XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[struc] What kind of error is this ?
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
debabrata.podder
User


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Sat Nov 16, 2013 12:47 pm  Reply with quote

Dear experts,

While I am going to run a structural analysis (uncoupled thermal structural) by taking the thermal load by LDREAD command, I am getting the following mentioned warnings:

1. "A reference force value times the tolerance is used by the Newton-Raphson method for checking convergence. The calculated reference FORCE CONVERGENCE VALUE = 0 is less than a threshold. This threshold defaults to 1.0-2 or is specified as MINREF on the CNVTOL command. Check results carefully."
2. There are 1 small equation solver pivot terms.

How to fix them?

Thanks in advance.

Regards-
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
Back to top
View user's profile Send private message
atul.patil
User


Joined: 05 Jul 2012
Posts: 24

PostPosted: Tue Nov 19, 2013 9:23 am  Reply with quote

Hello Debabrata

I am not expert but want share my experience. I am using ANSYS for structural analysis and finite element modelling.

About pivot term - I constrained the model with some minimum additional boundary condition such that it do not affect the final result . Over constrained system may not give proper results. So my guess would be checking for constraints so that there is not rigid body motion.

Regarding the 1st query - In my case, I tried to relax the tolerance so that the solution reaches till end as for first run . There will be some deviation from proper results but it may give more insight.

Again .. I am not expert but just sharing my experience in structural modelling in ANSYS. I never worked on thermal problem.

Regards
Atul Patil
Student
Florida State University


________________

________________________
From: xansys-bounces@xansys.org <xansys-bounces@xansys.org> on behalf of debabrata.podder <debabrata.podder@iitkgp.ac.in>
Sent: Saturday, November 16, 2013 7:47 PM
To: xansys@xansys.org
Subject: [Xansys] [struc] What kind of error is this ?

Dear experts,

While I am going to run a structural analysis (uncoupled thermal structural) by taking the thermal load by LDREAD command, I am getting the following mentioned warnings:

1. "A reference force value times the tolerance is used by the Newton-Raphson method for checking convergence. The calculated reference FORCE CONVERGENCE VALUE = 0 is less than a threshold. This threshold defaults to 1.0-2 or is specified as MINREF on the CNVTOL command. Check results carefully."
2. There are 1 small equation solver pivot terms.

How to fix them?

Thanks in advance.

Regards-

------------------------
Debabrata Podder
Research Scholar
IIT Kharagpur
PIN NO.: 721302
India






+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
=

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
debabrata.podder
User


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Tue Nov 19, 2013 3:57 pm  Reply with quote

Thanks Atul for your time.

Regards-

debabrata
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
Back to top
View user's profile Send private message
riccardo.testi
User


Joined: 28 Mar 2011
Posts: 154

PostPosted: Wed Nov 20, 2013 12:52 am  Reply with quote

Dear Mr. Podder,
the first message refers to a problem in the calculation of the Newton-Raphson residual, which is computed multiplying the stiffness matrix by the guessed displacement vector. Is the stiffness matrix is singular, you can obtain spurious residuals, resulting in the first error message.
The second message stems straight from a singular stiffness matrix, which can be caused by an underconstrained model.
So, I think both message have a common origin, that is, a system which can experience rigid motions. One typical way to investigate those motions is to carry out a modal analysis, to single out possible 0-frequency mode shapes.
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: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] Per conto di Patil, Atul
Inviato: martedý 19 novembre 2013 17:23
A: ANSYS User Discussion List
Oggetto: Re: [Xansys] [struc] What kind of error is this ?

Hello Debabrata

I am not expert but want share my experience. I am using ANSYS for structural analysis and finite element modelling.

About pivot term - I constrained the model with some minimum additional boundary condition such that it do not affect the final result . Over constrained system may not give proper results. So my guess would be checking for constraints so that there is not rigid body motion.

Regarding the 1st query - In my case, I tried to relax the tolerance so that the solution reaches till end as for first run . There will be some deviation from proper results but it may give more insight.

Again .. I am not expert but just sharing my experience in structural modelling in ANSYS. I never worked on thermal problem.

Regards
Atul Patil
Student
Florida State University


________________

________________________
From: xansys-bounces@xansys.org <xansys-bounces@xansys.org> on behalf of debabrata.podder <debabrata.podder@iitkgp.ac.in>
Sent: Saturday, November 16, 2013 7:47 PM
To: xansys@xansys.org
Subject: [Xansys] [struc] What kind of error is this ?

Dear experts,

While I am going to run a structural analysis (uncoupled thermal structural) by taking the thermal load by LDREAD command, I am getting the following mentioned warnings:

1. "A reference force value times the tolerance is used by the Newton-Raphson method for checking convergence. The calculated reference FORCE CONVERGENCE VALUE = 0 is less than a threshold. This threshold defaults to 1.0-2 or is specified as MINREF on the CNVTOL command. Check results carefully."
2. There are 1 small equation solver pivot terms.

How to fix them?

Thanks in advance.

Regards-

------------------------
Debabrata Podder
Research Scholar
IIT Kharagpur
PIN NO.: 721302
India






+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


<br>
PIAGGIO & C. S.p.A. - Sede legale: Viale Rinaldo Piaggio 25, 56025 Pontedera (PI) Italy - R.E.A. Pisa 134077 - Capitale Sociale Euro 206.026.903,84 i.v. - Reg. Imprese Pisa e Codice fiscale 04773200011 - Direzione e coordinamento IMMSI S.p.A<br>
<br>
The information transmitted is intended only for the person or entity to which it is addressed and may contain confidential and/or privileged information. Any disclosure, distribution or other use of this message by any subject different from the intended recipient is strictly prohibited. If you received this by mistake, please notify us immediately and delete this communication.

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Wed Nov 20, 2013 3:42 am  Reply with quote

On 20/11/2013 07:51, Testi Riccardo wrote:

Quote:
the first message refers to a problem in the calculation of the Newton-Raphson residual, which is computed multiplying the stiffness matrix by the guessed displacement vector. Is the stiffness matrix is singular, you can obtain spurious residuals, resulting in the first error message.

That wasn't my understanding of the first error message. My
understanding is that ANSYS sums the applied loads and then takes a
specified percentage (by default 0.5% or 0.1% depending on SOLCONTROL
setting) of the SRSS of the applied loads as a tolerance to use during
non linear analysis to compare against the residual (difference between
applied load and currently calculated reaction forces). If the loads
are zero or very small then it uses a specified value as the tolerance.
The problem with this approach is that the default specified tolerance
value is a purely arbitrary number which may or may not make sense for a
particular problem and can be overridden by the user. See section
8.6.2.3.2 of the Structural Analysis Guide. My guess is that the OP had
purely thermal loads and the SRSS was 0.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
riccardo.testi
User


Joined: 28 Mar 2011
Posts: 154

PostPosted: Wed Nov 20, 2013 6:38 am  Reply with quote

Dear Mr. Liddle,
I apologize. I was misled by the statement "in the following cases, the default Rref value is the specified or default minimum reference value set via the CNVTOL,,,,,MINREF command:
For structural DOFs if Rref falls below 1.0E-2 (typically occurring in rigid-body motion analyses, such as those involving stress-free rotation)". The statement can be found in section 15.12.2 of the Theory manual. Having that in mind, I was thinking that rigid body motions, even if unwanted, could cause Rref to fall below its minimum reference value.
I'm truly sorry.

Best regards
Riccardo Testi


-----Messaggio originale-----
Da: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] Per conto di Martin Liddle
Inviato: mercoledý 20 novembre 2013 11:43
A: xansys@xansys.org
Oggetto: Re: [Xansys] R: [struc] What kind of error is this ?

On 20/11/2013 07:51, Testi Riccardo wrote:

Quote:
the first message refers to a problem in the calculation of the Newton-Raphson residual, which is computed multiplying the stiffness matrix by the guessed displacement vector. Is the stiffness matrix is singular, you can obtain spurious residuals, resulting in the first error message.

That wasn't my understanding of the first error message. My understanding is that ANSYS sums the applied loads and then takes a specified percentage (by default 0.5% or 0.1% depending on SOLCONTROL
setting) of the SRSS of the applied loads as a tolerance to use during non linear analysis to compare against the residual (difference between applied load and currently calculated reaction forces). If the loads are zero or very small then it uses a specified value as the tolerance.
The problem with this approach is that the default specified tolerance value is a purely arbitrary number which may or may not make sense for a particular problem and can be overridden by the user. See section
8.6.2.3.2 of the Structural Analysis Guide. My guess is that the OP had purely thermal loads and the SRSS was 0.

--
Martin Liddle, Tynemouth Computer Services, Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


<br>
PIAGGIO & C. S.p.A. - Sede legale: Viale Rinaldo Piaggio 25, 56025 Pontedera (PI) Italy - R.E.A. Pisa 134077 - Capitale Sociale Euro 206.026.903,84 i.v. - Reg. Imprese Pisa e Codice fiscale 04773200011 - Direzione e coordinamento IMMSI S.p.A<br>
<br>
The information transmitted is intended only for the person or entity to which it is addressed and may contain confidential and/or privileged information. Any disclosure, distribution or other use of this message by any subject different from the intended recipient is strictly prohibited. If you received this by mistake, please notify us immediately and delete this communication.

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
david.gross
User


Joined: 14 Aug 2009
Posts: 139

PostPosted: Wed Nov 20, 2013 8:15 am  Reply with quote

Riccardo,

You need to keep in mind that, based on who the OP is, this is a very likely a welding analysis. It is not at all uncommon for the first step of a welding analysis to start off at the reference temperature with no mechanical loads. This will of course lead to a MINREF warning that can safely be ignored. The small pivot error can also occur in this situation due to "floating nodes" associated only with KILLED elements. He has posted on this subject before and received similar responses in the past.

It is entirely possible that this situation is different, and since the OP didn't give us any context of what he was doing, when in the analysis the warnings occurred, etc., we are left to rely on general rules of thumb. You should not feel the need to apologize.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of Testi Riccardo
Sent: Wednesday, November 20, 2013 8:38 AM
To: ANSYS User Discussion List
Subject: [Xansys] R: R: [struc] What kind of error is this ?

Dear Mr. Liddle,
I apologize. I was misled by the statement "in the following cases, the default Rref value is the specified or default minimum reference value set via the CNVTOL,,,,,MINREF command:
For structural DOFs if Rref falls below 1.0E-2 (typically occurring in rigid-body motion analyses, such as those involving stress-free rotation)". The statement can be found in section 15.12.2 of the Theory manual. Having that in mind, I was thinking that rigid body motions, even if unwanted, could cause Rref to fall below its minimum reference value.
I'm truly sorry.

Best regards
Riccardo Testi

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
riccardo.testi
User


Joined: 28 Mar 2011
Posts: 154

PostPosted: Thu Nov 21, 2013 1:00 am  Reply with quote

Dear Mr. Gross,
I have the habit of quickly admitting my mistakes. However, I thank you for your kindness.

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: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] Per conto di David Gross
Inviato: mercoledý 20 novembre 2013 16:16
A: ANSYS User Discussion List
Oggetto: Re: [Xansys] R: R: [struc] What kind of error is this ?

Riccardo,

You need to keep in mind that, based on who the OP is, this is a very likely a welding analysis. It is not at all uncommon for the first step of a welding analysis to start off at the reference temperature with no mechanical loads. This will of course lead to a MINREF warning that can safely be ignored. The small pivot error can also occur in this situation due to "floating nodes" associated only with KILLED elements. He has posted on this subject before and received similar responses in the past.

It is entirely possible that this situation is different, and since the OP didn't give us any context of what he was doing, when in the analysis the warnings occurred, etc., we are left to rely on general rules of thumb. You should not feel the need to apologize.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of Testi Riccardo
Sent: Wednesday, November 20, 2013 8:38 AM
To: ANSYS User Discussion List
Subject: [Xansys] R: R: [struc] What kind of error is this ?

Dear Mr. Liddle,
I apologize. I was misled by the statement "in the following cases, the default Rref value is the specified or default minimum reference value set via the CNVTOL,,,,,MINREF command:
For structural DOFs if Rref falls below 1.0E-2 (typically occurring in rigid-body motion analyses, such as those involving stress-free rotation)". The statement can be found in section 15.12.2 of the Theory manual. Having that in mind, I was thinking that rigid body motions, even if unwanted, could cause Rref to fall below its minimum reference value.
I'm truly sorry.

Best regards
Riccardo Testi

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


<br>
PIAGGIO & C. S.p.A. - Sede legale: Viale Rinaldo Piaggio 25, 56025 Pontedera (PI) Italy - R.E.A. Pisa 134077 - Capitale Sociale Euro 206.026.903,84 i.v. - Reg. Imprese Pisa e Codice fiscale 04773200011 - Direzione e coordinamento IMMSI S.p.A<br>
<br>
The information transmitted is intended only for the person or entity to which it is addressed and may contain confidential and/or privileged information. Any disclosure, distribution or other use of this message by any subject different from the intended recipient is strictly prohibited. If you received this by mistake, please notify us immediately and delete this communication.

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

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


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron