM264), Hdr=H, with H the sample height
(notice that I am using soil terminology, with H being the height of the
soil "sample" in the 1D oedometer test). In the expresssion of cv,
gammaw=rhowg is the specific weight of the fluid in N/m^3, rhow is the
density of the fluid in kg/m^3, g is the acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of permeability
in m/s, and D in Pa is the oedometric modulus of deformation 1D or 1D
constrained modulus, which for an isotropic linear elastic materil is
D=E(1-nu)/((1+nu)(1+2nu)), see equation (14.16) in Arnold Verruijt's
"Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time, according
to Darcy's law. For example, if the specific weight of the fluid is not
defined (TBOPT = FP), it is assumed to be 1 in the corresponding unit
used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list
Dear Professor Galan,
Thank you for the useful information.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html) and
add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have considered
large displacements in your static analysis, which may distort the
elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the simplest
problem, with an analytical solution that you can find in any Soil
Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2, where
t is in s, and Hdr is the drainage length in meters. In the simple 1D
consolidation case studied by Terzaghi, with permeable top and
impermeable bottom (same as VM264), Hdr=H, with H the sample height
(notice that I am using soil terminology, with H being the height of the
soil "sample" in the 1D oedometer test). In the expresssion of cv,
gammaw=rhowg is the specific weight of the fluid in N/m^3, rhow is the
density of the fluid in kg/m^3, g is the acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of permeability
in m/s, and D in Pa is the oedometric modulus of deformation 1D or 1D
constrained modulus, which for an isotropic linear elastic materil is
D=E(1-nu)/((1+nu)(1+2nu)), see equation (14.16) in Arnold Verruijt's
"Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time, according
to Darcy's law. For example, if the specific weight of the fluid is not
defined (TBOPT = FP), it is assumed to be 1 in the corresponding unit
used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Hello Prof Galan,
Just a follow up question, Is that we can do poroelastic analysis only
in ANSYS classic. As I can only simulate the model in Classic not in
Workbench. I was trying to find if its mentioned somewhere explicitly,
but can't find. So please let me know if we can run the simulation in
WORKBENCH also.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting PRITI priti@mech.kth.se:
Dear Professor Galan,
Thank you for the useful information.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html) and
add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have considered
large displacements in your static analysis, which may distort the
elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the simplest
problem, with an analytical solution that you can find in any Soil
Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2, where
t is in s, and Hdr is the drainage length in meters. In the simple 1D
consolidation case studied by Terzaghi, with permeable top and
impermeable bottom (same as VM264), Hdr=H, with H the sample height
(notice that I am using soil terminology, with H being the height of the
soil "sample" in the 1D oedometer test). In the expresssion of cv,
gammaw=rhowg is the specific weight of the fluid in N/m^3, rhow is the
density of the fluid in kg/m^3, g is the acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of permeability
in m/s, and D in Pa is the oedometric modulus of deformation 1D or 1D
constrained modulus, which for an isotropic linear elastic materil is
D=E(1-nu)/((1+nu)(1+2nu)), see equation (14.16) in Arnold Verruijt's
"Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time, according
to Darcy's law. For example, if the specific weight of the fluid is not
defined (TBOPT = FP), it is assumed to be 1 in the corresponding unit
used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS
to xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Dear Priti,
You can do it in Mechanical APDL. I do not know if it can be done in
workbench.
Perhaps you may try a similar approach as the one shown in this
presentation by R. Silva:
http://www.esss.com.br/events/ansys2013/brazil/pdf/25_2_1700.pdf
He uses APDL commands to perform a direct coupled thermal-structural
analysis in ANSYS WorkBench. With APDL commands, he changes the element
type to PLANE223 and he also applies thermal boundary conditions.
I am not sure if this will also work for CPT212 elements.
In addition, this approach requires a good knowledge of APDL commands. I
would only recommend using it when you are already familiar with solving
poroelastic models in Mechanical APDL.
Best regards,
Jose M. Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 20/04/2017 21:29, PRITI escribió:
Hello Prof Galan,
Just a follow up question, Is that we can do poroelastic analysis only in ANSYS classic. As I can only simulate the model in Classic not in Workbench. I was trying to find if its mentioned somewhere explicitly, but can't find. So please let me know if we can run the simulation in WORKBENCH also.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
By googling I found this paper by Chung and Mansour:
They solve some poroelastic problems with CPT213 in Mechanical APDL.
They compare their numerical results with several references. In
Appendix 1 they include an APDL script.
Regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 20/04/2017 21:29, PRITI escribió:
Hello Prof Galan,
Just a follow up question, Is that we can do poroelastic analysis only in ANSYS classic. As I can only simulate the model in Classic not in Workbench. I was trying to find if its mentioned somewhere explicitly, but can't find. So please let me know if we can run the simulation in WORKBENCH also.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting PRITI priti@mech.kth.se:
Dear Professor Galan,
Thank you for the useful information.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html) and
add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have considered
large displacements in your static analysis, which may distort the
elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the simplest
problem, with an analytical solution that you can find in any Soil
Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2, where
t is in s, and Hdr is the drainage length in meters. In the simple 1D
consolidation case studied by Terzaghi, with permeable top and
impermeable bottom (same as VM264), Hdr=H, with H the sample height
(notice that I am using soil terminology, with H being the height of the
soil "sample" in the 1D oedometer test). In the expresssion of cv,
gammaw=rhowg is the specific weight of the fluid in N/m^3, rhow is the
density of the fluid in kg/m^3, g is the acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of permeability
in m/s, and D in Pa is the oedometric modulus of deformation 1D or 1D
constrained modulus, which for an isotropic linear elastic materil is
D=E(1-nu)/((1+nu)(1+2nu)), see equation (14.16) in Arnold Verruijt's
"Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time, according
to Darcy's law. For example, if the specific weight of the fluid is not
defined (TBOPT = FP), it is assumed to be 1 in the corresponding unit
used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single email
per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Thank you Prof Galan!
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
By googling I found this paper by Chung and Mansour:
They solve some poroelastic problems with CPT213 in Mechanical APDL.
They compare their numerical results with several references. In
Appendix 1 they include an APDL script.
Regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 20/04/2017 21:29, PRITI escribió:
Hello Prof Galan,
Just a follow up question, Is that we can do poroelastic analysis
only in ANSYS classic. As I can only simulate the model in Classic
not in Workbench. I was trying to find if its mentioned somewhere
explicitly, but can't find. So please let me know if we can run
the simulation in WORKBENCH also.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting PRITI priti@mech.kth.se:
Dear Professor Galan,
Thank you for the useful information.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html) and
add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have considered
large displacements in your static analysis, which may distort the
elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the simplest
problem, with an analytical solution that you can find in any Soil
Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2, where
t is in s, and Hdr is the drainage length in meters. In the simple 1D
consolidation case studied by Terzaghi, with permeable top and
impermeable bottom (same as VM264), Hdr=H, with H the sample height
(notice that I am using soil terminology, with H being the height of the
soil "sample" in the 1D oedometer test). In the expresssion of cv,
gammaw=rhowg is the specific weight of the fluid in N/m^3, rhow is the
density of the fluid in kg/m^3, g is the acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of permeability
in m/s, and D in Pa is the oedometric modulus of deformation 1D or 1D
constrained modulus, which for an isotropic linear elastic materil is
D=E(1-nu)/((1+nu)(1+2nu)), see equation (14.16) in Arnold Verruijt's
"Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time, according
to Darcy's law. For example, if the specific weight of the fluid is not
defined (TBOPT = FP), it is assumed to be 1 in the corresponding unit
used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to static
load and load with certain time period or frequency. As this analysis
considers the time effect I am planning to model the cartilage as
POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in all
direction. The vertical downward force (0.02N) was applied on some nodes of
the top surface. I chose the element CPT217 (element type recommended in
ANSYS HELP for porous material). The material was defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I make sure
about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS
to xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single email
per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Hello Prof Galan and XANSYS group,
I need help with some basic questions regarding poro-elastic material analysis in ANSYS.
In ANSYS for poroelastic material we need to use the CPTXXX elements. I was checking the outcome variables for CPT elements (In ANSYS 16.0 Manual) and there is no option for pore pressure, volume void ratio.
The below mentioned link suggests for PRESOL,PMSV,
https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_cmd/Hlp_C_PRESOL.html
However, this command is not working and ANSYS showing the error message ''PMSV item is invalid''
I am interested in below mentioned results:
a. pore pressure
b. pressure on solid matrix.
c. Total hydrostatic pressure (which is sum of Pore Pressure and Pressure on Solid Matrix)
d. Octahedral shear stress (which I guess can be computed using principal stresses S1,S2 and S3)
e. fluid volume ratio
Please suggest me how can I extract these results.
Looking forward to hearing from you soon.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
-----Original Message-----
From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of PRITI
Sent: den 21 april 2017 08:02
To: XANSYS Mailing List Temporary Home
Subject: Re: [Xansys] poroelastic material model in ANSYS
Thank you Prof Galan!
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
By googling I found this paper by Chung and Mansour:
https://www.researchgate.net/publication/244478311_Application_of_ANSY
S_to_the_Stress_Relaxation_of_Articular_Cartilage_in_Unconfined_Compre
ssion
They solve some poroelastic problems with CPT213 in Mechanical APDL.
They compare their numerical results with several references. In
Appendix 1 they include an APDL script.
Regards,
Jose M Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 20/04/2017 21:29, PRITI escribió:
Hello Prof Galan,
Just a follow up question, Is that we can do poroelastic analysis
only in ANSYS classic. As I can only simulate the model in Classic
not in Workbench. I was trying to find if its mentioned somewhere
explicitly, but can't find. So please let me know if we can run the
simulation in WORKBENCH also.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting PRITI priti@mech.kth.se:
Dear Professor Galan,
Thank you for the useful information.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Quoting mfernan@us.es:
Dear Priti,
you should follow the forum rules (http://www.xansys.org/rules.html)
and add a signature in all your messages, stating "your full name and
company (or university) affiliation".
In numerical models you should always start simple. First solve the
linear problem, excluding geometric nonlinearities. You have
considered large displacements in your static analysis, which may
distort the elements so much that the may turn inside out.
You only describe the structural boundary conditions that you have
applied, but for poroelastic materials you should also add boundary
conditions for the fluid. If you do not apply any bc for the fluid,
impermeable boundaries are assumed. You should check if those are
adequate in your particular problem.
In the verification manual there are three examples of poroelastic
problems that you may find very helpful: VM260 , VM264 and VM295.
I strongly recommend you to start with VM264, "Terzaghi's
One-Dimensional Consolidation Settlement Problem", which is the
simplest problem, with an analytical solution that you can find in
any Soil Mechanics book, such as Arnold Verruijt's "Soil Mechanics"
(http://geo.verruijt.net/software/SoilMechBook2012.pdf) or Braja M.
Das's "Principles of Geotechnical Engineering". Terzaghi's field of
study was soil mechanics, and yours is biomechanics, but both use a
poroelastic model. In Terzaghi's problem, the coefficient of
consolidation cv=kD/gammaw , in m^2/s, determines the time rate of
consolidation, through the dimensionless parameter Tv=cvt/Hdr^2,
where t is in s, and Hdr is the drainage length in meters. In the
simple 1D consolidation case studied by Terzaghi, with permeable top
and impermeable bottom (same as VM264), Hdr=H, with H the sample
height (notice that I am using soil terminology, with H being the
height of the soil "sample" in the 1D oedometer test). In the
expresssion of cv, gammaw=rhowg is the specific weight of the fluid
in N/m^3, rhow is the density of the fluid in kg/m^3, g is the
acceleration of gravity in
m/s^3 (for water, rhow=1000 kg/m3, and g=9.81m/s^2, thus gammaw=9810
N/m3, or approximately 10^4 N/m^3), k is the coefficient of
permeability in m/s, and D in Pa is the oedometric modulus of
deformation 1D or 1D constrained modulus, which for an isotropic
linear elastic materil is D=E(1-nu)/((1+nu)(1+2nu)), see equation
(14.16) in Arnold Verruijt's "Soil Mechanics" book.
Regarding the units of permeability, you should be aware of the
following section of TFM ("the fine manual"):
"4.10.3.8. Units of Permeability
The units of permeability are always defined as Length/Time,
according to Darcy's law. For example, if the specific weight of the
fluid is not defined (TBOPT = FP), it is assumed to be 1 in the
corresponding unit used in the solution as Force/Length3."
In the examples of the verification manual the specific weight of the
fluid is not defined. Thus, it is assumed to be 1. In the APDL input
files, instead of introducing the permeabilities k in m/s, the values
khat=k/gammaw in m^4/(Ns) are introduced. The coefficient of
consolidation is calculated as cv=khatD.
Best regards,
El 04/04/2017 19:20, PRITI YADAV escribió:
Hello all,
For my project work, I need to analyze the effect of load timing on
cartilage stresses i.e. what happens if cartilage is subjected to
static load and load with certain time period or frequency. As this
analysis considers the time effect I am planning to model the
cartilage as POROELASTIC MATERIAL.
Just to start with I modeled a simple block and fixed it's bottom in
all direction. The vertical downward force (0.02N) was applied on
some nodes of the top surface. I chose the element CPT217 (element
type recommended in ANSYS HELP for porous material). The material was
defined as given below
E1=6
MP,EX,1,E1
MP,NUXY,1,0.4
fpx1=3e-4
TB,PM,1,,,perm
TBDATA,1,fpx1,fpx1,fpx1
The solver setting was
Analysis type : static
Analysis option : Large displacement static
Time at end of loadstep: 1
Time increment: time step size : 0.1, minimum time step: 0.1, maximum
time
step: 1
NROPT: Full N-R unsymm
The simulation is getting out because of the error that ' element xxx
(CPT217) is turning inside out'
Please someone help me to resolve this issue
Also can I solve this problem in ANSYS workbench? If so how can I
make sure about the ELEMENT TYPE?
Looking forward to hearing from you soon.
Have a nice day!
Thanks & Regards
Priti
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS
to xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider
changing account settings to Digest mode which will send a single
email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list
Dear Mr. Yadav,
In your post you ask how to obtain five different results, but you do
not seem to know (or notice) that ansys may be using different names for
those quantities. For example:
- Pore pressure --> pressure degree of freedom (PRES)
- Total hydrostatic pressure (which is sum of Pore Pressure and Pressure
on Solid Matrix) --> total stress (or, simply, stress). In 2D: SX,
SY,SXY,SZ - Pressure on solid matrix --> efective stress. In 2D: ESIG,X ESIG,Y
ESIG,XY ESIG,Z
The only way to notice is by carefully reading the manual, including
element description, underlying theory, material properties, analysis
types, commands, etc. You should also check the examples in the
verification manual.
Pore pressure is the pressure nodal degree of freedom (PRES) of CPTxxx
elements, as you may find in the help (for instance, CPT212,
help/ans_elem/Hlp_E_CPT212.html). To plot the pore pressure results, use
PLNSOL,PRES . By the way, this command is used in VM264.
The stresses (total and effective) are calculated in the elements and
are plotted with PLESOL. The stresses (SX,SY,SXY) are total stresses.
You will find that information in the manual:
help/ans_cou/Hlp_G_COU_porefluiddiffstruct.html#couCPTelems
"Example: PRESOL,ESIG,Z prints the effective stress in the Z direction,
and PRESOL,S,Z prints the total stress in the Z direction."
help/ans_mat/elemdatatblpor.html
The command PRESOL,PMSV, is incomplete. You need to specify an
additional argument, which can be PPRES,VRAT,DSAT or RPER, to obtain
pore pressure, void volume ratio, degree of saturation or relative
permeability, respectively. For example, you can plot the pore pressure
in the elements with:
PLESOL,PMSV,PPRES
This plot will be the same as PLNSOL,PRES
Best regards,
Jose M. Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 03/05/2017 14:22, PRITI YADAV escribió:
Hello Prof Galan and XANSYS group,
I need help with some basic questions regarding poro-elastic material
analysis in ANSYS.
In ANSYS for poroelastic material we need to use the CPTXXX elements.
I was checking the outcome variables for CPT elements (In ANSYS 16.0
Manual) and there is no option for pore pressure, volume void ratio.
The below mentioned link suggests for PRESOL,PMSV,
https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_cmd/Hlp_C_PRESOL.html
However, this command is not working and ANSYS showing the error
message ''PMSV item is invalid''
I am interested in below mentioned results:
a. pore pressure
b. pressure on solid matrix.
c. Total hydrostatic pressure (which is sum of Pore Pressure and
Pressure on Solid Matrix)
d. Octahedral shear stress (which I guess can be computed using
principal stresses S1,S2 and S3)
e. fluid volume ratio
Please suggest me how can I extract these results.
Looking forward to hearing from you soon.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Thank you Prof Galan!
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
-----Original Message-----
From: mfernan@us.es [mailto:mfernan@us.es]
Sent: den 3 maj 2017 18:14
To: XANSYS Mailing List Temporary Home
Subject: Re: [Xansys] poroelastic material model in ANSYS
Dear Mr. Yadav,
In your post you ask how to obtain five different results, but you do not seem to know (or notice) that ansys may be using different names for those quantities. For example:
- Pore pressure --> pressure degree of freedom (PRES)
- Total hydrostatic pressure (which is sum of Pore Pressure and Pressure on Solid Matrix) --> total stress (or, simply, stress). In 2D: SX, SY,SXY,SZ
- Pressure on solid matrix --> efective stress. In 2D: ESIG,X ESIG,Y
ESIG,XY ESIG,Z
The only way to notice is by carefully reading the manual, including element description, underlying theory, material properties, analysis types, commands, etc. You should also check the examples in the verification manual.
Pore pressure is the pressure nodal degree of freedom (PRES) of CPTxxx elements, as you may find in the help (for instance, CPT212, help/ans_elem/Hlp_E_CPT212.html). To plot the pore pressure results, use PLNSOL,PRES . By the way, this command is used in VM264.
The stresses (total and effective) are calculated in the elements and are plotted with PLESOL. The stresses (SX,SY,SXY) are total stresses.
You will find that information in the manual:
help/ans_cou/Hlp_G_COU_porefluiddiffstruct.html#couCPTelems
"Example: PRESOL,ESIG,Z prints the effective stress in the Z direction, and PRESOL,S,Z prints the total stress in the Z direction."
help/ans_mat/elemdatatblpor.html
The command PRESOL,PMSV, is incomplete. You need to specify an additional argument, which can be PPRES,VRAT,DSAT or RPER, to obtain pore pressure, void volume ratio, degree of saturation or relative permeability, respectively. For example, you can plot the pore pressure in the elements with:
PLESOL,PMSV,PPRES
This plot will be the same as PLNSOL,PRES
Best regards,
Jose M. Galan
Assistant professor
Dpt. Enginering Construction
Univ. Sevilla
El 03/05/2017 14:22, PRITI YADAV escribió:
Hello Prof Galan and XANSYS group,
I need help with some basic questions regarding poro-elastic material
analysis in ANSYS.
In ANSYS for poroelastic material we need to use the CPTXXX elements.
I was checking the outcome variables for CPT elements (In ANSYS 16.0
Manual) and there is no option for pore pressure, volume void ratio.
The below mentioned link suggests for PRESOL,PMSV,
https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_cmd/Hlp_C_P
RESOL.html
However, this command is not working and ANSYS showing the error
message ''PMSV item is invalid''
I am interested in below mentioned results:
a. pore pressure
b. pressure on solid matrix.
c. Total hydrostatic pressure (which is sum of Pore Pressure and
Pressure on Solid Matrix) d. Octahedral shear stress (which I guess
can be computed using principal stresses S1,S2 and S3) e. fluid volume
ratio
Please suggest me how can I extract these results.
Looking forward to hearing from you soon.
Thanks & Regards
Priti Yadav
PhD Student
Mechanics Department
KTH, Stockholm
Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list