[Xansys] "Convergence Issues -Nonlinear elastic Plastic

[Vijayasekar Burra]

All ANSYS Users,

Iam trying to analyze plastic tank with internal pressure load. I have
modeled plastic model with Shell 181 elements. Iam running nonlinear
elastic plastic run with large deformation on. I have been facing
convergence issues especially with moments are not converging and
resulting to error "Excessive destortion of the element XXXxx" after
30%-50% of load. On Same model somtimes I get "ROT UX DOF limit exceeded
"after solving 30% of load . Please let me know if there is are any
options iam missing or how do I overcome this problem and have results.


Right now Iam changing the convergence tolerance (CNVTOL) manually for
moments and making model to converge, but Iam not confident I can
believe the results with forced convergence.

Thanks in advance for you help.

Vijay Burra
RFA/Minnesota Engineering
Eden Prairie, MN

Post generated using Mail2Forum (http://www.mail2forum.com)

[Krueger, Mark]

Check your mesh - it may be too coarse leading to excessive distortion
of the elements.

Tracking the deformed results may indicate that part of the model has
let "loose" (lost contact, excessive plasticity, etc.) and therefore
exceeding the DOF limit.

- Mark K.
===============================
Mark Krueger, P.E.
Structural Analyst
Advanced Weapons Division - ATK
--email address suppressed--
===============================



-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Vijayasekar Burra
Sent: Tuesday, December 18, 2007 9:32 AM
To: --email address suppressed--
Subject: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
analysis"

All ANSYS Users,

Iam trying to analyze plastic tank with internal pressure load. I have
modeled plastic model with Shell 181 elements. Iam running nonlinear
elastic plastic run with large deformation on. I have been facing
convergence issues especially with moments are not converging and
resulting to error "Excessive destortion of the element XXXxx" after
30%-50% of load. On Same model somtimes I get "ROT UX DOF limit exceeded
"after solving 30% of load . Please let me know if there is are any
options iam missing or how do I overcome this problem and have results.


Right now Iam changing the convergence tolerance (CNVTOL) manually for
moments and making model to converge, but Iam not confident I can
believe the results with forced convergence.

Thanks in advance for you help.

Vijay Burra
RFA/Minnesota Engineering
Eden Prairie, MN

Post generated using Mail2Forum (http://www.mail2forum.com)

[S. Ismonov]

You may also try to follow the tips and guidelines for nonlinear analysis in
section 8.12 of your documentation for ANSYS 11.0. Gradually applying the
load has helped me once.

Thanks,
----
Shakhrukh Ismonov
Ph.D. Student
MSU, ME Dept

On Dec 18, 2007 1:01 PM, Krueger, Mark <--email address suppressed--> wrote:

> Check your mesh - it may be too coarse leading to excessive distortion
> of the elements.
>
> Tracking the deformed results may indicate that part of the model has
> let "loose" (lost contact, excessive plasticity, etc.) and therefore
> exceeding the DOF limit.
>
> - Mark K.
> ===============================
> Mark Krueger, P.E.
> Structural Analyst
> Advanced Weapons Division - ATK
> --email address suppressed--
> ===============================
>
>
>
> -----Original Message-----
> From: --email address suppressed-- [mailto:--email address suppressed--] On
> Behalf Of Vijayasekar Burra
> Sent: Tuesday, December 18, 2007 9:32 AM
> To: --email address suppressed--
> Subject: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
> analysis"
>
> All ANSYS Users,
>
> Iam trying to analyze plastic tank with internal pressure load. I have
> modeled plastic model with Shell 181 elements. Iam running nonlinear
> elastic plastic run with large deformation on. I have been facing
> convergence issues especially with moments are not converging and
> resulting to error "Excessive destortion of the element XXXxx" after
> 30%-50% of load. On Same model somtimes I get "ROT UX DOF limit exceeded
> "after solving 30% of load . Please let me know if there is are any
> options iam missing or how do I overcome this problem and have results.
>
>
> Right now Iam changing the convergence tolerance (CNVTOL) manually for
> moments and making model to converge, but Iam not confident I can
> believe the results with forced convergence.
>
> Thanks in advance for you help.
>
> Vijay Burra
> RFA/Minnesota Engineering
> Eden Prairie, MN
> ^--------------------------------------------------------
> | XANSYS - www.xansys.org |
> | The Discussion List for users of ANSYS, Inc. Software |
> | Hosted by PADT - www.padtinc.com |
> ^--------------------------------------------------------
>



--
Shakhrukh Ismonov

Post generated using Mail2Forum (http://www.mail2forum.com)

[Rod Scholl]

Hi Vijay,

I find this error is common if you have a thickness to edge length ratio
that is too high. What ratio do you have?

If you are indeed thin, like 5:1 or greater, then there are a few things
you can try if you are getting this distortion error. First of those
might be to set Keyoption3=1. Any difference?

Of course, if the mesh is distorting to the point that the element
shapes are no longer valid, there's not much you can do except
mesh-morphing, or prebias the mesh in anticipation of the distortion if
its in predictable fashion. Take a unconverged solution, or the last
converged solution, and do a shape check on the distorted shape... maybe
there is only one region that is giving you difficulty and that might
make solutions more targeted.

Rod


Rod Scholl
Specialist Engineer, Analysis
Phoenix Analysis & Design Technologies
612-605-6894
602-218-5391 (AZ Toll Free)
--email address suppressed--
http://www.padtinc.com


-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Vijayasekar Burra
Sent: Tuesday, December 18, 2007 9:32 AM
To: --email address suppressed--
Subject: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
analysis"

All ANSYS Users,

Iam trying to analyze plastic tank with internal pressure load. I have
modeled plastic model with Shell 181 elements. Iam running nonlinear
elastic plastic run with large deformation on. I have been facing
convergence issues especially with moments are not converging and
resulting to error "Excessive destortion of the element XXXxx" after
30%-50% of load. On Same model somtimes I get "ROT UX DOF limit exceeded
"after solving 30% of load . Please let me know if there is are any
options iam missing or how do I overcome this problem and have results.


Right now Iam changing the convergence tolerance (CNVTOL) manually for
moments and making model to converge, but Iam not confident I can
believe the results with forced convergence.

Thanks in advance for you help.

Vijay Burra
RFA/Minnesota Engineering
Eden Prairie, MN

Post generated using Mail2Forum (http://www.mail2forum.com)

[Raghavendran G]

VijaySekar,

You could additionally request Non linear Diagnostics (NLDIAG) and you could request Newton-Raphson Residuals to track areas where non-convergence is occurring ( There was an article in PADT Focus about using this). Also you could use *get to get the element aspect ratio which is failing during the solution and you could fine mesh or correct the elements in its vicinity to a better extent for subsequent run.

You have also mentioned about ROTX dof limit exceeded, I believe it might have something to do with constraints.

Thanks
Raghavendran. G
Infosys Technologies Ltd
India




**************** CAUTION - Disclaimer *****************
This e-mail contains PRIVILEGED AND CONFIDENTIAL INFORMATION intended solely for the use of the addressee(s). If you are not the intended recipient, please notify the sender by e-mail and delete the original message. Further, you are not to copy, disclose, or distribute this e-mail or its contents to any other person and any such actions are unlawful. This e-mail may contain viruses. Infosys has taken every reasonable precaution to minimize this risk, but is not liable for any damage you may sustain as a result of any virus in this e-mail. You should carry out your own virus checks before opening the e-mail or attachment. Infosys reserves the right to monitor and review the content of all messages sent to or from this e-mail address. Messages sent to or from this e-mail address may be stored on the Infosys e-mail system.
***INFOSYS******** End of Disclaimer ********INFOSYS***

Post generated using Mail2Forum (http://www.mail2forum.com)

[Aadith Om]

One more possibility I can think is that if the ENTIRE structure becomes
plastic the solution will stop. If the entire structure becomes plastic
then there is no more load carrying capability to the structure. Check
the plastic strain plot at the end of last converged sub step.

Regards
Aadith Om,
Freelancer,
FEA Consultant,
Chennai & B'lore.
We offer FEA consultancy and Training.


----- Original Message -----
From: "Raghavendran G"
To: "--email address suppressed--"
Subject: Re: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
analysis"
Date: Wed, 19 Dec 2007 12:05:42 +0530


VijaySekar,

You could additionally request Non linear Diagnostics (NLDIAG)
and you could request Newton-Raphson Residuals to track areas where
non-convergence is occurring ( There was an article in PADT Focus
about using this). Also you could use *get to get the element
aspect ratio which is failing during the solution and you could
fine mesh or correct the elements in its vicinity to a better
extent for subsequent run.

You have also mentioned about ROTX dof limit exceeded, I believe it
might have something to do with constraints.

Thanks
Raghavendran. G
Infosys Technologies Ltd
India




--
Got No Time? Shop Online for Great Gift Ideas!
http://mail.shopping.com/?linkin_id=8033174

Post generated using Mail2Forum (http://www.mail2forum.com)

[Vijayasekar Burra]

Rod,
Iam not sure about the element to edge ratio, but Iam using 4mm thick
tank and maximum element size of 7 mm. I tried running the model with
fine mesh but no luck...

When I check unconverged solution it is actually one region which is
like 3D bend radius location where bends from 3 sides merge.

Let me try running the model with KEYOPT 3=1,

Appreciate all your suggestions ......

Thanks,
Vijay Burra
RFA/Minnesota Engineering
--email address suppressed--



-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Rod Scholl
Sent: Tuesday, December 18, 2007 6:10 PM
To: ANSYS User Discussion List
Subject: RE: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
analysis"

Hi Vijay,

I find this error is common if you have a thickness to edge length ratio
that is too high. What ratio do you have?

If you are indeed thin, like 5:1 or greater, then there are a few things
you can try if you are getting this distortion error. First of those
might be to set Keyoption3=1. Any difference?

Of course, if the mesh is distorting to the point that the element
shapes are no longer valid, there's not much you can do except
mesh-morphing, or prebias the mesh in anticipation of the distortion if
its in predictable fashion. Take a unconverged solution, or the last
converged solution, and do a shape check on the distorted shape... maybe
there is only one region that is giving you difficulty and that might
make solutions more targeted.

Rod


Rod Scholl
Specialist Engineer, Analysis
Phoenix Analysis & Design Technologies
612-605-6894
602-218-5391 (AZ Toll Free)
--email address suppressed--
http://www.padtinc.com


-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Vijayasekar Burra
Sent: Tuesday, December 18, 2007 9:32 AM
To: --email address suppressed--
Subject: [Xansys] "Convergence Issues -Nonlinear elastic Plastic
analysis"

All ANSYS Users,

Iam trying to analyze plastic tank with internal pressure load. I have
modeled plastic model with Shell 181 elements. Iam running nonlinear
elastic plastic run with large deformation on. I have been facing
convergence issues especially with moments are not converging and
resulting to error "Excessive destortion of the element XXXxx" after
30%-50% of load. On Same model somtimes I get "ROT UX DOF limit exceeded
"after solving 30% of load . Please let me know if there is are any
options iam missing or how do I overcome this problem and have results.


Right now Iam changing the convergence tolerance (CNVTOL) manually for
moments and making model to converge, but Iam not confident I can
believe the results with forced convergence.

Thanks in advance for you help.

Vijay Burra
RFA/Minnesota Engineering
Eden Prairie, MN

Post generated using Mail2Forum (http://www.mail2forum.com)