XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[Xansys] Modal - Large file size
 
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
thomas.wittenschlaeger
User


Joined: 25 Apr 2014
Posts: 4

PostPosted: Wed May 28, 2014 12:37 am  Reply with quote

Hello everyone,



I am receiving a full disk error as Ansys tries to write the results of a Modal analysis I am performing. It is clear that this is indeed the problem as I have about 200 GB available on my hard drive and when I examine the printout for the disk and directory usage, I see that one file, file.P78 is almost 177 GB large. Does anyone know what this file is? Googling and checking previous XANSYS threads turned up nothing so far for me. I can't imagine why it would be this large.



My case is average with on average 1 million nodes and I ask for only 6 eigen frequencies. The only thing that I can think of is that my case has about 45 springs in it and this is causing a large data amount jump.



I am using ANSYS WB V13. Any help is much appreciated.



Mit besten GrŘ▀en - with kind regards



Thomas Wittenschlaeger

Engineering



FAB Bertelmann Technologie

+-------------------------------------------------------------+
| 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
bhaumik.dave
User


Joined: 11 Dec 2013
Posts: 13
Location: Ahmedabad

PostPosted: Wed May 28, 2014 12:43 am  Reply with quote

Hello,
ANSYS WB have options wherein you can save the files(Please check the
dialogue box of Analysis options) and explore "Data" options so that you can
find it.
Orelse, if you could, please send the .cdb file to me or share the .inp file
so that I can take a look.

Regards,
Bhaumik Dave
Sr. FEA Specialist
Hi Tech Outsourcing Services,
Gujarat,
India
PH: +919879488468

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
Wittenschlaeger, Thomas
Sent: Wednesday, May 28, 2014 1:08 PM
To: xansys@xansys.org
Subject: [Xansys] Modal - Large file size

Hello everyone,



I am receiving a full disk error as Ansys tries to write the results of a
Modal analysis I am performing. It is clear that this is indeed the problem
as I have about 200 GB available on my hard drive and when I examine the
printout for the disk and directory usage, I see that one file, file.P78 is
almost 177 GB large. Does anyone know what this file is? Googling and
checking previous XANSYS threads turned up nothing so far for me. I can't
imagine why it would be this large.



My case is average with on average 1 million nodes and I ask for only 6
eigen frequencies. The only thing that I can think of is that my case has
about 45 springs in it and this is causing a large data amount jump.



I am using ANSYS WB V13. Any help is much appreciated.



Mit besten GrŘ▀en - with kind regards



Thomas Wittenschlaeger

Engineering



FAB Bertelmann Technologie

+-------------------------------------------------------------+
| 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 Send e-mail
thomas.wittenschlaeger
User


Joined: 25 Apr 2014
Posts: 4

PostPosted: Wed May 28, 2014 1:35 am  Reply with quote

Hello Mr. Bhaumik,

Thanks for the quick reply. I checked the dialogue box that you suggested however nothing there is relevant to my situation. I am guessing the main problem is that I don't understand how the system is saved in the different ansys files because I am generating files that are just too big. For example, when I examine the .mode file, it is also quite big, 390 MB for only 6 eigen frequencies requested. I have run a larger simulation (larger in terms of nodes) and I didn't have such huge files but for some reason now I do.

Unfortunately I cannot send the .ind or .cdb files because it is a simulation for a client and this is confidential. I understand that this severely limits any help that can be provided but I had hoped that maybe someone had some ideas that may prove valuable.


Mit besten Gr├╝├čen - with kind regards
 
Thomas Wittenschlaeger
Engineering
 
FAB Bertelmann Technologie

-----Urspr├╝ngliche Nachricht-----
Von: Xansys [mailto:xansys-bounces@xansys.org] Im Auftrag von Bhaumik Dave
Gesendet: Mittwoch, 28. Mai 2014 09:43
An: 'ANSYS User Discussion List'
Betreff: Re: [Xansys] Modal - Large file size

Hello,
ANSYS WB have options wherein you can save the files(Please check the dialogue box of Analysis options) and explore "Data" options so that you can find it.
Orelse, if you could, please send the .cdb file to me or share the .inp file so that I can take a look.

Regards,
Bhaumik Dave
Sr. FEA Specialist
Hi Tech Outsourcing Services,
Gujarat,
India
PH: +919879488468

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Wittenschlaeger, Thomas
Sent: Wednesday, May 28, 2014 1:08 PM
To: xansys@xansys.org
Subject: [Xansys] Modal - Large file size

Hello everyone,



I am receiving a full disk error as Ansys tries to write the results of a Modal analysis I am performing. It is clear that this is indeed the problem as I have about 200 GB available on my hard drive and when I examine the printout for the disk and directory usage, I see that one file, file.P78 is almost 177 GB large. Does anyone know what this file is? Googling and checking previous XANSYS threads turned up nothing so far for me. I can't imagine why it would be this large.



My case is average with on average 1 million nodes and I ask for only 6 eigen frequencies. The only thing that I can think of is that my case has about 45 springs in it and this is causing a large data amount jump.



I am using ANSYS WB V13. Any help is much appreciated.



Mit besten Gr├╝├čen - with kind regards



Thomas Wittenschlaeger

Engineering



FAB Bertelmann Technologie

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


+-------------------------------------------------------------+
| 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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Wed May 28, 2014 3:09 am  Reply with quote

Dear Mr. Wittenschlaeger,

since the .mode file is 390 MB for 6 eigenmodes, that gives 390/6=65 MB
per eigenmode. Since your model has aproximately 1 million nodes, you
can calculate the number of bytes stored per node as 65 MB/ 1 Million
nodes= 6.5 bytes/node. In each node there are several degrees of freedom
that need to be stored: for example, 3 displacements for structural
SOLID models, or 6 d.o.f. (3 displacements and 3 rotations) in BEAM and
SHELL models. I can guess that your model is solid, which gives (6.5
bytes/node) / (3 dof/node)=2.2 bytes/dof., which is roughly 2 bytes/dof,
the memory required by a double-precision floating point number.

Your file size seems reasonable.

You may consider using the reduced method and selecting a lower number
of master DOF to reduce . You have to be careful, because your results
will depend on the DOF selected.

You may also consider buying an external HDD with a fast connection
(SATA3, USB3, thunderbolt). You could place your ansys working directory
there.

Best regards,

Jose M. Galan

Assistant Professor

Dept. Engineering Construction

Universidad de Sevilla

El 28/05/2014 10:35, Wittenschlaeger, Thomas escribi├│:

Quote:
Hello Mr. Bhaumik,

Thanks for the quick reply. I checked the dialogue box that you suggested however nothing there is relevant to my situation. I am guessing the main problem is that I don't understand how the system is saved in the different ansys files because I am generating files that are just too big. For example, when I examine the .mode file, it is also quite big, 390 MB for only 6 eigen frequencies requested. I have run a larger simulation (larger in terms of nodes) and I didn't have such huge files but for some reason now I do.

Unfortunately I cannot send the .ind or .cdb files because it is a simulation for a client and this is confidential. I understand that this severely limits any help that can be provided but I had hoped that maybe someone had some ideas that may prove valuable.

Mit besten Gr├╝├čen - with kind regards

Thomas Wittenschlaeger
Engineering

FAB Bertelmann Technologie

+-------------------------------------------------------------+
| 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
thomas.wittenschlaeger
User


Joined: 25 Apr 2014
Posts: 4

PostPosted: Wed May 28, 2014 7:39 am  Reply with quote

Dear Mr. Galan,

Thank you for the answer. It cleared up and explained a lot for me. One question remains, do you know what the file file.P77 is? This is actually the huge problem...it is 200 GB. I can't imagine what it is used to do. Fo

Mit besten Gr├╝├čen - with kind regards
 
Thomas Wittenschlaeger
Engineering
 
FAB Bertelmann Technologie

´üÉ Before printing this email, assess if it is really needed

-----Urspr├╝ngliche Nachricht-----
Von: Xansys [mailto:xansys-bounces@xansys.org] Im Auftrag von mfernan@us.es
Gesendet: Mittwoch, 28. Mai 2014 12:09
An: ANSYS User Discussion List
Betreff: Re: [Xansys] Modal - Large file size



Dear Mr. Wittenschlaeger,

since the .mode file is 390 MB for 6 eigenmodes, that gives 390/6=65 MB per eigenmode. Since your model has aproximately 1 million nodes, you can calculate the number of bytes stored per node as 65 MB/ 1 Million nodes= 6.5 bytes/node. In each node there are several degrees of freedom that need to be stored: for example, 3 displacements for structural SOLID models, or 6 d.o.f. (3 displacements and 3 rotations) in BEAM and SHELL models. I can guess that your model is solid, which gives (6.5
bytes/node) / (3 dof/node)=2.2 bytes/dof., which is roughly 2 bytes/dof, the memory required by a double-precision floating point number.

Your file size seems reasonable.

You may consider using the reduced method and selecting a lower number of master DOF to reduce . You have to be careful, because your results will depend on the DOF selected.

You may also consider buying an external HDD with a fast connection (SATA3, USB3, thunderbolt). You could place your ansys working directory there.

Best regards,

Jose M. Galan

Assistant Professor

Dept. Engineering Construction

Universidad de Sevilla

El 28/05/2014 10:35, Wittenschlaeger, Thomas escribi├│:

Quote:
Hello Mr. Bhaumik,

Thanks for the quick reply. I checked the dialogue box that you suggested however nothing there is relevant to my situation. I am guessing the main problem is that I don't understand how the system is saved in the different ansys files because I am generating files that are just too big. For example, when I examine the .mode file, it is also quite big, 390 MB for only 6 eigen frequencies requested. I have run a larger simulation (larger in terms of nodes) and I didn't have such huge files but for some reason now I do.

Unfortunately I cannot send the .ind or .cdb files because it is a simulation for a client and this is confidential. I understand that this severely limits any help that can be provided but I had hoped that maybe someone had some ideas that may prove valuable.

Mit besten Gr├╝├čen - with kind regards

Thomas Wittenschlaeger
Engineering

FAB Bertelmann Technologie

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


Joined: 17 Jun 2009
Posts: 927

PostPosted: Wed May 28, 2014 10:21 am  Reply with quote

On May 28, 2014, at 3:35 AM, Wittenschlaeger, Thomas wrote:

Quote:
For example, when I examine the .mode file, it is also quite big,
390 MB for only 6 eigen frequencies requested. I have run a larger
simulation (larger in terms of nodes) and I didn't have such huge
files but for some reason now I do.

The simple answer is that your model is just too damn big. Three
million DOF makes for big files, especially in a modal analysis. No
point in a model that size if you're only going after 6 modes. If you
could resurrect Ludwig Durr he'd give you the first six modes of the
Hindenburg with a pencil and a few sheets of paper in an afternoon.

Try using Guyan reduction with about 20 MDOF that would describe the
kind of motion you'd expect. (Transverse displacement for bending
modes for example.) Also make sure that you haven't inadvertently
expanded more than the 6 eigenvectors you've requested. Check the
output listing to see what ANSYS thinks you've asked for.


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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Wed May 28, 2014 11:15 am  Reply with quote

Dear Mr. Wittenschlaeger,

You may find some useful information in the following sections of the
ansys documentation:

* Ansys documentation > Mechanical APDL > Performance Guide > 4. Ansys
memory usage and Performance> 4.1.3. Modal (Eigensolvers) Solver Memory
Usage help/ans_per/perlineqsolv.html#perlineqsolv_sparse
* Ansys documentation > Mechanical APDL > Basic Analysis Guide >20.
File Management and Files > 20.4.2. Files that ANSYS Writes
help/ans_bas/Hlp_G_BAS18_4.html

In the former section you will find estimates of the memory usage and
I/O file size for the different eigensolvers. For example, for a
Block-Lanczos solver running out-of-core, the file size estimate is
15-20 GB/MDOF. Since your model has about 6 million DOF, the file size
estimate is about 90-120 GB, which is similar to the 177 GB files you
found.

In the latter section there is a list of temporary and permanent files
written by the Ansys program. Unfortunately, I have not seen the
extension .P77. The closest extension is PCn, which is a scratch binayr
file for PCG solver (n being an intenger number).

Best regards,

Jose M. Galan

Assistant Professor

Dept. Engineering Construction

Universidad de Sevilla


+-------------------------------------------------------------+
| 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
chean.lee
User


Joined: 01 Feb 2012
Posts: 21

PostPosted: Wed May 28, 2014 2:29 pm  Reply with quote

Perhaps, you could quickly solve this problem by installing a bigger hdd?

200gb is nothing when it comes to acoustic simulations. 1 million nodes is massive. My work with 100k elements and 500 load steps, I need around 50 to 100gb.

Chean Lee, PhD
Research Student
Electronics and Ultrasonics Engineering
General Engineering Research Institute
Liverpool John Moores University

+-------------------------------------------------------------+
| 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)
_________________
Chean Lee
Research Student
General Engineering Research Institute
Liverpool John Moores University
L3 3AF, Liverpool, UK
Back to top
View user's profile Send private message Send e-mail
thomas.wittenschlaeger
User


Joined: 25 Apr 2014
Posts: 4

PostPosted: Thu May 29, 2014 4:45 am  Reply with quote

Hello everyone,

Thanks for the help in diagnosing this problem. The overwhelming opinion is that the case is too big. I will give the last suggestions a try to see if I can manage it. If not, well time to invest in a bigger harddrive.

Mit besten GrŘ▀en - with kind regards
á
Thomas Wittenschlaeger
Engineering
á
FAB Bertelmann Technologie

-----UrsprŘngliche Nachricht-----
Von: Xansys [mailto:xansys-bounces@xansys.org] Im Auftrag von Christopher Wright
Gesendet: Mittwoch, 28. Mai 2014 19:21
An: ANSYS User Discussion List
Betreff: Re: [Xansys] Modal - Large file size


On May 28, 2014, at 3:35 AM, Wittenschlaeger, Thomas wrote:

Quote:
For example, when I examine the .mode file, it is also quite big, 390
MB for only 6 eigen frequencies requested. I have run a larger
simulation (larger in terms of nodes) and I didn't have such huge
files but for some reason now I do.

The simple answer is that your model is just too damn big. Three million DOF makes for big files, especially in a modal analysis. No point in a model that size if you're only going after 6 modes. If you could resurrect Ludwig Durr he'd give you the first six modes of the Hindenburg with a pencil and a few sheets of paper in an afternoon.

Try using Guyan reduction with about 20 MDOF that would describe the kind of motion you'd expect. (Transverse displacement for bending modes for example.) Also make sure that you haven't inadvertently expanded more than the 6 eigenvectors you've requested. Check the output listing to see what ANSYS thinks you've asked for.


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


+-------------------------------------------------------------+
| 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
peter.attar
User


Joined: 21 Oct 2008
Posts: 67

PostPosted: Thu May 29, 2014 4:53 am  Reply with quote

If it is absolutely necessary to have that many degrees of freedom to properly resolve the first 6 modes (which would seem doubtful and which you should check via convergence study), you may want to look into component mode synthesis another "reduced" option which can be used instead of the Guyan reduction Mr. Wright mentioned.

Peter

Peter Attar
Associate Professor
Graduate Student Liaison
The University of Oklahoma
School of Aerospace and Mechanical Engineering
865 Asp Ave.
Felgar Hall Room 212
Norman, OK 73019-1052
phone:405-325-1749
fax:405-325-1088

________________________________________
From: Xansys [xansys-bounces@xansys.org] on behalf of Wittenschlaeger, Thomas [wittenschlaeger@fa-b.de]
Sent: Thursday, May 29, 2014 6:45 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Modal - Large file size

Hello everyone,

Thanks for the help in diagnosing this problem. The overwhelming opinion is that the case is too big. I will give the last suggestions a try to see if I can manage it. If not, well time to invest in a bigger harddrive.

Mit besten GrŘ▀en - with kind regards

Thomas Wittenschlaeger
Engineering

FAB Bertelmann Technologie

-----UrsprŘngliche Nachricht-----
Von: Xansys [mailto:xansys-bounces@xansys.org] Im Auftrag von Christopher Wright
Gesendet: Mittwoch, 28. Mai 2014 19:21
An: ANSYS User Discussion List
Betreff: Re: [Xansys] Modal - Large file size


On May 28, 2014, at 3:35 AM, Wittenschlaeger, Thomas wrote:

Quote:
For example, when I examine the .mode file, it is also quite big, 390
MB for only 6 eigen frequencies requested. I have run a larger
simulation (larger in terms of nodes) and I didn't have such huge
files but for some reason now I do.

The simple answer is that your model is just too damn big. Three million DOF makes for big files, especially in a modal analysis. No point in a model that size if you're only going after 6 modes. If you could resurrect Ludwig Durr he'd give you the first six modes of the Hindenburg with a pencil and a few sheets of paper in an afternoon.

Try using Guyan reduction with about 20 MDOF that would describe the kind of motion you'd expect. (Transverse displacement for bending modes for example.) Also make sure that you haven't inadvertently expanded more than the 6 eigenvectors you've requested. Check the output listing to see what ANSYS thinks you've asked for.


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


+-------------------------------------------------------------+
| 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
david.gross
User


Joined: 14 Aug 2009
Posts: 139

PostPosted: Thu May 29, 2014 7:30 am  Reply with quote

All,

You guys are bringing back "fond" memories for me. I was working as an intern at in the central engineering department of a very large company. The year was 1988, the ANSYS version was 4.2, the computer was an IBM PS/2 Model 80, with an Intel 386 processor, including a math co-processor -- it was the hottest computer the department had under any engineer's desk.

I had a task to do a modal analysis of a particular structure. The department didn't have any FEA experts to mentor me, so I was blazing my own path. Back in those days, there was no automated mesh generation -- you sat down with your drawings and sketches, made a mesh plan that suited your gut instincts, and started building it. If you decided that you wanted a different mesh density, then to some degree or other, you simply had to start over.

So I went and made my model, and it didn't fit in the confines of my state-of-the-art PC. Ran for a week, and then died when it filled the hard drive. Couldn't even make use of any results after if finished either.

Desperate, we got in contact with our local ASD and told them what was going on. They put us in touch with another very large company in their region that had ANSYS running on a some sort of big-iron mainframe. I sent them my batch listing, and got on a plane so I could review the results on their vector-graphics monitor. Not counting travel, I think several thousand dollars traded hands for this service.

When I got back to my PC, I started work on a model with a basic element size about twice as big as the original. Guess what? Same results as the big model, ran in a few hours on my PC, and fit on the hard drive no problem. A very expensive lesson learned at my employer's expense, and it is simply stated as follows:

Always, always, always start with a very coarse model that runs in minutes -- to ensure you have all your physics, boundary conditions, etc. right and that the model will run to completion. Only then, step up to successively finer models that get you to your final result. And while you're doing that, remember that you can always find a way to exceed the resources you have, and it is your job to get the best answer that you can while working within the resources you have available.

I'm sure many in the OFB have their own version of this war story. I'm glad I wasn't fired on the spot, but I learned my lesson for sure.

Regards,

David Gross
Dominion Engineering, Inc.


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Phil Vidori
Sent: Thursday, May 29, 2014 8:26 AM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Modal - Large file size

6 million dofs for a structural modal analysis is way way way too big.
If you were my employee, I would fire you on the spot ! ;-)

+-------------------------------------------------------------+
| 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
chuck.ritter
User


Joined: 21 Oct 2008
Posts: 165

PostPosted: Thu May 29, 2014 8:49 am  Reply with quote

Phil

I had occasion to run modal analysis on a 2
million DOF problem last year. The model
refinement was governed by other requirements and
I could either hive off a separate lower
refinement model or gamble I could get that pig
through. Worse, there was a wide band shock
spectrum, so 94 modes in 10khz to process. An
80GB results file was created, but I didn't see
anything approaching a 200GB scratch file. Ansys
Classic, btw. The mode combinations took a lot
longer than the solution - and I wasn't happy
having to select from the half dozen combination
procedures, either. No One True Answer coming out of that smorgasbord.

regards

Chuck Ritter
JAR Associates
North Kingstown RI 02852


At 08:25 AM 5/29/2014, you wrote:
Quote:
6 million dofs for a structural modal analysis is way way way too big.
If you were my employee, I would fire you on the spot ! ;-)

Joking aside, I never worked on acoustic problems so I can't talk from
experience.
When I performed a modal analysis to get the first 6 to 8 modes,
I was interested in the ones exhibiting the highest energy and
highest effective mass. The higher modes aren't useful.
I saw Guyan reduction pass by in the previous posts. Chris,
I'm not sure It's still available as an option.

On the other hand, acoustic analysis may require many modes
and a finer mesh.



Best regards,

p.




Philippe Vidori, ing. M.Sc.A.
Services Techniques D.O.F. Technical Services
35, 111iŔme 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 Attar, Peter J.
Sent: Thursday, May 29, 2014 7:54 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Modal - Large file size

If it is absolutely necessary to have that many degrees of freedom to
properly resolve the first 6 modes (which would seem doubtful and which you
should check via convergence study), you may want to look into component
mode synthesis another "reduced" option which can be used instead of the
Guyan reduction Mr. Wright mentioned.

Peter

Peter Attar
Associate Professor
Graduate Student Liaison
The University of Oklahoma
School of Aerospace and Mechanical Engineering
865 Asp Ave.
Felgar Hall Room 212
Norman, OK 73019-1052
phone:405-325-1749
fax:405-325-1088

________________________________________
From: Xansys [xansys-bounces@xansys.org] on behalf of Wittenschlaeger,
Thomas [wittenschlaeger@fa-b.de]
Sent: Thursday, May 29, 2014 6:45 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Modal - Large file size

Hello everyone,

Thanks for the help in diagnosing this problem. The overwhelming opinion is
that the case is too big. I will give the last suggestions a try to see if I
can manage it. If not, well time to invest in a bigger harddrive.

Mit besten GrŘ▀en - with kind regards

Thomas Wittenschlaeger
Engineering

FAB Bertelmann Technologie

-----UrsprŘngliche Nachricht-----
Von: Xansys [mailto:xansys-bounces@xansys.org] Im Auftrag von Christopher
Wright
Gesendet: Mittwoch, 28. Mai 2014 19:21
An: ANSYS User Discussion List
Betreff: Re: [Xansys] Modal - Large file size


On May 28, 2014, at 3:35 AM, Wittenschlaeger, Thomas wrote:

Quote:
For example, when I examine the .mode file, it is also quite big, 390
MB for only 6 eigen frequencies requested. I have run a larger
simulation (larger in terms of nodes) and I didn't have such huge
files but for some reason now I do.

The simple answer is that your model is just too damn big. Three million DOF
makes for big files, especially in a modal analysis. No point in a model
that size if you're only going after 6 modes. If you could resurrect Ludwig
Durr he'd give you the first six modes of the Hindenburg with a pencil and a
few sheets of paper in an afternoon.

Try using Guyan reduction with about 20 MDOF that would describe the kind of
motion you'd expect. (Transverse displacement for bending modes for
example.) Also make sure that you haven't inadvertently expanded more than
the 6 eigenvectors you've requested. Check the output listing to see what
ANSYS thinks you've asked for.


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


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


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

Chuck Ritter
JAR Associates Inc
70 Romano Vineyard Way
North Kingstown, RI
www.jar.com
401-294-4589
401-835-4465 (cell)
+-------------------------------------------------------------+
| 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: Fri May 30, 2014 10:35 am  Reply with quote

On May 29, 2014, at 11:58 AM, Phil Vidori wrote:

Quote:
Unfortunately, if the goal is to determine stress via a harmonic
or random runs, we need a fine mesh in the region(s) of
interest. In this case, the mode combination takes much
longer than the solution and is a real pain.
There are a few ways around that, which I've employed on occasion.
--A model can be coarse and still get you reasonable frequencies. The
mass and stiffness matrices aren't inescapably corrupted by a rough
mesh, and those matrices determine the frequencies. Only modes that
involve significant regions of the model are going to be significant
anyway. The really important thing is getting the weights right. A
somewhat coarse mesh saves enough time so you can run a couple of
cases on either side to see if you're close enough.

--Review the mode coefficients and effective masses to determine
significant modes. Properly done, this review provides all the
evidence needed to show that you've ignored the insignificant modes
because they're insignificant, and that you haven't wasted his
valuable time expanding a lot of trash modes. A good thing about FEA
is that the customer isn't always right.

--Knowing the significant modes makes it easier to narrow down the
number of stress passes you need for harmonic analysis or mode
combination. If I were forced to run a million node model because I
needed to figure a stress concentration for a harmonic analysis, I'd
prefer running a sub model to doing a full modal extraction on a
couple of hundred modes, most of which would be of no value. Better
yet, use a handbook stress concentration factor--modal analysis isn't
all that precise (compared to, say, sine sweep results) because the
model weights and boundary condition stiffnesses may be off. And
modal combinations, even the revered CQC method or Navy
methodologies, have their own inaccuracies.

Quote:
When I was talking about firing someone, it comes back to
a time that I had to train someone on NX (Unigraphics) and
NX-Nastran.
I think that firing someone for running a grossly overmeshed model
was a bit severe. You should have fired him for not checking with you
first. If he felt insulted when you gave him good advice, you
probably didn't rattle his cage hard enough. Raking someone over the
coals should leave the guy grateful he wasn't on the street at that
very moment. And just out of curiosity, which language is better for
that--French or English?

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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 03, 2014 11:28 am  Reply with quote

On Jun 3, 2014, at 8:14 AM, Phil Vidori wrote:

Quote:
I didn't know that submodeling could be used for modal / harmonic /
random
analyses.
I have to be honest and say I never used it in practice, but I'm sure
it can be done if you're careful about it. In efect you'd be
operating on particular load steps saved off to the results files no
differently than static load steps. With time domain analysis you'd
just cut out a piece at a load step of interest and do the
submodeling with the instantaneous displacements as boundary
conditions. You should be able to do the same thing with harmonic
analysis, with the saved off load step from the frequency of
interest, which you'd determine from POST26.

With response spectrum analysis or random response it's a bit
trickier because you'd be dealing with combined modal responses, with
displacements taken without reference to sign. That makes the imposed
displacements seem to be all positive when in fact both signs are
equally probable. If I were going to do it, I'd identify the highest
peak stress from the combined results and try to identify the mode
which governs that response, by comparing the modal stress and
displacement profile to the combined stress profile. Then you could
do the submodeling with results from the governing mode. I might also
scale up the submodel results by the ratio of the maximum
displacement from the combined results to the corresponding modal
displacement, because that feels right intuitively. Then to satisfy
my curiosity and my compulsion for back-checking, I'd do the submodel
from the combined modal stress results to see if there was a big
difference.

The reason I think this would work is that any region small enough
for submodeling is probably 'carried along' by the overall structural
motion so the submodel displacements would all be the same sign
anyway. So the unsigned displacements at the cut boundary wouldn't
have different signs anyway. I don't think you'd need to worry about
inertial loading within the submodel because it isn't especially
massive. And again, to be compulsive, You could try a third approach,
namely imposing the signs of the displacements taken from the
governing mode onto the combined (unsigned) displacements and doing
the submodel on that load case. You can do that combination with
LCCALC. That should be the most accurate of all.

So what do you think--possible?

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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jun 10, 2014 11:21 am  Reply with quote

On Jun 9, 2014, at 9:35 AM, Phil Vidori wrote:

Quote:

I personally used it for static stress in the past,
so I was surprised when you came up with cut boundary
displacement for modal analysis.
I bet you could write off a load step from a harmonic analysis to a
second rst file, and use it to restart with a submodel. There are
things you'd need to be careful with such as loading and the
possibility of closely-spaced modes, but I suspect that just about
any analysis type could be used. I doubt that a small piece of a
model would carry enough inertia loading to affect the results
greatly--most of the dynamic loading concentrates at areas of large
displacement, which stress concentrations tend to be pretty highly
restrained--almost encapsulated. I think if you were careful, you
could probably get something useful out of combined

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
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