Large strain convergence issues.
I'm having difficulty modeling a thermoplastic material which is being used as a vibration damper. I want to do a static analysis to predict the deformed shape and stress in the damper from an assembly compression. I have lots of contact, NLGEOM,ON and gradually compressing the damper in multiple load steps (50 max). For the time being, I'm simulating this hyperelastic material as linear elastic with a very low modulus (roughly 4 orders of magnitude softer than the metal structure that is compressing it. I'm using solid 186's and 187's with reduced integration, keyopt(6)=1 for both. The damper geometry is rather complex so I'm meshing with tet's for most of it, but the main zone of compression uses 186's, but they ended up being 6 layers of degenerate penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied". ANSYS has problems when the total mechanical strain reaches ~15-20% or so. My questions are:
-
Is 15-20% strain a typical limit before rezoning is required? The rezoning feature in ANSYS is rather limited, so this will be a painful process if I have to manually rezone several times during the analysis. Does anyone have any experience with this to say what a typical level of strain you can get before rezoning is necessary? -
Also, I've tried relaxing the volumetric compatibility criteria a bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this criteria to use? How do you tell if this is relaxed too much? -
Is there any advantage to using unsymmetric matrices (NROPT, UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
Hi Joe,
Mileage varies on the strain thresholds, depending on the class of problem/geometry. Most anything can converge up to 10% -- about 1/2 our plastic deformation analyses will hit distortion errors around 15-20% that can't be overcome besides with remeshing/rezoning. I note, however, that simple test cases on a regular tet mesh of a beam in bending can fairly reliably hit 80%... for whatever that input is worth.
I've not had much luck increasing tolerance on volumetric compatibility... it buys another substep, and then it crashes anyway. I'm not sure about "NROPT, UNSYMM" benefits in this case.
However, I think you might have a magic bullet in turning on mixed U-P formulation. This exhibits the characteristics of past problems that we doubled the maximum strain just by adding this one key-option (with relatively little expense given it only adds 1DOF per element). Did you try that approach.
Take care,
Rod
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
-----Original Message-----
From: Metrisin, Joe (FTTINC) JMetrisin@fttinc.com
Sent: Wednesday, July 11, 2018 10:00 AM
To: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Subject: [Xansys] Large strain convergence issues.
I'm having difficulty modeling a thermoplastic material which is being used as a vibration damper. I want to do a static analysis to predict the deformed shape and stress in the damper from an assembly compression. I have lots of contact, NLGEOM,ON and gradually compressing the damper in multiple load steps (50 max). For the time being, I'm simulating this hyperelastic material as linear elastic with a very low modulus (roughly 4 orders of magnitude softer than the metal structure that is compressing it. I'm using solid 186's and 187's with reduced integration, keyopt(6)=1 for both. The damper geometry is rather complex so I'm meshing with tet's for most of it, but the main zone of compression uses 186's, but they ended up being 6 layers of degenerate penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied". ANSYS has problems when the total mechanical strain reaches ~15-20% or so. My questions are:
-
Is 15-20% strain a typical limit before rezoning is required? The rezoning feature in ANSYS is rather limited, so this will be a painful process if I have to manually rezone several times during the analysis. Does anyone have any experience with this to say what a typical level of strain you can get before rezoning is necessary? -
Also, I've tried relaxing the volumetric compatibility criteria a bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this criteria to use? How do you tell if this is relaxed too much? -
Is there any advantage to using unsymmetric matrices (NROPT, UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
Joe
- Rezoning is most useful when there is distortion of the elements cause
by large change in aspect ratios, change in the min/max angles between
element faces leading to poorly shaped elements. Strains themselves are
sometimes not useful to determine if rezoning is required or not.
If you decide to use rezoning, there are 2 methods. The old method in
Classic is to use an external meshing tool to manually recreate the mesh.
You will have to ensure certain nodes are retained if they are at an edge
of a contact definition/location where constraints are applied (help doc
has greater detail on this).
A better way would be to use the Nonlinear Adaptivity where the mesh is
recreated by the solver during solution. This is more powerful and SOLID187
and SOLID285 elements are supported.
- The default volumetric compatibility ratio is best left as is.
Increasing the tolerance will have to be used cautiously - you will want to
monitor carefully the elements where the compatibilty is violated.
Is this material modeled using a hyperelastic material with a
compressibility ratio of 0.? If yes, introducing a small finite
compressibility may be beneficial. I usually use a value which is analogous
to a poisson's ratio of 0.4995 to get over such issues.
- NROPT,UNSYMM is most useful if you frictional contact. The general
recommendation is to use it when the friction coefficient is greater than
0.2 for models with contact. However for hyperelastic models, I almost
always turn it on to see better convergence performance.
Harish
Harish Radhakrishnan
Product Manager - Mechanical Products
ANSYS Inc
15915 Katy Freeway, Suite 550
Houston, TX 77094
Office: 281-676-7013
On Wed, Jul 11, 2018 at 9:59 AM, Metrisin, Joe (FTTINC) <
JMetrisin@fttinc.com> wrote:
I'm having difficulty modeling a thermoplastic material which is being
used as a vibration damper. I want to do a static analysis to predict the
deformed shape and stress in the damper from an assembly compression. I
have lots of contact, NLGEOM,ON and gradually compressing the damper in
multiple load steps (50 max). For the time being, I'm simulating this
hyperelastic material as linear elastic with a very low modulus (roughly 4
orders of magnitude softer than the metal structure that is compressing
it. I'm using solid 186's and 187's with reduced integration, keyopt(6)=1
for both. The damper geometry is rather complex so I'm meshing with tet's
for most of it, but the main zone of compression uses 186's, but they ended
up being 6 layers of degenerate penta shaped elements created using the
inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied".
ANSYS has problems when the total mechanical strain reaches ~15-20% or so.
My questions are:
-
Is 15-20% strain a typical limit before rezoning is required?
The rezoning feature in ANSYS is rather limited, so this will be a painful
process if I have to manually rezone several times during the analysis.
Does anyone have any experience with this to say what a typical level of
strain you can get before rezoning is necessary?
-
Also, I've tried relaxing the volumetric compatibility criteria a
bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this criteria to
use? How do you tell if this is relaxed too much?
-
Is there any advantage to using unsymmetric matrices (NROPT,
UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are
proprietary and may be privileged, intended only for the use of the
individual or entity named above. If the reader of this message is not the
intended recipient, you are hereby notified that any dissemination,
distribution, or copying of this communication is strictly prohibited. If
you received this communication in error, please delete the message and
immediately notify the sender via the contact information listed above.
Thanks Rod. Yes, the mixed U/P keyopt(6)=1 is the first thing I tried. Maybe just my ignorance, but I expected these elements to handle more strain than 15%. Also, I'm really disappointed in the crude rezoning capability. For 3D, about all it can do is some basic local splitting/morphing. I think in my case I need to do a manual rezoning, probably multiple times. This involves exporting the deformed mesh, synthesizing geometry from it, then remeshing and importing back into the solution using REMESH. Very tedious.
Joseph Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.com
Affordable InnovationsT
Visit our website: www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----Original Message-----
From: Rod Scholl [mailto:rod.scholl@epsilonfea.com]
Sent: Wednesday, July 11, 2018 11:50 AM
To: XANSYS Mailing List Temporary Home
Subject: Re: [Xansys] Large strain convergence issues.
Hi Joe,
Mileage varies on the strain thresholds, depending on the class of problem/geometry. Most anything can converge up to 10% -- about 1/2 our plastic deformation analyses will hit distortion errors around 15-20% that can't be overcome besides with remeshing/rezoning. I note, however, that simple test cases on a regular tet mesh of a beam in bending can fairly reliably hit 80%... for whatever that input is worth.
I've not had much luck increasing tolerance on volumetric compatibility... it buys another substep, and then it crashes anyway. I'm not sure about "NROPT, UNSYMM" benefits in this case.
However, I think you might have a magic bullet in turning on mixed U-P formulation. This exhibits the characteristics of past problems that we doubled the maximum strain just by adding this one key-option (with relatively little expense given it only adds 1DOF per element). Did you try that approach.
Take care,
Rod
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
-----Original Message-----
From: Metrisin, Joe (FTTINC) JMetrisin@fttinc.com
Sent: Wednesday, July 11, 2018 10:00 AM
To: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Subject: [Xansys] Large strain convergence issues.
I'm having difficulty modeling a thermoplastic material which is being used as a vibration damper. I want to do a static analysis to predict the deformed shape and stress in the damper from an assembly compression. I have lots of contact, NLGEOM,ON and gradually compressing the damper in multiple load steps (50 max). For the time being, I'm simulating this hyperelastic material as linear elastic with a very low modulus (roughly 4 orders of magnitude softer than the metal structure that is compressing it. I'm using solid 186's and 187's with reduced integration, keyopt(6)=1 for both. The damper geometry is rather complex so I'm meshing with tet's for most of it, but the main zone of compression uses 186's, but they ended up being 6 layers of degenerate penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied". ANSYS has problems when the total mechanical strain reaches ~15-20% or so. My questions are:
-
Is 15-20% strain a typical limit before rezoning is required? The rezoning feature in ANSYS is rather limited, so this will be a painful process if I have to manually rezone several times during the analysis. Does anyone have any experience with this to say what a typical level of strain you can get before rezoning is necessary? -
Also, I've tried relaxing the volumetric compatibility criteria a bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this criteria to use? How do you tell if this is relaxed too much? -
Is there any advantage to using unsymmetric matrices (NROPT, UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
Wow! Nonlinear adaptivity appears to be exactly what I need. I didn't know that existed. I'm going to try that route now.
Thanks Harish!!!
Joseph Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.com
Affordable InnovationsT
Visit our website: www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----Original Message-----
From: Harish Radhakrishnan [mailto:harish.radhakrishnan@ansys.com]
Sent: Wednesday, July 11, 2018 11:57 AM
To: XANSYS Mailing List Temporary Home
Subject: Re: [Xansys] Large strain convergence issues.
Joe
- Rezoning is most useful when there is distortion of the elements cause by large change in aspect ratios, change in the min/max angles between element faces leading to poorly shaped elements. Strains themselves are sometimes not useful to determine if rezoning is required or not.
If you decide to use rezoning, there are 2 methods. The old method in Classic is to use an external meshing tool to manually recreate the mesh.
You will have to ensure certain nodes are retained if they are at an edge of a contact definition/location where constraints are applied (help doc has greater detail on this).
A better way would be to use the Nonlinear Adaptivity where the mesh is recreated by the solver during solution. This is more powerful and SOLID187 and SOLID285 elements are supported.
- The default volumetric compatibility ratio is best left as is.
Increasing the tolerance will have to be used cautiously - you will want to monitor carefully the elements where the compatibilty is violated.
Is this material modeled using a hyperelastic material with a compressibility ratio of 0.? If yes, introducing a small finite compressibility may be beneficial. I usually use a value which is analogous to a poisson's ratio of 0.4995 to get over such issues.
- NROPT,UNSYMM is most useful if you frictional contact. The general recommendation is to use it when the friction coefficient is greater than
0.2 for models with contact. However for hyperelastic models, I almost always turn it on to see better convergence performance.
Harish
Harish Radhakrishnan
Product Manager - Mechanical Products
ANSYS Inc
15915 Katy Freeway, Suite 550
Houston, TX 77094
Office: 281-676-7013
On Wed, Jul 11, 2018 at 9:59 AM, Metrisin, Joe (FTTINC) < JMetrisin@fttinc.com> wrote:
I'm having difficulty modeling a thermoplastic material which is being
used as a vibration damper. I want to do a static analysis to predict
the deformed shape and stress in the damper from an assembly
compression. I have lots of contact, NLGEOM,ON and gradually compressing the damper in
multiple load steps (50 max). For the time being, I'm simulating this
hyperelastic material as linear elastic with a very low modulus
(roughly 4 orders of magnitude softer than the metal structure that is
compressing it. I'm using solid 186's and 187's with reduced
integration, keyopt(6)=1 for both. The damper geometry is rather
complex so I'm meshing with tet's for most of it, but the main zone of
compression uses 186's, but they ended up being 6 layers of degenerate
penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied".
ANSYS has problems when the total mechanical strain reaches ~15-20% or so.
My questions are:
-
Is 15-20% strain a typical limit before rezoning is required?
The rezoning feature in ANSYS is rather limited, so this will be a
painful process if I have to manually rezone several times during the analysis.
Does anyone have any experience with this to say what a typical level
of strain you can get before rezoning is necessary?
-
Also, I've tried relaxing the volumetric compatibility criteria a
bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this
criteria to use? How do you tell if this is relaxed too much?
-
Is there any advantage to using unsymmetric matrices (NROPT,
UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are
proprietary and may be privileged, intended only for the use of the
individual or entity named above. If the reader of this message is not
the intended recipient, you are hereby notified that any
dissemination, distribution, or copying of this communication is
strictly prohibited. If you received this communication in error,
please delete the message and immediately notify the sender via the contact information listed above.
-------------- next part -------------- A non-text attachment was
scrubbed...
Name: image001.png
Type: image/png
Size: 15415 bytes
Desc: image001.png
URL: <http://xansystest.info/mailman/private/xansys-temp_
xansystest.info/attachments/20180711/c2a26043/attachment.png>
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. Metrisin,
a few months I generated a model of an engine mount. I specified a Mooney-Rivlin hyperelastic material for the elastomer part, which was coupled with steel plates.
I let Workbench make all the choices as for the element type of the elastomer body. It chose 187s with keypot(6)=0.
I used no inflation regions while meshing.
The solution was successful without rezoning.
The elastomer elements near the interfaces with the steel parts underwent deformations of about 19%.
Best regards
Riccardo Testi
Development and Strategies
2 Wheeler Engines Technical Centre
Piaggio & C. S.p.A
Viale Rinaldo Piaggio, 25
56025 Pontedera (Pisa) - ITALY
Phone: +39 0587 272850
Fax: +39 0587 272010
Mobile: +39 339 7241918
E-mail: riccardo.testi@piaggio.com
-----Messaggio originale-----
Da: Metrisin, Joe (FTTINC) [mailto:JMetrisin@fttinc.com]
Inviato: mercoledì 11 luglio 2018 17:00
A: XANSYS Mailing List Temporary Home xansys-temp@xansystest.info
Oggetto: [Xansys] Large strain convergence issues.
I'm having difficulty modeling a thermoplastic material which is being used as a vibration damper. I want to do a static analysis to predict the deformed shape and stress in the damper from an assembly compression. I have lots of contact, NLGEOM,ON and gradually compressing the damper in multiple load steps (50 max). For the time being, I'm simulating this hyperelastic material as linear elastic with a very low modulus (roughly 4 orders of magnitude softer than the metal structure that is compressing it. I'm using solid 186's and 187's with reduced integration, keyopt(6)=1 for both. The damper geometry is rather complex so I'm meshing with tet's for most of it, but the main zone of compression uses 186's, but they ended up being 6 layers of degenerate penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied". ANSYS has problems when the total mechanical strain reaches ~15-20% or so. My questions are:
-
Is 15-20% strain a typical limit before rezoning is required? The rezoning feature in ANSYS is rather limited, so this will be a painful process if I have to manually rezone several times during the analysis. Does anyone have any experience with this to say what a typical level of strain you can get before rezoning is necessary? -
Also, I've tried relaxing the volumetric compatibility criteria a bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this criteria to use? How do you tell if this is relaxed too much? -
Is there any advantage to using unsymmetric matrices (NROPT, UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution, or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
Hi Joe,
If possible, please share your candid thoughts about the nonlinear
adaptivity feature when you try it.
Thanks
Harish
On Wed, Jul 11, 2018 at 12:08 PM Metrisin, Joe (FTTINC) <
JMetrisin@fttinc.com> wrote:
Wow! Nonlinear adaptivity appears to be exactly what I need. I didn't
know that existed. I'm going to try that route now.
Thanks Harish!!!
Joseph Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.com
Affordable InnovationsT
Visit our website: www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are
proprietary and may be privileged, intended only for the use of the
individual or entity named above. If the reader of this message is not the
intended recipient, you are hereby notified that any dissemination,
distribution, or copying of this communication is strictly prohibited. If
you received this communication in error, please delete the message and
immediately notify the sender via the contact information listed above.
-----Original Message-----
From: Harish Radhakrishnan [mailto:harish.radhakrishnan@ansys.com]
Sent: Wednesday, July 11, 2018 11:57 AM
To: XANSYS Mailing List Temporary Home
Subject: Re: [Xansys] Large strain convergence issues.
Joe
- Rezoning is most useful when there is distortion of the elements cause
by large change in aspect ratios, change in the min/max angles between
element faces leading to poorly shaped elements. Strains themselves are
sometimes not useful to determine if rezoning is required or not.
If you decide to use rezoning, there are 2 methods. The old method in
Classic is to use an external meshing tool to manually recreate the mesh.
You will have to ensure certain nodes are retained if they are at an edge
of a contact definition/location where constraints are applied (help doc
has greater detail on this).
A better way would be to use the Nonlinear Adaptivity where the mesh is
recreated by the solver during solution. This is more powerful and SOLID187
and SOLID285 elements are supported.
- The default volumetric compatibility ratio is best left as is.
Increasing the tolerance will have to be used cautiously - you will want
to monitor carefully the elements where the compatibilty is violated.
Is this material modeled using a hyperelastic material with a
compressibility ratio of 0.? If yes, introducing a small finite
compressibility may be beneficial. I usually use a value which is analogous
to a poisson's ratio of 0.4995 to get over such issues.
- NROPT,UNSYMM is most useful if you frictional contact. The general
recommendation is to use it when the friction coefficient is greater than
0.2 for models with contact. However for hyperelastic models, I almost
always turn it on to see better convergence performance.
Harish
Harish Radhakrishnan
Product Manager - Mechanical Products
ANSYS Inc
15915 Katy Freeway, Suite 550
Houston, TX 77094
Office: 281-676-7013
On Wed, Jul 11, 2018 at 9:59 AM, Metrisin, Joe (FTTINC) <
JMetrisin@fttinc.com> wrote:
I'm having difficulty modeling a thermoplastic material which is being
used as a vibration damper. I want to do a static analysis to predict
the deformed shape and stress in the damper from an assembly
compression. I have lots of contact, NLGEOM,ON and gradually
compressing the damper in
multiple load steps (50 max). For the time being, I'm simulating this
hyperelastic material as linear elastic with a very low modulus
(roughly 4 orders of magnitude softer than the metal structure that is
compressing it. I'm using solid 186's and 187's with reduced
integration, keyopt(6)=1 for both. The damper geometry is rather
complex so I'm meshing with tet's for most of it, but the main zone of
compression uses 186's, but they ended up being 6 layers of degenerate
penta shaped elements created using the inflation meshing in WB.
My convergence issue is due to "volumetric compatibility not satisfied".
ANSYS has problems when the total mechanical strain reaches ~15-20% or
so.
My questions are:
-
Is 15-20% strain a typical limit before rezoning is required?
The rezoning feature in ANSYS is rather limited, so this will be a
painful process if I have to manually rezone several times during the
analysis.
Does anyone have any experience with this to say what a typical level
of strain you can get before rezoning is necessary?
-
Also, I've tried relaxing the volumetric compatibility criteria
a
bit (CNVTOL, COMP,, 0.02). What is a reasonable value of this
criteria to use? How do you tell if this is relaxed too much?
-
Is there any advantage to using unsymmetric matrices (NROPT,
UNSYMM)?
Thanks.
Joseph Metrisin
Structures Lead
[cid:image001.png@01D3CB67.7CCEBD30]
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110 | Jupiter, FL 33458 USA
+1 (561) 427-6346 Office | (561) 427-6191 Fax
JMetrisin@fttinc.commailto:JMetrisin@fttinc.com
Affordable Innovations(tm)
Visit our website: www.fttcompanies.comhttp://www.fttcompanies.com
Confidentiality Note:
The information contained in this transmission and any attachments are
proprietary and may be privileged, intended only for the use of the
individual or entity named above. If the reader of this message is not
the intended recipient, you are hereby notified that any
dissemination, distribution, or copying of this communication is
strictly prohibited. If you received this communication in error,
please delete the message and immediately notify the sender via the
contact information listed above.
-------------- next part -------------- A non-text attachment was
scrubbed...
Name: image001.png
Type: image/png
Size: 15415 bytes
Desc: image001.png
URL: <http://xansystest.info/mailman/private/xansys-temp_
xansystest.info/attachments/20180711/c2a26043/attachment.png>
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
--
Harish Radhakrishnan
Product Manager - Mechanical Products
ANSYS Inc
15915 Katy Freeway, Suite 550
Houston, TX 77094
Office: 281-676-7013