XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[APDL] Saving and resuming results from an analysis
 
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
kerry.kreitman
User


Joined: 02 Feb 2014
Posts: 29

PostPosted: Fri Jun 06, 2014 9:56 am  Reply with quote

Hello everyone,

I have a question regarding which ANSYS-created files I need to be saving to be able to later resume the database and examine the results. Despite reading through the ANSYS documentation and many forum and google searches, I still don't quite understand it yet.

Based on everything I've read, I thought that if I saved the .db file using SAVE,jobname,db,,SOLU the nodal and elemental results would be saved along with the model data in the .db file. However, after deleting the .rst files and reloading the database using RESUME,jobname,db, I cannot access the results. For example, using SET,LIST I get the message "An error occurred while attempting to open the results file jobname.rst", which makes complete sense because the .rst file doesn't exist.

Is there a different way to access the results through the saved database? Or do I always need to keep the .rst file to go back and re-visit the results in the future? Are there any other files that I need as well?

Thanks in advance!
Kerry
_________________
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)
Back to top
View user's profile Send private message
dean.brown
User


Joined: 10 Nov 2008
Posts: 27

PostPosted: Fri Jun 06, 2014 11:52 am  Reply with quote

Kerry,

A .db file can contain only one results set. When you use "SAVE,jobname,db,,SOLU", the database is saved along with the single results set that is in memory at that time. Later, when the file is resumed, you can work with results for that set only, without needing a results file. The documentation for the SET command states that this command scans the results file and produces a summary of each load step on the file. If you have multiple load steps, you need to keep your results file.

Depending on what you want to do, there may be other files you should keep, for instance, for restart, superelement, and mode superposition analyses. If you use load step files (LSWRITE command), you'll probably want to keep those. I would suggest keeping any batch input files. Session log files and error files can be useful, as well as output files from batch runs.

Best regards,
Dean Brown
Principal Engineer
Microvision, Inc.
USA
www.microvision.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of kerry.kreitman
Sent: Friday, June 06, 2014 9:57 AM
To: xansys@xansys.org
Subject: [Xansys] [APDL] Saving and resuming results from an analysis

Hello everyone,

I have a question regarding which ANSYS-created files I need to be saving to be able to later resume the database and examine the results. Despite reading through the ANSYS documentation and many forum and google searches, I still don't quite understand it yet.

Based on everything I've read, I thought that if I saved the .db file using SAVE,jobname,db,,SOLU the nodal and elemental results would be saved along with the model data in the .db file. However, after deleting the .rst files and reloading the database using RESUME,jobname,db, I cannot access the results. For example, using SET,LIST I get the message "An error occurred while attempting to open the results file jobname.rst", which makes complete sense because the .rst file doesn't exist.

Is there a different way to access the results through the saved database? Or do I always need to keep the .rst file to go back and re-visit the results in the future? Are there any other files that I need as well?

Thanks in advance!
Kerry

------------------------
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)


________________________________

CONFIDENTIAL OR PROPRIETARY COMMUNICATION: This message (including any attachments) is for the sole use of the intended recipient and is assumed to contain confidential or proprietary information of Microvision, Inc. Review, publication, use or distribution of this message, in whole or in part, by an unintended recipient is prohibited and may be a violation of law. If you are not the intended recipient, please contact the sender by reply e-mail and delete this e-mail and any copies.
+-------------------------------------------------------------+
| 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
david.gross
User


Joined: 14 Aug 2009
Posts: 139

PostPosted: Fri Jun 06, 2014 2:49 pm  Reply with quote

Kerry,

Very similar to what Dean just said, we have actually kicked this around in our shop, and have developed the following guidelines for archiving analyses performed in MAPDL, and the guidance includes the following:

-- All batch input listings that were used in the analysis. This includes all post-processing input listings.
-- Other text or binary files (e.g., CAD geometry files) necessary to re-create the run.
-- The ".out" file that is created which records all of the batch input listing commands and the result of each command.
-- The ANSYS database files (*.db) that contain the model geometry information.
-- The ANSYS results file. Structural analysis results files have the ".rst" file extension and thermal analysis results files have the ".rth" file extension.
-- The "file.err" file that is produced as part of every ANSYS analysis.

The above will be sufficient to review previous work, but will not be sufficient to allow a typical analysis to be "resumed" and continued with additional load steps. If you intend to "restart" an analysis, you will need other files, as Dean also noted. These typically include *.emat and *.esav files for nonlinear runs, and also *.ldhi files if you're trying to use multi-frame restart.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Dean Brown
Sent: Friday, June 06, 2014 2:53 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] [APDL] Saving and resuming results from an analysis

Kerry,

A .db file can contain only one results set. When you use "SAVE,jobname,db,,SOLU", the database is saved along with the single results set that is in memory at that time. Later, when the file is resumed, you can work with results for that set only, without needing a results file. The documentation for the SET command states that this command scans the results file and produces a summary of each load step on the file. If you have multiple load steps, you need to keep your results file.

Depending on what you want to do, there may be other files you should keep, for instance, for restart, superelement, and mode superposition analyses. If you use load step files (LSWRITE command), you'll probably want to keep those. I would suggest keeping any batch input files. Session log files and error files can be useful, as well as output files from batch runs.

Best regards,
Dean Brown
Principal Engineer
Microvision, Inc.
USA
www.microvision.com

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

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


Joined: 02 Feb 2014
Posts: 29

PostPosted: Sun Jun 08, 2014 3:46 pm  Reply with quote

Thanks Dean and David - that is very helpful information

Kerry
_________________
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)
Back to top
View user's profile Send private message
siva.ganesh
User


Joined: 14 Apr 2014
Posts: 32
Location: hyderabad

PostPosted: Tue Jun 10, 2014 3:28 am  Reply with quote

Hi Kerry

I have a doubt in plotting a load vs displacement curve
i wanted to get a reaction for all the load substeps or timesteps for the
selected nodes.
Currently i'm trying with path, ppath and pdef command.
but in pdef command there is no reaction in the given items.

in second case i used the following code for getting the reaction for the
selection nodes
SET,,, ,,, ,1
PRRFOR,Fz
!1 refers first load substep
but every time i used to copy paste on the command window.
it's a time consuming task

for minimizing the time i used the following *do command

*GET,LASTSUBSTEP,ACTIVE,,SET,SBST
*DO,Q,1,LASTSUBSTEP
SET,,, ,,, ,Q
PRRFOR,FY
*ENDDO

but i'm getting the output file only for the 1st substep
How to get a total reaction in the selected nodes for all the substep in a
single output file?

thanks in advance






On Mon, Jun 9, 2014 at 4:16 AM, kerry.kreitman <kerry.kreitman@utexas.edu>
wrote:

Quote:
Thanks Dean and David - that is very helpful information

Kerry

------------------------
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+




--
*S.Sivaganesh*
PhD Student,
Indian Institute of Technology Hyderabad <http://www.iith.ac.in/>
+-------------------------------------------------------------+
| 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)
_________________
--
S.Sivaganesh
PhD Student,
IIT Hyderabad
Back to top
View user's profile Send private message Send e-mail Visit poster's website
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jun 10, 2014 4:44 am  Reply with quote

Dear Siva,

try the time-history postprocessor (/post26) instead of the general
postprocessor (/post1). It is made for what you need.

I am truly amazed that you have not found that for yourself. It is a
basic postprocessing tool that is essential when solving nonlinear or
transient problems. Moreover it is not a hidden or undocumented feature.
In the ansys manual, in the "nonlinear structural analysis" section
(which, by the way, should have been your first stop in your work),
there is a section describing how to review the results on both
postprocessors. You even have one sample problem solved interactively
and by commands.

I would really reccommend that you make a good use of the ansys help
before asking on the xansys forum.

Best regards,

Jose M. Galan

Assistant Professor

Dept. Construction Engineering

Universidad de Sevilla (Spain)

El 10/06/2014 12:28, S Siva Ganesh escribió:

Quote:
Hi Kerry

I have a doubt in plotting a load vs displacement curve
i wanted to get a reaction for all the load substeps or timesteps for the
selected nodes.
Currently i'm trying with path, ppath and pdef command.
but in pdef command there is no reaction in the given items.

in second case i used the following code for getting the reaction for the
selection nodes
SET,,, ,,, ,1
PRRFOR,Fz
!1 refers first load substep
but every time i used to copy paste on the command window.
it's a time consuming task

for minimizing the time i used the following *do command

*GET,LASTSUBSTEP,ACTIVE,,SET,SBST
*DO,Q,1,LASTSUBSTEP
SET,,, ,,, ,Q
PRRFOR,FY
*ENDDO

but i'm getting the output file only for the 1st substep
How to get a total reaction in the selected nodes for all the substep in a
single output file?

thanks in advance

On Mon, Jun 9, 2014 at 4:16 AM, kerry.kreitman <kerry.kreitman@utexas.edu>
wrote:

Quote:
Thanks Dean and David - that is very helpful information Kerry ------------------------ Kerry Kreitman PhD Student The University of Texas at Austin (USA) -------------------- m2f -------------------- Sent using Mail2Forum (http://www.mail2forum.com [1]). Read this topic online here: http://xansys.org/forum/viewtopic.php?p=94362#94362 [2] -------------------- m2f -------------------- +-------------------------------------------------------------+ | XANSYS web - www.xansys.org/forum [3] | | The Online Community for users of ANSYS, Inc. Software | | Hosted by PADT - www.padtinc.com [4] | | Send administrative requests to xansys-mod@tynecomp.co.uk | +-------------------------------------------------------------+


Links:
------
[1] http://www.mail2forum.com
[2] http://xansys.org/forum/viewtopic.php?p=94362#94362
[3] http://www.xansys.org/forum
[4] http://www.padtinc.com
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

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


Joined: 02 Feb 2014
Posts: 29

PostPosted: Tue Jun 10, 2014 6:19 am  Reply with quote

Siva,

As Jose said, the time history post-processor is what you need. I am just discovering how useful that can be so I don't know too much about it yet, but perhaps the following code will help you get started. This will produce a plot in ansys of the time-deflection behavior at a particular node (where time is directly proportional to load):

FINISH
/POST26 ! enter time-history post processor
ALLSEL
dd = NODE(0,-(t_fl/2+d_fl),-P1_loc) ! select node of interest
NSOL,2,dd,U,Y,P1_y_displ ! create variable for y displacement of that node
STORE,MERGE ! store data in the variable
PLVAR,P1_y_displ ! plot the variable vs time
_________________
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 10, 2014 9:54 am  Reply with quote

On Jun 10, 2014, at 6:44 AM, mfernan@us.es wrote:

Quote:
I am truly amazed that you have not found that for yourself.
This whole thread is amazing. In so very many ways.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
siva.ganesh
User


Joined: 14 Apr 2014
Posts: 32
Location: hyderabad

PostPosted: Tue Jun 10, 2014 10:28 am  Reply with quote

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
--
S.Sivaganesh
PhD Student,
IIT Hyderabad
Back to top
View user's profile Send private message Send e-mail Visit poster's website
siva.ganesh
User


Joined: 14 Apr 2014
Posts: 32
Location: hyderabad

PostPosted: Tue Jun 10, 2014 10:29 am  Reply with quote

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
--
S.Sivaganesh
PhD Student,
IIT Hyderabad
Back to top
View user's profile Send private message Send e-mail Visit poster's website
siva.ganesh
User


Joined: 14 Apr 2014
Posts: 32
Location: hyderabad

PostPosted: Tue Jun 10, 2014 10:57 am  Reply with quote

I learning from X ansys only.
thanks for everyone for commenting on my posts


On Tue, Jun 10, 2014 at 11:08 PM, Phil Vidori <philvid@videotron.ca> wrote:

Quote:
I'm sorry to say that you need to take an ANSYS class ( introduction ).
Or have someone else do the analysis work for you.
Otherwise, how can you be sure that the experimental results
match the FEA results ??

Regards,


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of S Siva Ganesh
Sent: Tuesday, June 10, 2014 1:30 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] [APDL] Saving and resuming results from an analysis

Respected Professor Jose

I'm a integrated Ph.D Student. (Ph.D after Bachelor Degree)
I never gone through any FEM course.
This is the first time i'm working with ansys.
My strength is in Experimental work.
Ansys is a simulation software, where the exact result can be found as like
experimental.
But the trick is that, how to work with ansys. That's what i'm learning
now.

There is nothing wrong, "if i don't know something",
but that is the big mistake, " if i don't learn that thing".

Now i learned it.
Thanks for your comments professor.



--
*S.Sivaganesh*
PhD Student,
+-------------------------------------------------------------+
| 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)
_________________
--
S.Sivaganesh
PhD Student,
IIT Hyderabad
Back to top
View user's profile Send private message Send e-mail Visit poster's website
michael.morsches
User


Joined: 02 Apr 2013
Posts: 11

PostPosted: Tue Jun 10, 2014 11:04 am  Reply with quote

"I learning from X ansys only.
thanks for everyone for commenting on my posts"

I am struggling with this statement...

Mr Vidori is correct and you should definitely take a class. This forum doesn't exist to teach you how to use software, it exists to discuss topics/problems/techniques.

Regards,

Mike

Mike Morsches
Staff Engineer - R&D Surgical Solutions
Covidien

This information may be confidential and/or privileged. Use of this information by anyone other than the intended recipient is prohibited. If you receive this in error, please inform the sender and remove any record of this message.
 Please consider the environment before printing

+-------------------------------------------------------------+
| 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
martin.liddle
Site Admin


Joined: 21 Oct 2008
Posts: 152

PostPosted: Tue Jun 10, 2014 11:08 am  Reply with quote

On 10/06/2014 18:56, S Siva Ganesh wrote:
Quote:
I learning from X ansys only.

I am sorry but you are making far too many posts. XANSYS can never be a
way to teach new users from scratch; please take a basic training
course. In future your posts will be moderated and limited to one post
per day.

--
Martin Liddle, XANSYS Moderator, 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 |
+-------------------------------------------------------------+

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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 10, 2014 11:09 am  Reply with quote

On Jun 10, 2014, at 12:38 PM, Phil Vidori wrote:

Quote:
I'm sorry to say that you need to take an ANSYS class
( introduction ).
Or have someone else do the analysis work for you.
Otherwise, how can you be sure that the experimental results
match the FEA results ??

Haven't you heard? ANSYS gives you the exact answer--it has to match
the test.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
carl.mally
User


Joined: 21 Oct 2008
Posts: 120

PostPosted: Tue Jun 10, 2014 11:17 am  Reply with quote

Quote:
Quote:
Haven't you heard? ANSYS gives you the exact answer--it has to match the test.<<

So that's where I have been going wrong! I learn something new every day.


Carl Mally
Product Development Engineer
Centro Inc.
950 North Bend Drive
North Liberty, IA 52317


+-------------------------------------------------------------+
| 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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 10, 2014 11:30 am  Reply with quote

On Jun 10, 2014, at 1:17 PM, Mally, Carl wrote:

Quote:
So that's where I have been going wrong! I learn something new
every day.

Strictly speaking, ANSYS doesn't *give* you anything. It's more a
matter of trading punches and rifling its pockets for whatever's there.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
kerry.kreitman
User


Joined: 02 Feb 2014
Posts: 29

PostPosted: Tue Jun 10, 2014 1:23 pm  Reply with quote

First of all, I'd just like to say a huge thank you to all of the experienced ANSYS users who take the time to read these posts and help out people who have much less experience using the program. I know that you all get essentially nothing out of it, and I greatly appreciate any assistance that is provided. You may not realize how much something like simply providing the name of a useful command can help someone who is struggling. And while I can only speak for myself, I imagine that the majority of the less-experienced XANSYS users do in fact go to great lengths to find the answer to their question through other sources before they post it. Despite how silly or basic the question may be, the answer can be hard to find, especially if you don't know exactly where to look.

While I've had wonderful experiences communicating with other XANSYS users in the past, it seems like some of the comments on this thread got a little bit harsh today. While I realize and agree with the fact that the forum is not a place to start from scratch learning ANSYS, it is however a great place to learn for ANSYS users of any skill level. In fact, the home page of XANSYS states that the site is "a place for the ANSYS user community to exchange ideas and help each other be more productive." The way I see it, if another forum user is willing to help me find the one command I need or points me in the right direction to accomplish what I'm trying to do, that makes me more productive. And it will do the same for the next person who has a similar question and finds the answer by searching the forum. It also helps to accelerate my learning pace so that maybe next time (or many many times down the road), I can return the favor by helping someone else figure out their current ANSYS problem. Thus, answering questions that are asked through this forum is a win for everyone.

That being said, I respect the fact that there is (and should be) a basic level of knowledge attained before posting in the forum, and that there are some questions that are in fact too basic for this setting. However, I think everyone could benefit from keeping in mind that what seems basic to someone with 25 years of experience can be very different from what seems basic to someone with only a few years under their belt.

Apologies for the long post, but the last thing I’d like to point out is that good ANSYS-learning resources are not always readily available, especially in a university setting. For example, our graduate-level FEM course is focused on the mathematics behind FEM, rather than on how to use commercial software. So while it was a very good course, I still had much to learn to actually apply the concepts I got from the class. If there was another course available to me (inside or outside the university) that was more specific to ANSYS, I’d sign up in a heartbeat. Unfortunately though, there is not. For now at least, I’m largely working through the challenge of learning the program on my own. I imagine that this is a similar situation in which many students around the world are struggling through, and forums such as this one are very valuable learning tools to supplement that education.

I have hopes that this super long post has perhaps instilled a bit more patience and tolerance in some of the more experienced users of the forum. I also hope that going forward, those who are newer to ANSYS can do a good job of recognizing the purpose of the forum and develop a good understanding for appropriate questions to ask (and ways in which to ask them).

FINALLY! A quick disclaimer: I mean no offense to anyone through anything I’ve written here. I’ve taken great care to try to be objective on this subject and present a point of view that may not always be considered when posting. I apologize if any of it rubbed anyone the wrong way – that was not my intention. I have great respect for the XANSYS forum, those who maintain it, and those who actively participate on it, and I am very grateful for its existence. And if you've made it all the way through all of my rambling above, congrats :)

Regards,
Kerry
_________________
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 10, 2014 10:54 pm  Reply with quote

On Jun 10, 2014, at 3:23 PM, kerry.kreitman wrote:

Quote:
FINALLY! A quick disclaimer: I mean no offense to anyone through
anything Ive written here.

None taken. SO here's a clarification and a bit of advice that may
serve you well.

The clarification is that the list is intended as a discussion
resource--give and take. Occasionally subscribers (you saw that
yesterday) need reminding that it's not just a focal point for
questions when someone wants some hand-holding. The The list expects
sensible, well-thought out questions with some indication that
there's some study and effort made to find an answer. Failure to ask
questions intelligently carries consequences.

The advice is this--don't lecture your betters, of which the list
numbers plenty. Obviously you meant no offense, but those who have
been subscribers for 10-15 years may find your post presumptuous.
When you've been in the engineering biz for 20 years you'll know
enough about the profession to be able to take liberties


Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
martin.liddle
Site Admin


Joined: 21 Oct 2008
Posts: 152

PostPosted: Wed Jun 11, 2014 2:23 am  Reply with quote

On 10/06/2014 21:23, kerry.kreitman wrote:
Quote:
First of all, I'd just like to say a huge thank you to all of the experienced ANSYS users who take the time to read these posts and help out people who have much less experience using the program. I know that you all get essentially nothing out of it, and I greatly appreciate any assistance that is provided. You may not realize how much something like simply providing the name of a useful command can help someone who is struggling. And while I can only speak for myself, I imagine that the majority of the less-experienced XANSYS users do in fact go to great lengths to find the answer to their question through other sources before they post it. Despite how silly or basic the question may be, the answer can be hard to find, especially if you don't know exactly where to look.

The fundamental problem is that the most knowledgeable people here are
also very busy people and they don't like getting enormous volumes of
email on trivial questions. We (as a community) do not want to lose
their knowledge so I am afraid we have to apply some limits to people
who feel entitled to excessive hand holding. The solution will be to
have a separate section of XANSYS devoted to beginners and only those
old hands with time on their hands will subscribe. The problem is that
the current XANSYS infrastructure is extremely creaky and I certainly do
not want to tamper with it. We have started to evaluate possible
software replacements but that takes time and I have been too busy
recently to do any work on it.
--
Martin Liddle, XANSYS Moderator, 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 |
+-------------------------------------------------------------+

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
kerry.kreitman
User


Joined: 02 Feb 2014
Posts: 29

PostPosted: Wed Jun 11, 2014 7:29 am  Reply with quote

Martin and Christopher,

I completely understand and respect the purpose of the forum, the physical limitations of the forum server, and the impracticality of the most experienced users taking valuable time from their days to answer the smallest of questions. The intent of my post was merely to encourage a bit more understanding and tolerance of those who are less experienced and tend to post more trivial questions, while also attempting to make them aware of why such trivial questions can be inappropriate to be posting on this site.

Kerry
_________________
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)
Back to top
View user's profile Send private message
jan.blazek
User


Joined: 08 Apr 2014
Posts: 5

PostPosted: Wed Jun 11, 2014 5:02 pm  Reply with quote

Dear Philippe and other experts,

first of all I would like to thank you for giving all valuable advice free of charge, it is really encouraging to see platform like this one.

Lets change a question, you as experts are familiar with FEM calculations especially in Ansys, and therefore you can see far far away in FEM. Lets have a look on future of FEM. Imagine you are begginers as most of us and try to guess what the future of FEM is. There are meshless methods, there are other FEM software, some of them are even under General Public License. In CFD there is for example openfoam having GPL license with strong support partner. What will be your decision about FEM software to work with, except ANSYS that is a must.

Hope I am not too much curious.

Jan Blažek

Project Engineer
Rizzo Associates Czech
-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Phil Vidori
Sent: Wednesday, June 11, 2014 4:44 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] [APDL] Saving and resuming results from an analysis

The problem is that you
need to ( in order ):

1) Crawl
2) Walk
3) Run
4) Fly

And a lot of new users on this list
think that will fly on day 1.
FEA and ANSYS are complex topics,
and new users must show some effort
by Reading The F.....g Manual,
verification manual examples,
learn the basics of FEA ( if you're new to FEA as well ).

I did find your answer presumptuous, since the experts in this list are paid ( zero + zero = zero ) to help out...
Show some good will and you won't get hit over the head.

p.



Philippe Vidori, ing. M.Sc.A.
Services Techniques D.O.F. Technical Services 35, 111ième Ave. Ouest / 35, 111th Ave. West Blainville, QC J7C 4N8 t.450.970.1847/ f.450.979.0789 / c.514.803.4805 philvid@videotron.ca







-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of kerry.kreitman
Sent: Wednesday, June 11, 2014 10:30 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [APDL] Saving and resuming results from an analysis

Martin and Christopher,

I completely understand and respect the purpose of the forum, the physical limitations of the forum server, and the impracticality of the most experienced users taking valuable time from their days to answer the smallest of questions. The intent of my post was merely to encourage a bit more understanding and tolerance of those who are less experienced and tend to post more trivial questions, while also attempting to make them aware of why such trivial questions can be inappropriate to be posting on this site.

Kerry

------------------------
Kerry Kreitman
PhD Student
The University of Texas at Austin (USA)






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+


---
This email is free from viruses and malware because avast! Antivirus protection is active.
http://www.avast.com

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

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


Joined: 26 Jun 2015
Posts: 9

PostPosted: Wed Jul 15, 2015 12:17 pm  Reply with quote

kerry.kreitman wrote:
Hello everyone,

I have a question regarding which ANSYS-created files I need to be saving to be able to later resume the database and examine the results. Despite reading through the ANSYS documentation and many forum and google searches, I still don't quite understand it yet.

Based on everything I've read, I thought that if I saved the .db file using SAVE,jobname,db,,SOLU the nodal and elemental results would be saved along with the model data in the .db file. However, after deleting the .rst files and reloading the database using RESUME,jobname,db, I cannot access the results. For example, using SET,LIST I get the message "An error occurred while attempting to open the results file jobname.rst", which makes complete sense because the .rst file doesn't exist.

Is there a different way to access the results through the saved database? Or do I always need to keep the .rst file to go back and re-visit the results in the future? Are there any other files that I need as well?

Thanks in advance!
Kerry


A full disk would also yield to the same error... :D
_________________
Primož Ogrinec
Faculty of Mechanical Engineering
University of Ljubljana
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