Author 
Message 
sushant.goel User
Joined: 08 May 2014 Posts: 66

Posted: Thu Sep 11, 2014 1:32 am 


Hello everyone,
I am doing eigenvalue buckling analysis for a 10mm thick spherical glass dome with 10 meter span and 2 meter rise. In section 17.5.1, Ansys recommends to keep PSTRES on for eigenvalue buckling analysis. This option allows calculation of stress stiffness matrix. I ran my model with PSTRES on and off. And I am getting exactly same buckling factors for both cases (see attached images). The dome is only loaded by selfweight. There are many tutorials available on internet which say PSTRES should be on. But why do get same results even with PSTRES off?
https://www.dropbox.com/sh/1yj9321u3n0plq9/AACrZNniGHTD8aoM2puagPiZa?dl=0
Second part of my question is regarding the high value of buckling factors. First buckling factor is 277. It means the structure will buckle at 277 x dead weight. I know that this is linear buckling analysis and imperfections (reality) are not taken into account. But still isn't this value very high and unrealistic? _________________ Best regards,
Sushant Goel
MSc Uni Stuttgart 

Back to top 


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

Posted: Thu Sep 11, 2014 3:32 am 


Dear Mr. Goel:
in the documentation the mention what you say in your email: that
pstres,on is required in the static analysis. With this command the user
asked Ansys to calculate and store the tangential stiffness matrix,
which is used for linear buckling analysis or prestressed modal
analysis. That was the usual way in older ansys versions.
After a certain version (whose numberI don't recall), Ansys introduced
linear perturbation analysis to do those same calculations. If you check
the procedure for linear perturbation analysis (see Ansys Documentation
Quote:  Mechanical APDL > 15.8.5. Eigenvalue Buckling Analysis Based on Linear Perturbation), you will notice that ansys does not require using the command PSTRES. In fact, the tangential stiffness matrix Kt is calculated when the command PERTURB,BUCKLE is issued. Since this command is equivalent to ANTYPE,BUCKLE, I guess that both commands do the same thing (i.e. calculate Kt ), even when PSTRES,ON was not issued on the static solve.

Regarding the buckling factor, if your sphere has a uniform thickness
and a single material, you could compare your numerical results with the
analytical expression for the theoretical buckling pressure of the
perfect shell under external pressure:
pcr=E* (t/R)^2 * 2/sqrt(3*(1nu^2))
As you point out, this is the theoretical buckling pressure. The actual
buckling pressure will be much lower.
I reccommend you to read the following document by D. Bushnell about
imperfection sensitivity of shells.
http://shellbuckling.com/papers/imperfsensitivity.pdf
The imperfection sensitivity of a spherical dome depends on its
shallowness (see pages 5 and 6 of the pdf document, and the definition
of shallowness parameter).
In your case, shallowness parameter is
lambda=2* (3*(10.2^2))^0.2 * sqrt(2 m/0.01 m) = 36.8 > 20
Therefore, your shell is extremely sensitive to initial imperfections
(see slide 47, figure (f))
For steel shells, DIN18800 gives a procedure to calculate a design
pressure, taking into account the quality of construction of the shell
(which is related to the maximum amplitude of imperfections that are
allowed).
For a concrete dome, you can use ACI 34906 to obtain the knockdown
reductions factors due to large deflections, cereep effects,
temperature, cracking and deviations between the actual and theoretical
shell geometry.
http://www.wmsym.org/archives/2012/papers/12278.pdf
For glass domes, you will have to look on the literature for reduction
factors. I do not know if there is a DIN standard for glass shells yet.
I am sure that your advisor will have information on the topic.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Universidad de Sevilla
Spain
El 11/09/2014 10:32, sushant.goel escribió:
Quote:  Hello everyone,
I am doing eigenvalue buckling analysis for a 10mm thick spherical glass dome with 10 meter span and 2 meter rise. In section 17.5.1, Ansys recommends to keep PSTRES on for eigenvalue buckling analysis. This option allows calculation of stress stiffness matrix. I ran my model with PSTRES on and off. And I am getting exactly same buckling factors for both cases (see attached images). The dome is only loaded by selfweight. There are many tutorials available on internet which say PSTRES should be on. But why do get same results even with PSTRES off?
https://www.dropbox.com/sh/1yj9321u3n0plq9/AACrZNniGHTD8aoM2puagPiZa?dl=0 [1]
Second part of my question is regarding the high value of buckling factors. First buckling factor is 277. It means the structure will buckle at 277 x dead weight. I know that this is linear buckling analysis and imperfections (reality) are not taken into account. But still isn't this value very high and unrealistic?

Best regards,
Sushant Goel
MSc Uni Stuttgart
++
 XANSYS web  www.xansys.org/forum [4] 
 The Online Community for users of ANSYS, Inc. Software 
 Hosted by PADT  www.padtinc.com [5] 
 Send administrative requests to xansysmod@tynecomp.co.uk 
++

Links:

[1]
https://www.dropbox.com/sh/1yj9321u3n0plq9/AACrZNniGHTD8aoM2puagPiZa?dl=0
[2] http://www.mail2forum.com
[3] http://xansys.org/forum/viewtopic.php?p=95430#95430
[4] http://www.xansys.org/forum
[5] 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 


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

Posted: Thu Sep 11, 2014 3:46 am 


Dear Mr. Goel:
doing a google search on "buckling load glass dome" you may finnd some
interesting references.
For example, Jaap Aanhaanen's MS thesis, "The stability of a glass
facetted shell structure", from Delft University of Technology seems
relevant and includes a chapter on imperfection sensitivity.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Universidad de Sevilla
Spain
El 11/09/2014 12:32, mfernan@us.es escribió:
Quote:  Dear Mr. Goel:
in the documentation the mention what you say in your email: that
pstres,on is required in the static analysis. With this command the user
asked Ansys to calculate and store the tangential stiffness matrix,
which is used for linear buckling analysis or prestressed modal
analysis. That was the usual way in older ansys versions.
After a certain version (whose numberI don't recall), Ansys introduced
linear perturbation analysis to do those same calculations. If you check
the procedure for linear perturbation analysis (see Ansys Documentation
Quote:  Mechanical APDL > 15.8.5. Eigenvalue Buckling Analysis Based on Linear Perturbation), you will notice that ansys does not require using the command PSTRES. In fact, the tangential stiffness matrix Kt is calculated when the command PERTURB,BUCKLE is issued. Since this command is equivalent to ANTYPE,BUCKLE, I guess that both commands do the same thing (i.e. calculate Kt ), even when PSTRES,ON was not issued on the static solve.

Regarding the buckling factor, if your sphere has a uniform thickness
and a single material, you could compare your numerical results with the
analytical expression for the theoretical buckling pressure of the
perfect shell under external pressure:
pcr=E* (t/R)^2 * 2/sqrt(3*(1nu^2))
As you point out, this is the theoretical buckling pressure. The actual
buckling pressure will be much lower.
I reccommend you to read the following document by D. Bushnell about
imperfection sensitivity of shells.
http://shellbuckling.com/papers/imperfsensitivity.pdf [6]
The imperfection sensitivity of a spherical dome depends on its
shallowness (see pages 5 and 6 of the pdf document, and the definition
of shallowness parameter).
In your case, shallowness parameter is
lambda=2* (3*(10.2^2))^0.2 * sqrt(2 m/0.01 m) = 36.8 > 20
Therefore, your shell is extremely sensitive to initial imperfections
(see slide 47, figure (f))
For steel shells, DIN18800 gives a procedure to calculate a design
pressure, taking into account the quality of construction of the shell
(which is related to the maximum amplitude of imperfections that are
allowed).
For a concrete dome, you can use ACI 34906 to obtain the knockdown
reductions factors due to large deflections, cereep effects,
temperature, cracking and deviations between the actual and theoretical
shell geometry.
http://www.wmsym.org/archives/2012/papers/12278.pdf [7]
For glass domes, you will have to look on the literature for reduction
factors. I do not know if there is a DIN standard for glass shells yet.
I am sure that your advisor will have information on the topic.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Universidad de Sevilla
Spain
El 11/09/2014 10:32, sushant.goel escribió:
Quote:  Hello everyone, I am doing eigenvalue buckling analysis for a 10mm thick spherical glass dome with 10 meter span and 2 meter rise. In section 17.5.1, Ansys recommends to keep PSTRES on for eigenvalue buckling analysis. This option allows calculation of stress stiffness matrix. I ran my model with PSTRES on and off. And I am getting exactly same buckling factors for both cases (see attached images). The dome is only loaded by selfweight. There are many tutorials available on internet which say PSTRES should be on. But why do get same results even with PSTRES off? https://www.dropbox.com/sh/1yj9321u3n0plq9/AACrZNniGHTD8aoM2puagPiZa?dl=0 [1] [1 [1]] Second part of my question is regarding the high value of buckling factors. First buckling factor is 277. It means the structure will buckle at 277 x dead weight. I know that this is linear buckling analysis and imperfections (reality) are not taken into account. But still isn't this value very high and unrealistic?

  Best regards, Sushant Goel MSc Uni Stuttgart  m2f  Sent using Mail2Forum (http://www.mail2forum.com [2] [2 [2]]). Read this topic online here: http://xansys.org/forum/viewtopic.php?p=95430#95430 [3] [3 [3]]  m2f  ++  XANSYS web  www.xansys.org/forum [4] [4 [4]]   The Online Community for users of ANSYS, Inc. Software   Hosted by PADT  www.padtinc.com [5] [5 [5]]   Send administrative requests to xansysmod@tynecomp.co.uk  ++
Links:

[1]
https://www.dropbox.com/sh/1yj9321u3n0plq9/AACrZNniGHTD8aoM2puagPiZa?dl=0
[2] http://www.mail2forum.com
[3] http://xansys.org/forum/viewtopic.php?p=95430#95430
[4] http://www.xansys.org/forum
[5] http://www.padtinc.com
[6] http://shellbuckling.com/papers/imperfsensitivity.pdf
[7] http://www.wmsym.org/archives/2012/papers/12278.pdf
++
 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 


sushant.goel User
Joined: 08 May 2014 Posts: 66

Posted: Thu Sep 11, 2014 4:52 am 


Quote:  Dear Mr. Goel:
doing a google search on "buckling load glass dome" you may finnd some
interesting references.
For example, Jaap Aanhaanen's MS thesis, "The stability of a glass
facetted shell structure", from Delft University of Technology seems
relevant and includes a chapter on imperfection sensitivity. 
Quote:  Dear Mr. Goel:
in the documentation the mention what you say in your email: that
pstres,on is required in the static analysis. With this command the user
asked Ansys to calculate and store the tangential stiffness matrix,
which is used for linear buckling analysis or prestressed modal
analysis. That was the usual way in older ansys versions.
After a certain version (whose numberI don't recall), Ansys introduced
linear perturbation analysis to do those same calculations. If you check
the procedure for linear perturbation analysis (see Ansys Documentation
Quote:
Mechanical APDL > 15.8.5. Eigenvalue Buckling Analysis Based on Linear Perturbation), you will notice that ansys does not require using the command PSTRES. In fact, the tangential stiffness matrix Kt is calculated when the command PERTURB,BUCKLE is issued. Since this command is equivalent to ANTYPE,BUCKLE, I guess that both commands do the same thing (i.e. calculate Kt ), even when PSTRES,ON was not issued on the static solve.
Regarding the buckling factor, if your sphere has a uniform thickness
and a single material, you could compare your numerical results with the
analytical expression for the theoretical buckling pressure of the
perfect shell under external pressure:
pcr=E* (t/R)^2 * 2/sqrt(3*(1nu^2))
As you point out, this is the theoretical buckling pressure. The actual
buckling pressure will be much lower.
I reccommend you to read the following document by D. Bushnell about
imperfection sensitivity of shells.
http://shellbuckling.com/papers/imperfsensitivity.pdf
The imperfection sensitivity of a spherical dome depends on its
shallowness (see pages 5 and 6 of the pdf document, and the definition
of shallowness parameter).
In your case, shallowness parameter is
lambda=2* (3*(10.2^2))^0.2 * sqrt(2 m/0.01 m) = 36.8 > 20
Therefore, your shell is extremely sensitive to initial imperfections
(see slide 47, figure (f))
For steel shells, DIN18800 gives a procedure to calculate a design
pressure, taking into account the quality of construction of the shell
(which is related to the maximum amplitude of imperfections that are
allowed).
For a concrete dome, you can use ACI 34906 to obtain the knockdown
reductions factors due to large deflections, cereep effects,
temperature, cracking and deviations between the actual and theoretical
shell geometry.
http://www.wmsym.org/archives/2012/papers/12278.pdf
For glass domes, you will have to look on the literature for reduction
factors. I do not know if there is a DIN standard for glass shells yet.
I am sure that your advisor will have information on the topic.
Best regards,
Jose M. Galan
Constr. Engin. Dept.
Universidad de Sevilla
Spain
El 11/09/2014 10:32, sushant.goel escribió:

Dear Mr Galan,
Thank you very much once again for your detailed replies. I have already gone through the Master thesis of Jaap Aanhaanen as its very relevant to my thesis topic. I will look into the imperfection sensitivity chapter once again.
Thank you for sharing information on linear pertubation analysis. The tutorials which I am following are mostly for older Ansys versions and none of them mentions about PERTURB.
Quote:  pcr=E* (t/R)^2 * 2/sqrt(3*(1nu^2)) 
This formula comes from solving this differential equation;[CIE4143 Shell Analysis, Theory and Application,TU Delft]
https://www.dropbox.com/s/4oam7w7au16a574/4143.PNG?dl=0
I did the calculation using the above formula. The buckling factor is 630 according to this formula and Ansys gives 614 as first buckling factor (Dome support condition all translations and rotations fixed). So, it means this formula is applicable only for fully fixed support conditions. Am I correct?
Also, I tried the optimum support system for dome (tangential to shell surface) and first bucking factor was around 277 in Ansys (do you know the analytical expression for this?).
And another inference from these results is that although tangential support system helps to keep the dome in membrane state and avoid bending, the buckling factor for such a support system is almost half (277) when compared to fully fixed support system (614). Is this result analogous to the four basic Euler buckling configurations?
https://www.dropbox.com/s/wygfbn9aq5xs0vs/buck.PNG?dl=0 _________________ Best regards,
Sushant Goel
MSc Uni Stuttgart 

Back to top 


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

Posted: Thu Sep 11, 2014 5:48 am 


Dear Mr. Goel:
indeed, the buckling load depends on the support conditions. The
expression I sent you was the ideal buckling pressure for a full sphere
under uniform external pressure. You can find the complete expressions
for other support conditions in a textbook on shell buckling. Also, in
Section 7.2 of DIN 188004, which contains the expression for the ideal
buckling buckling stresses of spherical shells of uniform wall
thicknesses:
sigma_x_cr=Ck*E* (t/R) * 1/sqrt(3*(1nu^2))
with Ck depending on the support conditions (RB1 to RB5), going from 1
to 0.2. Your boundary conditions are RB4, for which Ck=0.4 (for
halfsubtended angles <=135º), which is very similar to the numerical
values that you have obtained, 277/613=0.45. Your conclusion is correct:
when the support conditions are defined to avoid the local shell bending
stresses at the supports, the buckling stress goes down.
The factors Ck are not the quantitatively the same as those for the
classical Euler beam buckling problem, but the effect of edge constrains
on buckling load is similar (qualitatively, more constrains lead to
higher buckling loads). For a compressed bar, the buckling load depends
on its effective buckling length, Lk=beta*L, with L being the physical
length and beta a coefficient which depends on many parameters (edge
restrains, distribution of axial compression along the bar, etc); the
classical values of beta for a vertical columns under uniform
compression are well known(1 for pinnedpinned support, 2 for
fixedfree, 0.5 for fixedfixed, and 0.7 for fixedpinned). On the other
hand, the buckling load of a "long" shell does not depend on the shell
length, as you can see on the expression for sigma_x_cr. It only depends
on the ratio (t/R).
If you want some additional information, you should find some textbook
on shell buckling.
Best regards,
Jose M. Galan
Constr. Eng. Dept.
Universidad de Sevilla
Spain
Quote:  Dear Mr Galan,
Thank you very much once again for your detailed replies. I have already gone through the Master thesis of Jaap Aanhaanen as its very relevant to my thesis topic. I will look into the imperfection sensitivity chapter once again.
Thank you for sharing information on linear pertubation analysis. The tutorials which I am following are mostly for older Ansys versions and none of them mentions about PERTURB.
Quote:  pcr=E* (t/R)^2 * 2/sqrt(3*(1nu^2))

This formula comes from solving this differential equation;[CIE4143 Shell Analysis, Theory and Application,TU Delft]
https://www.dropbox.com/s/4oam7w7au16a574/4143.PNG?dl=0 [1]
I did the calculation using the above formula. The buckling factor is 630 according to this formula and Ansys gives 614 as first buckling factor (Dome support condition all translations and rotations fixed). So, it means this formula is applicable only for fully fixed support conditions. Am I correct?
Also, I tried the optimum support system for dome (tangential to shell surface) and first bucking factor was around 277 in Ansys (do you know the analytical expression for this?).
And another inference from these results is that although tangential support system helps to keep the dome in membrane state and avoid bending, the buckling factor for such a support system is almost half (277) when compared to fully fixed support system (614). Is this result analogous to the four basic Euler buckling configurations?
https://www.dropbox.com/s/wygfbn9aq5xs0vs/buck.PNG?dl=0 [2]

Best regards,
Sushant Goel
MSc Uni Stuttgart

Links:

[1] https://www.dropbox.com/s/4oam7w7au16a574/4143.PNG?dl=0
[2] https://www.dropbox.com/s/wygfbn9aq5xs0vs/buck.PNG?dl=0
++
 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 


sushant.goel User
Joined: 08 May 2014 Posts: 66

Posted: Thu Sep 11, 2014 6:56 am 


Quote:  Dear Mr. Goel:
indeed, the buckling load depends on the support conditions. The
expression I sent you was the ideal buckling pressure for a full sphere
under uniform external pressure. You can find the complete expressions
for other support conditions in a textbook on shell buckling. Also, in
Section 7.2 of DIN 188004, which contains the expression for the ideal
buckling buckling stresses of spherical shells of uniform wall
thicknesses:
sigma_x_cr=Ck*E* (t/R) * 1/sqrt(3*(1nu^2))
with Ck depending on the support conditions (RB1 to RB5), going from 1
to 0.2. Your boundary conditions are RB4, for which Ck=0.4 (for
halfsubtended angles <=135º), which is very similar to the numerical
values that you have obtained, 277/613=0.45. Your conclusion is correct:
when the support conditions are defined to avoid the local shell bending
stresses at the supports, the buckling stress goes down.
The factors Ck are not the quantitatively the same as those for the
classical Euler beam buckling problem, but the effect of edge constrains
on buckling load is similar (qualitatively, more constrains lead to
higher buckling loads). For a compressed bar, the buckling load depends
on its effective buckling length, Lk=beta*L, with L being the physical
length and beta a coefficient which depends on many parameters (edge
restrains, distribution of axial compression along the bar, etc); the
classical values of beta for a vertical columns under uniform
compression are well known(1 for pinnedpinned support, 2 for
fixedfree, 0.5 for fixedfixed, and 0.7 for fixedpinned). On the other
hand, the buckling load of a "long" shell does not depend on the shell
length, as you can see on the expression for sigma_x_cr. It only depends
on the ratio (t/R).
If you want some additional information, you should find some textbook
on shell buckling.
Best regards,
Jose M. Galan
Constr. Eng. Dept.
Universidad de Sevilla
Spain 
Dear Mr Galan,
Thank you very much for all the responses. :D _________________ Best regards,
Sushant Goel
MSc Uni Stuttgart 

Back to top 


christopher.wright User
Joined: 17 Jun 2009 Posts: 927

Posted: Thu Sep 11, 2014 1:17 pm 


On Sep 11, 2014, at 3:32 AM, sushant.goel wrote:
Quote:  I know that this is linear buckling analysis and imperfections
(reality) are not taken into account. But still isn't this value
very high and unrealistic?

What value does the theoretical buckling analysis give you? The
theoretical (large displacement) buckling analysis should be pretty
close to the experimental value. That'll give you a basis for knowing
if you've done the ANSYS analysis correctly.
You do yourself no favors by launching into an ANSYS analysis before
doing some simple estimates. As you've discovered, doing the ANSYS
calculation first gives you no basis to know if you've screwed up the
FEA model or the loading application. You end up like the Sorcerer's
apprentice: Your teacher gives you a job but you get lazy and figure
you'll create a device to do your work for you. Your device turns
into a monster and and you end up with a kick in the ass from your
teacher and cleaning up the mess anyway.
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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sushant.goel User
Joined: 08 May 2014 Posts: 66

Posted: Tue Sep 16, 2014 8:40 pm 


Quote:  What value does the theoretical buckling analysis give you? The
theoretical (large displacement) buckling analysis should be pretty
close to the experimental value. That'll give you a basis for knowing
if you've done the ANSYS analysis correctly.
You do yourself no favors by launching into an ANSYS analysis before
doing some simple estimates. As you've discovered, doing the ANSYS
calculation first gives you no basis to know if you've screwed up the
FEA model or the loading application. You end up like the Sorcerer's
apprentice: Your teacher gives you a job but you get lazy and figure
you'll create a device to do your work for you. Your device turns
into a monster and and you end up with a kick in the ass from your
teacher and cleaning up the mess anyway.

Dear Mr Wright,
Ansys gives first buckling factor = 277.
Theoretical value = 252 (using 'sigma_x_cr=Ck*E* (t/R) * 1/sqrt(3*(1nu^2))' with Ck =0.4) [stated by Mr Galan]
I will try to keep my future queries restricted to Ansys and find answers for theoretical formulas/explanations myself. _________________ Best regards,
Sushant Goel
MSc Uni Stuttgart 

Back to top 


christopher.wright User
Joined: 17 Jun 2009 Posts: 927

Posted: Tue Sep 16, 2014 10:28 pm 


On Sep 16, 2014, at 10:40 PM, sushant.goel wrote:
Quote:  I will try to keep my future queries restricted to Ansys and find
answers for theoretical formulas/explanations myself.
 What you choose to keep to yourself is only of concern where it sheds
light on answers to your questions. In this case you should have
sniffed around for a theoretical large displacement analysis to act
as a check on your ANSYS work. As every OFB subscriber has said at
one time or another, ANSYS doesn't think for youit does what you
tell it even if you tell it something outrageous (like those brooms
in the Sorceror's Apprentice). The first step when you suspect an
incorrect analysis, is to make an approximate figure to estimate
about what the answer should be. In this case the error isn't so big,
so you were probably on the right track.
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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


sushant.goel User
Joined: 08 May 2014 Posts: 66

Posted: Wed Sep 17, 2014 5:46 pm 


Quote:  In this case you should have
sniffed around for a theoretical large displacement analysis to act
as a check on your ANSYS work. 
Agreed Mr Wright. I am relying too much on Anys without proper results verification. Thank you for stressing on this point. I'll do the verification of all my FE models with theoretical formulas. _________________ Best regards,
Sushant Goel
MSc Uni Stuttgart 

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

