Author 
Message 
michele.cerullo User
Joined: 04 Jun 2014 Posts: 4 Location: Copenhagen

Posted: Mon Jun 16, 2014 11:40 am 


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 


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

Posted: Mon Jun 16, 2014 11:44 am 


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 15132432366
Original Message
From: Xansys [mailto:xansysbounces@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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) _________________ Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Mon Jun 16, 2014 5:09 pm 


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 escribiÃ³:
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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Mon Jun 16, 2014 5:21 pm 


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 escribiÃ³:
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 escribiÃ³:
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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


michele.cerullo User
Joined: 04 Jun 2014 Posts: 4 Location: Copenhagen

Posted: Tue Jun 17, 2014 3:36 am 


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 escribiÃ³:
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 escribiÃ³:
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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 


Back to top 


michele.cerullo User
Joined: 04 Jun 2014 Posts: 4 Location: Copenhagen

Posted: Tue Jun 17, 2014 3:42 am 


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 escribiÃ³:
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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 
_________________ Best regards,
Michele Cerullo
PhD student
DTU, Kgs. Lyngby
Denmark 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Tue Jun 17, 2014 4:20 am 


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 escribiÃ³:
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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Tue Jun 17, 2014 4:33 am 


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 escribiÃ³:
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 escribiÃ³: 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 xansysmod@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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Tue Jun 17, 2014 5:05 am 


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 escribiÃ³:
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 escribiÃ³:
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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 




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

