XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Load cases for fatigue 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
michele.cerullo
User


Joined: 04 Jun 2014
Posts: 4
Location: Copenhagen

PostPosted: Mon Jun 16, 2014 11:40 am  Reply with quote

Dear all,
I would like to calculate the stress intensity factor, according to LEFM, at a crack tip, during a varying load. For this reason I divided the load in "itimef" values and I created a loop in a macro that may look like

Code:
input.mac        !define input parameters
geom.mac        !create geometry
mesh.mac        !mesh geometry
bc.mac             !apply Boundary conditions
*do,itime,1,itimef
       load.mac         !apply load(itime)
       sol.mac           !solve
       sifcalc.mac     !calculate SIF
*enddo


At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like to save all the
solutions, for each time steps. If I save at the end of every loop though, it overwrites the results from previous computations. Moreover I would like to avoid to save different jobnames for each time step. I tried with load cases but I cannot manage it to work. Does anybody have some suggestions please?

Best,
Michele
Back to top
View user's profile Send private message
danbohlen
User


Joined: 18 Aug 2008
Posts: 951
Location: Evendale OH

PostPosted: Mon Jun 16, 2014 11:44 am  Reply with quote

The results should show up as separate set of results for each.

The only way to save the .dbs (no reason why you should need to) would be new names.

And unless there is some big nonlinearity in your model the SI factor should scale with the load I believe.

If the above doesn't cut it for you, you might need to post snippets of the macros below. You tell us what they are doing, but they might be doing more than you think!


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 1-513-243-2366



-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of michele.cerullo
Sent: Monday, June 16, 2014 2:40 PM
To: xansys@xansys.org
Subject: [Xansys] Load cases for fatigue analysis

Dear all,
I would like to calculate the stress intensity factor, according to LEFM, at a crack tip, during a varying load. For this reason I divided the load in "itimef" values and I created a loop in a macro that may look like


Code:
input.mac !define input parameters
geom.mac !create geometry
mesh.mac !mesh geometry
bc.mac !apply Boundary conditions
*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
sifcalc.mac !calculate SIF
*enddo



At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like to save all the solutions, for each time steps. If I save at the end of every loop though, it overwrites the results from previous computations. Moreover I would like to avoid to save different jobnames for each time step. I tried with load cases but I cannot manage it to work. Does anybody have some suggestions please?

Best,
Michele






+-------------------------------------------------------------+
| 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)
_________________
Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Mon Jun 16, 2014 5:09 pm  Reply with quote

Dear Mr. Cerullo,
if you are performing a linear static analysis (antype,static), you can
define multiple load steps that will be stored in the same ansys
database by default (outres,all,all). Ansys provides several methods to
define and solve multiple load steps. I reccommend you to read the ansys
manual for more details:

Basic Guide > Chapter 3. Solution > 3.7. Solving Multiple Load Steps

The simplest method is the multiple SOLVE method. "It involves issuing
the SOLVE [1] command after each load step is defined. The main
disadvantage, for interactive use, is that you have to wait for the
solution to be completed before defining the next load step. A typical
command stream for the multiple SOLVE [1]method is shown below:

/SOLU
...
! Load step 1:
D,...
SF,...
SOLVE ! Solution for load step 1
! Load step 2
F,...
SF,...
...
SOLVE ! Solution for load step 2
Etc.

". The text and example are taken from the manual.

However, if you leave the solution module (with the command finish or
entering other module) and then reenter (/solu), when you issue a solve
command you will start over with load step 1, losing all the previously
calculated results. This looks like what it is happening to you.

At some point in one (or more) of the macros inside your *do loop, you
are leaving the solution module. When you reenter the solution module in
the next iteration, you overwrite the previous results.

You should review your macros in order to avoid leaving the solution
module.

I would reccommend you to divide you loop in two consecutive loops, the
first one to calculate the solutions to all the load steps, and the
second one to postprocess the results to obtain the sif. You have to
make sure that in the first loop the macros do not leave the solution
module at any point.

! First loop: solve all load steps

! Make sure that you do not leave the solution module at any point

/solu

antype,static,new

*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
*enddo

! Second loop: postproccess the results of all load steps.

! All the results are stored in the same database, as different load
steps

*do,itime,1,itimef
sifcalc.mac !calculate SIF
*enddo

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 16/06/2014 20:40, michele.cerullo escribió:

Dear all,
I would like to calculate the stress intensity factor, according to
LEFM, at a crack tip, during a varying load. For this reason I divided
the load in "itimef" values and I created a loop in a macro that may
look like

Code:
input.mac !define input parameters
geom.mac !create geometry
mesh.mac !mesh geometry
bc.mac !apply Boundary conditions
*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
sifcalc.mac !calculate SIF
*enddo

At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like
to save all the
solutions, for each time steps. If I save at the end of every loop
though, it overwrites the results from previous computations. Moreover I
would like to avoid to save different jobnames for each time step. I
tried with load cases but I cannot manage it to work. Does anybody have
some suggestions please?

Best,
Michele

Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html
+-------------------------------------------------------------+
| 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: Mon Jun 16, 2014 5:21 pm  Reply with quote

By the way, you should follow xansys netiquette and include your full
affiliation in all your posts (http://www.xansys.org/rules.html [4]).
There are consequences for not complying with the rules.

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 17/06/2014 02:09, mfernan@us.es escribió:

Quote:
Dear Mr. Cerullo,
if you are performing a linear static analysis (antype,static), you can
define multiple load steps that will be stored in the same ansys
database by default (outres,all,all). Ansys provides several methods to
define and solve multiple load steps. I reccommend you to read the ansys
manual for more details:

Basic Guide > Chapter 3. Solution > 3.7. Solving Multiple Load Steps

The simplest method is the multiple SOLVE method. "It involves issuing
the SOLVE [1] command after each load step is defined. The main
disadvantage, for interactive use, is that you have to wait for the
solution to be completed before defining the next load step. A typical
command stream for the multiple SOLVE [1]method is shown below:

/SOLU
...
! Load step 1:
D,...
SF,...
SOLVE ! Solution for load step 1
! Load step 2
F,...
SF,...
...
SOLVE ! Solution for load step 2
Etc.

". The text and example are taken from the manual.

However, if you leave the solution module (with the command finish or
entering other module) and then reenter (/solu), when you issue a solve
command you will start over with load step 1, losing all the previously
calculated results. This looks like what it is happening to you.

At some point in one (or more) of the macros inside your *do loop, you
are leaving the solution module. When you reenter the solution module in
the next iteration, you overwrite the previous results.

You should review your macros in order to avoid leaving the solution
module.

I would reccommend you to divide you loop in two consecutive loops, the
first one to calculate the solutions to all the load steps, and the
second one to postprocess the results to obtain the sif. You have to
make sure that in the first loop the macros do not leave the solution
module at any point.

! First loop: solve all load steps

! Make sure that you do not leave the solution module at any point

/solu

antype,static,new

*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
*enddo

! Second loop: postproccess the results of all load steps.

! All the results are stored in the same database, as different load
steps

*do,itime,1,itimef
sifcalc.mac !calculate SIF
*enddo

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 16/06/2014 20:40, michele.cerullo escribió:

Dear all,
I would like to calculate the stress intensity factor, according to
LEFM, at a crack tip, during a varying load. For this reason I divided
the load in "itimef" values and I created a loop in a macro that may
look like

Code:
input.mac !define input parameters
geom.mac !create geometry
mesh.mac !mesh geometry
bc.mac !apply Boundary conditions
*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
sifcalc.mac !calculate SIF
*enddo

At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like
to save all the
solutions, for each time steps. If I save at the end of every loop
though, it overwrites the results from previous computations. Moreover I
would like to avoid to save different jobnames for each time step. I
tried with load cases but I cannot manage it to work. Does anybody have
some suggestions please?

Best,
Michele

Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html [1]
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
[4] http://www.xansys.org/rules.html
+-------------------------------------------------------------+
| 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
michele.cerullo
User


Joined: 04 Jun 2014
Posts: 4
Location: Copenhagen

PostPosted: Tue Jun 17, 2014 3:36 am  Reply with quote

You are right Jose, I just checked the netiquette, that for some reason I could not find. Thanks for noticing. I Also should have put [APDL] in the subject beside my signature.

jose.galan wrote:
By the way, you should follow xansys netiquette and include your full
affiliation in all your posts (http://www.xansys.org/rules.html [4]).
There are consequences for not complying with the rules.

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 17/06/2014 02:09, mfernan@us.es escribió:

Quote:
Dear Mr. Cerullo,
if you are performing a linear static analysis (antype,static), you can
define multiple load steps that will be stored in the same ansys
database by default (outres,all,all). Ansys provides several methods to
define and solve multiple load steps. I reccommend you to read the ansys
manual for more details:

Basic Guide > Chapter 3. Solution > 3.7. Solving Multiple Load Steps

The simplest method is the multiple SOLVE method. "It involves issuing
the SOLVE [1] command after each load step is defined. The main
disadvantage, for interactive use, is that you have to wait for the
solution to be completed before defining the next load step. A typical
command stream for the multiple SOLVE [1]method is shown below:

/SOLU
...
! Load step 1:
D,...
SF,...
SOLVE ! Solution for load step 1
! Load step 2
F,...
SF,...
...
SOLVE ! Solution for load step 2
Etc.

". The text and example are taken from the manual.

However, if you leave the solution module (with the command finish or
entering other module) and then reenter (/solu), when you issue a solve
command you will start over with load step 1, losing all the previously
calculated results. This looks like what it is happening to you.

At some point in one (or more) of the macros inside your *do loop, you
are leaving the solution module. When you reenter the solution module in
the next iteration, you overwrite the previous results.

You should review your macros in order to avoid leaving the solution
module.

I would reccommend you to divide you loop in two consecutive loops, the
first one to calculate the solutions to all the load steps, and the
second one to postprocess the results to obtain the sif. You have to
make sure that in the first loop the macros do not leave the solution
module at any point.

! First loop: solve all load steps

! Make sure that you do not leave the solution module at any point

/solu

antype,static,new

*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
*enddo

! Second loop: postproccess the results of all load steps.

! All the results are stored in the same database, as different load
steps

*do,itime,1,itimef
sifcalc.mac !calculate SIF
*enddo

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 16/06/2014 20:40, michele.cerullo escribió:

Dear all,
I would like to calculate the stress intensity factor, according to
LEFM, at a crack tip, during a varying load. For this reason I divided
the load in "itimef" values and I created a loop in a macro that may
look like

Code:
input.mac !define input parameters
geom.mac !create geometry
mesh.mac !mesh geometry
bc.mac !apply Boundary conditions
*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
sifcalc.mac !calculate SIF
*enddo

At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like
to save all the
solutions, for each time steps. If I save at the end of every loop
though, it overwrites the results from previous computations. Moreover I
would like to avoid to save different jobnames for each time step. I
tried with load cases but I cannot manage it to work. Does anybody have
some suggestions please?

Best,
Michele

Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html [1]
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
[4] http://www.xansys.org/rules.html
+-------------------------------------------------------------+
| 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
michele.cerullo
User


Joined: 04 Jun 2014
Posts: 4
Location: Copenhagen

PostPosted: Tue Jun 17, 2014 3:42 am  Reply with quote

Dear Jose,
thanks a lot for your suggestions: the problem was in the fact that everytime I exit the module from /SOL to /POST1 it erased the load step. I followed your suggestions to break the loop and it works just perfect: thanks again.
Do you think that may work even if I make a nonlinear analysis, introducing for example contact elements?




jose.galan wrote:
Dear Mr. Cerullo,
if you are performing a linear static analysis (antype,static), you can
define multiple load steps that will be stored in the same ansys
database by default (outres,all,all). Ansys provides several methods to
define and solve multiple load steps. I reccommend you to read the ansys
manual for more details:

Basic Guide > Chapter 3. Solution > 3.7. Solving Multiple Load Steps

The simplest method is the multiple SOLVE method. "It involves issuing
the SOLVE [1] command after each load step is defined. The main
disadvantage, for interactive use, is that you have to wait for the
solution to be completed before defining the next load step. A typical
command stream for the multiple SOLVE [1]method is shown below:

/SOLU
...
! Load step 1:
D,...
SF,...
SOLVE ! Solution for load step 1
! Load step 2
F,...
SF,...
...
SOLVE ! Solution for load step 2
Etc.

". The text and example are taken from the manual.

However, if you leave the solution module (with the command finish or
entering other module) and then reenter (/solu), when you issue a solve
command you will start over with load step 1, losing all the previously
calculated results. This looks like what it is happening to you.

At some point in one (or more) of the macros inside your *do loop, you
are leaving the solution module. When you reenter the solution module in
the next iteration, you overwrite the previous results.

You should review your macros in order to avoid leaving the solution
module.

I would reccommend you to divide you loop in two consecutive loops, the
first one to calculate the solutions to all the load steps, and the
second one to postprocess the results to obtain the sif. You have to
make sure that in the first loop the macros do not leave the solution
module at any point.

! First loop: solve all load steps

! Make sure that you do not leave the solution module at any point

/solu

antype,static,new

*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
*enddo

! Second loop: postproccess the results of all load steps.

! All the results are stored in the same database, as different load
steps

*do,itime,1,itimef
sifcalc.mac !calculate SIF
*enddo

Best regards,

Jose M. Galan

Asst. Prof.

Engin. Const. Dept.

Univ. Sevilla

Spain

El 16/06/2014 20:40, michele.cerullo escribió:

Dear all,
I would like to calculate the stress intensity factor, according to
LEFM, at a crack tip, during a varying load. For this reason I divided
the load in "itimef" values and I created a loop in a macro that may
look like

Code:
input.mac !define input parameters
geom.mac !create geometry
mesh.mac !mesh geometry
bc.mac !apply Boundary conditions
*do,itime,1,itimef
load.mac !apply load(itime)
sol.mac !solve
sifcalc.mac !calculate SIF
*enddo

At the end of every loop I erase the load so that it does not add up.
My problem is that I am making a static linear analysis and I would like
to save all the
solutions, for each time steps. If I save at the end of every loop
though, it overwrites the results from previous computations. Moreover I
would like to avoid to save different jobnames for each time step. I
tried with load cases but I cannot manage it to work. Does anybody have
some suggestions please?

Best,
Michele

Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html
+-------------------------------------------------------------+
| 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)

_________________
Best regards,

Michele Cerullo
PhD student
DTU, Kgs. Lyngby
Denmark
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jun 17, 2014 4:20 am  Reply with quote

Dear Mr. Cerullo,

You forgot your signature again.

"Anonymous posts are not welcome on the XANSYS list. Read the Rules page
at www.xansys.org [1] and include a complete signature on all posts. If
you are using the forum interface I recommend editing your profile to
include an automatic signature. " [message taken from the xansys
moderators]

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 12:36, michele.cerullo escribió:

Quote:
You are right Jose, I just checked the netiquette, that for some reason I could not find. Thanks for noticing. I Also should have put [APDL] in the subject beside my signature.


Links:
------
[1] http://www.xansys.org/
+-------------------------------------------------------------+
| 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: Tue Jun 17, 2014 4:33 am  Reply with quote

Dear Mr. Cerullo:

the multiple load step method is valid in both linear and nonlinear
analysis.

With nonlinear problems, you will have to take into account that your
solution may not converge at some load step. In such cases you may need
to restart the analysis. Please, review the procedures for restarting an
analysis in the ansys manual

Basic Guide | Chapter 3. Solution | 3.9. Restarting an Analysis

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

PS: now you have a proper signature. You are ready for xansys.

El 17/06/2014 12:42, michele.cerullo escribió:

Quote:
Dear Jose,
thanks a lot for your suggestions: the problem was in the fact that everytime I exit the module from /SOL to /POST1 it erased the load step. I followed your suggestions to break the loop and it works just perfect: thanks again.
Do you think that may work even if I make a nonlinear analysis, introducing for example contact elements?

jose.galan wrote:

Quote:
Dear Mr. Cerullo, if you are performing a linear static analysis (antype,static), you can define multiple load steps that will be stored in the same ansys database by default (outres,all,all). Ansys provides several methods to define and solve multiple load steps. I reccommend you to read the ansys manual for more details: Basic Guide > Chapter 3. Solution > 3.7. Solving Multiple Load Steps The simplest method is the multiple SOLVE method. "It involves issuing the SOLVE [1] command after each load step is defined. The main disadvantage, for interactive use, is that you have to wait for the solution to be completed before defining the next load step. A typical command stream for the multiple SOLVE [1]method is shown below: /SOLU ... ! Load step 1: D,... SF,... SOLVE ! Solution for load step 1 ! Load step 2 F,... SF,... ... SOLVE ! Solution for load step 2 Etc. ". The text and example are taken from the manual. However, if you leave the solution module (with the command finish or
entering other module) and then reenter (/solu), when you issue a solve command you will start over with load step 1, losing all the previously calculated results. This looks like what it is happening to you. At some point in one (or more) of the macros inside your *do loop, you are leaving the solution module. When you reenter the solution module in the next iteration, you overwrite the previous results. You should review your macros in order to avoid leaving the solution module. I would reccommend you to divide you loop in two consecutive loops, the first one to calculate the solutions to all the load steps, and the second one to postprocess the results to obtain the sif. You have to make sure that in the first loop the macros do not leave the solution module at any point. ! First loop: solve all load steps ! Make sure that you do not leave the solution module at any point /solu antype,static,new *do,itime,1,itimef load.mac !apply load(itime) sol.mac !solve *enddo ! Second loop:
postproccess the results of all load steps. ! All the results are stored in the same database, as different load steps *do,itime,1,itimef sifcalc.mac !calculate SIF *enddo Best regards, Jose M. Galan Asst. Prof. Engin. Const. Dept. Univ. Sevilla Spain El 16/06/2014 20:40, michele.cerullo escribió: Dear all, I would like to calculate the stress intensity factor, according to LEFM, at a crack tip, during a varying load. For this reason I divided the load in "itimef" values and I created a loop in a macro that may look like Code: input.mac !define input parameters geom.mac !create geometry mesh.mac !mesh geometry bc.mac !apply Boundary conditions *do,itime,1,itimef load.mac !apply load(itime) sol.mac !solve sifcalc.mac !calculate SIF *enddo At the end of every loop I erase the load so that it does not add up. My problem is that I am making a static linear analysis and I would like to save all the solutions, for each time steps. If I save at the end of every loop though, it overwrites
the results from previous computations. Moreover I would like to avoid to save different jobnames for each time step. I tried with load cases but I cannot manage it to work. Does anybody have some suggestions please? Best, Michele Links: ------ [1] http://buzonweb.us.es/Hlp_C_SOLVE.html [1] +-------------------------------------------------------------+ | XANSYS web - www.xansys.org/forum [2] | | The Online Community for users of ANSYS, Inc. Software | | Hosted by PADT - www.padtinc.com [3] | | Send administrative requests to xansys-mod@tynecomp.co.uk | +-------------------------------------------------------------+ Post generated using Mail2Forum (http://www.mail2forum.com [4])
Quote:

------------------------
Best regards,

Michele Cerullo
PhD student
DTU, Kgs. Lyngby
Denmark


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://buzonweb.us.es/Hlp_C_SOLVE.html
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
[4] http://www.mail2forum.com
[5] http://xansys.org/forum/viewtopic.php?p=94517#94517
+-------------------------------------------------------------+
| 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: Tue Jun 17, 2014 5:05 am  Reply with quote

Dear Mr. Cerullo,

I noticed that you had added your signature at the end of your message.
I apologize for the undeserved reprimand. My mistake.

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 13:19, mfernan@us.es escribió:

Quote:
Dear Mr. Cerullo,

You forgot your signature again.

"Anonymous posts are not welcome on the XANSYS list. Read the Rules page
at www.xansys.org [1][1] and include a complete signature on all posts. If
you are using the forum interface I recommend editing your profile to
include an automatic signature. " [message taken from the xansys
moderators]

Best regards,

El 17/06/2014 12:36, michele.cerullo escribió:

Quote:
You are right Jose, I just checked the netiquette, that for some reason I could not find. Thanks for noticing. I Also should have put [APDL] in the subject beside my signature.

Links:
------
[1] http://www.xansys.org/ [2]
+-------------------------------------------------------------+
| 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.xansys.org
[2] http://www.xansys.org/
[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
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