XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Prestressed Cable Stayed Column Buckling 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
jack.callaghan
User


Joined: 02 Dec 2014
Posts: 4
Location: Newcastle Upon Tyne, UK

PostPosted: Thu Dec 04, 2014 4:21 pm  Reply with quote

Hi All,

I am attempting to recreate an analysis in a research journal of a prestressed cable stayed column. It uses PIPE20 elements for the main column and crossarms and LINK10 elements for the cable stays. I know that these are outdated elements, but I want to make an exact recreation.

The problem is arising in the prestress of the stays. When performing eigenvalue buckling analysis, changing the initial strain in the real constraint for the LINK10 elements seems to have no effect, and I get the same buckling load every time.

Does anyone have any experience with this kind of problem?

The APDL code I am using is as follows:

FINISH
/CLEAR
/TITLE, STAYED COLUMN

!---PREPROCESSING---
/PREP7

!---SET CONSTANTS---
*SET, CRO, 89.3
*SET, CRT, 3.2
*SET, ARO, 42.6
*SET, ART, 3
*SET, SR, 6.35/2
*SET, SA, PI*(SR**2)
*SET, I, 8

!---SET SINUSOIDAL IMPERFECTIONS ALONG COLUMN LENGTH---
*AFUN,DEG
*SET, XA, SI*SIN(1/6*90)
*SET, XB, SI*SIN(2/6*90)
*SET, XC, SI*SIN(3/6*90)
*SET, XD, SI*SIN(4/6*90)
*SET, XE, SI*SIN(5/6*90)

!---DEFINE MATERIALS, ELEMENTS, REAL CONSTRAINTS---
MP, EX, 1, 205E3
MP, EX, 2, 100E3
MP, PRXY, 1, 0.3
MP, PRXY, 2, 0.3
ET, 1, PIPE20
ET, 2, LINK10
KEYPOPT, 2, 3, 0
R, 1, CRO, CRT
R, 2, ARO, ART
R, 3, SA, 1780/100E9

!---PLOT NODES---
N, 1, 0, 0, 0
N, 2, XA, 1000, 0
N, 3, XB, 2000, 0
N, 4, XC, 3000, 0
N, 5, XD, 4000, 0
N, 6, XE, 5000, 0
N, 7, 8, 6000, 0
N, 8, XE, 7000, 0
N, 9, XD, 8000, 0
N, 10, XC, 9000, 0
N, 11, XB, 10000, 0
N, 12, XA, 11000, 0
N, 13, 0, 12000, 0
N, 14, 8, 6000, 300
N, 15, 8, 6000, 600
N, 16, -292, 6000, 0
N, 17, -592, 6000, 0
N, 18, 8, 6000, -300
N, 19, 8, 6000, -600
N, 20, 308, 6000, 0
N, 21, 608, 6000, 0

!---COLUMN ELEMENTS---
MAT, 1
TYPE, 1
REAL, 1
EN, 1, 1, 2
EN, 2, 2, 3
EN, 3, 3, 4
EN, 4, 4, 5
EN, 5, 5, 6
EN, 6, 6, 7
EN, 7, 7, 8
EN, 8, 8, 9
EN, 9, 9, 10
EN, 10, 10, 11
EN, 11, 11, 12
EN, 12, 12, 13

!---CROSSARM ELEMENTS---
MAT, 1
TYPE, 1
REAL, 2
EN, 13, 7, 14
EN, 14, 14, 15
EN, 15, 7, 16
EN, 16, 16, 17
EN, 17, 7, 18
EN, 18, 18, 19
EN, 19, 7, 20
EN, 20, 20, 21

!---STAY ELEMENTS---
MAT, 2
TYPE, 2
REAL, 3
EN, 21, 1, 15
EN, 22, 1, 17
EN, 23, 1, 19
EN, 24, 1, 21
EN, 25, 13, 15
EN, 26, 13, 17
EN, 27, 13, 19
EN, 28, 13, 21

FINISH

!---STATIC ANALYSIS---
/SOLU
ANTYPE,STATIC
PSTRES,ON

!---CONSTRAINTS---
D,1,UX
D,1,UZ
D,1,UY
D,1,ROTY
D,13,UX
D,13,UZ
D,13,ROTY

!---FORCE---
F,13,FY,-1

SOLVE
FINISH

!---BUCKLING ANALYSIS---
/SOLU ! Enter the solution mode again to solve buckling
ANTYPE,BUCKLE ! Buckling analysis
BUCOPT,LANB,1 ! Buckling options - subspace, one mode
SOLVE
FINISH

!---EXPANSION PASS---
/SOLU ! Re-enter solution mode to expand info - necessary
EXPASS,ON ! An expantion pass will be performed
MXPAND,1 ! Specifies the number of modes to expand
SOLVE
FINISH

!---POSTPROCESSING---
/POST1 ! Enter post-processor
SET,LIST ! List eigenvalue solution - Time/Freq listing is the
! force required for buckling (in N for this case).
SET,LAST ! Read in data for the desired mode
PLDISP ! Plots the deflected shape


Thanks,

Jack Callaghan
Mechanical Engineering Student
Northumbria University
Back to top
View user's profile Send private message Send e-mail
ernst.hustedt
User


Joined: 22 Oct 2010
Posts: 127

PostPosted: Thu Dec 04, 2014 6:39 pm  Reply with quote

My guess is: Why should it change, as long as the stays don't go slack
and their effect/stiffness changes? If the stays cause axial load in
the column, the working load limit changes accordingly but not the
buckling load for the column.

Ernst Hustedt
AMES Ltd
Chch, NZ

On 5/12/2014 12:21, jack.callaghan wrote:
Quote:
Hi All,

I am attempting to recreate an analysis in a research journal of a prestressed cable stayed column. It uses PIPE20 elements for the main column and crossarms and LINK10 elements for the cable stays. I know that these are outdated elements, but I want to make an exact recreation.

The problem is arising in the prestress of the stays. When performing eigenvalue buckling analysis,

changing the initial strain in the real constraint for the LINK10
elements seems to have no effect, and I get the same buckling load every
time.
Quote:

Does anyone have any experience with this kind of problem?
+-------------------------------------------------------------+
| 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
jack.callaghan
User


Joined: 02 Dec 2014
Posts: 4
Location: Newcastle Upon Tyne, UK

PostPosted: Fri Dec 05, 2014 4:29 am  Reply with quote

An increase in prestress of the stayed cables does increase the buckling load of the column (to a limit), as the stays cause compression in the crossarms which then act as stabilisers.

I'm not sure if my method of applying the prestress is correct.
I am assuming that the initial strain in the element real constraint is axial between the element nodes, and that strain is the prestress/young's modulus (1780/100E9).
Is this right?

Regards,
Jack
_________________
Jack Callaghan
Mechanical Engineering Student
Northumbria University
Back to top
View user's profile Send private message Send e-mail
luciano.engel
User


Joined: 22 Sep 2014
Posts: 4

PostPosted: Fri Dec 05, 2014 6:31 am  Reply with quote

I think ernst got it ritgh... Why should they change since the column stiffness dont change? Try using stays in diferent positions around the column and see if it changes.

Att,
Luciano Engel
Mechanical Engineer
SIGMA P.C.
Florianópolis, Brazil
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Fri Dec 05, 2014 6:53 am  Reply with quote

The bending stiffness of the column does actually change when it is
subjected to axial stresses, when the equilibrium equation is expressed
in the deformed configuration instead of in the undeformed
configuration. In such case, the stiffness matrix has two terms:

K=Ke+Kg

where Ke is the standard elastic stiffness matrix calculated in the
undeformed configuration, which is constant and does not depend on the
loads applied to the structure, and Kg is the geometrical stiffness
matrix, which do depends on the load applied on the structure. You can
read some additional information on chapter 15 of the book "Theory of
matrix structural analysis" by Przemieniecki.

An axial compression will reduce the bending stiffness (until it becomes
zero at the first buckling load -bifurcation load-), and a traction will
increase it. However, this change in stiffness will only be significant
if the axial load is a non-negligible fraction of the first buckling
load.

Perhaps the axial compression introduced on the column by the cable
stays is very small compared with the buckling load of the column.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 05/12/2014 14:31, luciano.engel escribió:

Quote:
I think ernst got it ritgh... Why should they change since the column stiffness dont change? Try using stays in diferent positions around the column and see if it changes.

Att,
Luciano Engel
Mechanical Engineer
SIGMA P.C.
Florianópolis, Brazil

+-------------------------------------------------------------+
| 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: Fri Dec 05, 2014 7:04 am  Reply with quote

Dear Mr. Callaghan,

if you want to know if your initial strain is correctly applied, you
should check the results of the static analysis. Check the values of the
reaction forces, and compare with the values that you think that you
have applied.

I would also like to ask you to check if the units that you have used
are consistent. The young modulus is 100e9 in the initial strain
calculation of the cables, and 1280 the initial stress. However, for the
other materials (1 and 2 in the input file) you used young modulus
values of 205E3 and 100E3, a factor 1e6 smaller. Could it be possible
that you were applying a much smaller (1e6 times smaller) initial strain
than you intended to?

Best regards,

José M. Galan

Constr Eng. Dept.

Univ. Sevilla

Spain

El 05/12/2014 12:29, jack.callaghan escribió:

Quote:
An increase in prestress of the stayed cables does increase the buckling load of the column (to a limit), as the stays cause compression in the crossarms which then act as stabilisers.

I'm not sure if my method of applying the prestress is correct.
I am assuming that the initial strain in the element real constraint is axial between the element nodes, and that strain is the prestress/young's modulus (1780/100E9).
Is this right?

Regards,
Jack

------------------------
Jack Callaghan
Mechanical Engineering Student
Northumbria University


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [3] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [4] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.mail2forum.com
[2] http://xansys.org/forum/viewtopic.php?p=96401#96401
[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
luciano.engel
User


Joined: 22 Sep 2014
Posts: 4

PostPosted: Fri Dec 05, 2014 7:20 am  Reply with quote

I get it, but like you said, in a symmetrical stayed layout that would only be relevant in a case where the prestresses introduce a compression close enought to the buckling load limit.
It's worth trying though! You got me wondering if even then, the geometrical influence would result in a relevant change in the buckling load limit.

Att,
Luciano Engel
Mechanical Engineer
SIGMA P .C.
Florianópolis- Brazil


jose.galan wrote:
The bending stiffness of the column does actually change when it is
subjected to axial stresses, when the equilibrium equation is expressed
in the deformed configuration instead of in the undeformed
configuration. In such case, the stiffness matrix has two terms:

K=Ke+Kg

where Ke is the standard elastic stiffness matrix calculated in the
undeformed configuration, which is constant and does not depend on the
loads applied to the structure, and Kg is the geometrical stiffness
matrix, which do depends on the load applied on the structure. You can
read some additional information on chapter 15 of the book "Theory of
matrix structural analysis" by Przemieniecki.

An axial compression will reduce the bending stiffness (until it becomes
zero at the first buckling load -bifurcation load-), and a traction will
increase it. However, this change in stiffness will only be significant
if the axial load is a non-negligible fraction of the first buckling
load.

Perhaps the axial compression introduced on the column by the cable
stays is very small compared with the buckling load of the column.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 05/12/2014 14:31, luciano.engel escribió:

Quote:
I think ernst got it ritgh... Why should they change since the column stiffness dont change? Try using stays in diferent positions around the column and see if it changes.

Att,
Luciano Engel
Mechanical Engineer
SIGMA P.C.
Florianópolis, Brazil

+-------------------------------------------------------------+
| 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
jack.callaghan
User


Joined: 02 Dec 2014
Posts: 4
Location: Newcastle Upon Tyne, UK

PostPosted: Sun Dec 07, 2014 11:23 am  Reply with quote

I think I have solved the problem, which seems to have been the following code issues:
- Setting the sinusoidal imperfections used "SI*SIN(1/6*90)" changed to "I*SIN(1/6*90)"
- PI was not recognised, changed to 3.1416

With these ammendments I achieved good results; with no inital strain the buckling load is 34.75 kN, with initail strain of 1780/100E9 the buckling load is 52.29 kN.

Jose, I think the material young's modulus is set in MPa, therefore defining 205E3 MPa which equals 205E9 Pa.

For those wondering, the prestress of 1.78 kN is taken from the research paper example.

Reagrds,
Jack
_________________
Jack Callaghan
Mechanical Engineering Student
Northumbria University
Back to top
View user's profile Send private message Send e-mail
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Sun Dec 07, 2014 2:27 pm  Reply with quote

On 07/12/2014 18:23, jack.callaghan wrote:
Quote:
I think I have solved the problem, which seems to have been the following code issues:

Thanks for taking the time to come back and explain the cause of the
problems. Obvious when you explain it. pi is not defined by default
but it is quite common to define a variable called pi in the
startxxx.ans file so that it is available to any macro on a particular
computer.


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

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
ernst.hustedt
User


Joined: 22 Oct 2010
Posts: 127

PostPosted: Mon Dec 08, 2014 3:15 am  Reply with quote

First let me apologise for my knotted way of thinking in my first
response. I consider a buckling load to be a value that is inherent to
the stress free structure for a given set of conditions. A pre-load (or
pre-deformation) then takes out some or all of the permissible working
load on the structure. Your example shows really well that that is not
always clear cut and as simple as this - and more!

Your reported increase of the buckling load through pre-stress (from
34.75 kN to 52.29 kN) had me baffled, as it should really be the
opposite. What you are overlooking in your model is that fact that the
structure effective in carrying the load without initial strain is just
the PIPE16 part plus only one pair of stays, i.e. the two LINK10 that go
into tension due to the 'pre bent' column when the 1N compression
compression is applied. To see the true effect of pre-stress in the
structure (a bit academic, but still) replace the LINK10 with LINK8 and
run the model with and without initial strain:
52.29 with initial strain, just as in your original LINK10 model, but
57.37 kN without initial strain (in both cases the same structure is
involved).

But now here it comes: If you do a simple static run with your model and
apply a load of just -5N, up by -4N !!!!! you will see that you are back
to the same effective structure as without initial load - so your
increase to 52.29 kN buckling load is just a dream.

Goes to show how absurd eigenvalue buckling can be.

You get closer to reality, if you crank up the initial strain to the
point where none of the stays goes slack when the buckling load plus a
margin of safety is applied in a static run. Let's see what buckling
load you end up with. You can effectively forget about LINK10 an use
LINK8, making sure that they all stay in tension.

Ernst Hustedt
AMES Ltd.
Chch, NZ

On 8/12/2014 07:23, jack.callaghan wrote:
Quote:
I think I have solved the problem, which seems to have been the following code issues:
- Setting the sinusoidal imperfections used "SI*SIN(1/6*90)" changed to "I*SIN(1/6*90)"
- PI was not recognised, changed to 3.1416

With these ammendments I achieved good results; with no inital strain the buckling load is 34.75 kN, with initail strain of 1780/100E9 the buckling load is 52.29 kN.

Jose, I think the material young's modulus is set in MPa, therefore defining 205E3 MPa which equals 205E9 Pa.

For those wondering, the prestress of 1.78 kN is taken from the research paper example.

Reagrds,
Jack

------------------------
Jack Callaghan
Mechanical Engineering Student
Northumbria 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 |
+-------------------------------------------------------------+


-----
No virus found in this message.
Checked by AVG - www.avg.com
Version: 2015.0.5577 / Virus Database: 4235/8696 - Release Date: 12/07/14


+-------------------------------------------------------------+
| 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: Mon Dec 08, 2014 11:32 am  Reply with quote

On Dec 8, 2014, at 4:15 AM, Ernst Hustedt wrote:

Quote:
Goes to show how absurd eigenvalue buckling can be.
Actually eigenvalue buckling isn't all that absurd. It works just
fine for framed structures--not so fine for curved shells. To risk
beating a dead horse, I think the real problem (besides the input
blunders that eventually came to light) is that Callaghan apparently
didn't realize that the calculated load factor applies to all the
loads present including the preload in the guy wires. Looks to me
that the results were screwy because he didn't realize that the
buckling load factor also applies to the pre-load. The preload wasn't
the initial load applied in the static analysis, rather it was the
initial pre-load multiplied by the buckling load factor.

I'd have to think about it, but I suspect you can't include a preload
in an eigenvalue buckling analysis. The problem runs fine, but the
answers don't reflect the initial preload. I also suspect that the
tension in the guy wires doesn't change much when the column loading
varies between the service and buckling loads, so maybe he could
apply the guy loading as a static load along with the service load
and get a very good assessment of the buckling load with the follow-
on buckling analysis. But maybe not--if it were my problem, I'd check
the results with an approximate energy solution as outlined in
Timoshenko's Strength of Materials text.

By way of unwanted commentary, before posting I would have also
checked the output listing and found those input typos by noting
where ANSYS had choked when it read them: WARNING--PI IS NOT A
RECOGNIZED VARIABLE, FUNCTION OR PARAMETER or something like that.
Saves a little embarrassment.


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
jack.callaghan
User


Joined: 02 Dec 2014
Posts: 4
Location: Newcastle Upon Tyne, UK

PostPosted: Mon Dec 08, 2014 12:04 pm  Reply with quote

Quote:
To see the true effect of pre-stress in the
structure (a bit academic, but still) replace the LINK10 with LINK8 and
run the model with and without initial strain

Ernst, the analysis I am trying to copy uses LINK10 elements for the stays, so for continuity I would like to use them too.
Also as the column deflects it is expected that some of the stays lose tension, so no need to make them always in tension.
Quote:
the calculated load factor applies to all the
loads present including the preload in the guy wires.

Christopher, I was not aware that this was the case. I thought the load factor only multiplied applied forces, not the real constraints of the elements.
You mention performing a static analysis of the structure with only the prstress of the stays (no applied axial force), then buckling analysis. I am quite new to ANSYS so I apologise for my ignorance, but could I do that by applying the forces on the column and crossarms that would be generated by the stays (using trig to calculate) and solving, then apply the -1N column axial force and performing buckling analysis? This would mean I would not put a prestress across the cables.

FYI The analyses in question is found in the paper "Experimental and numerical assessment of stayed steel columns" by RR. de Araujo et al. in the Journal of Construction Steel Research 64 (2008).

Regards,
Jack
_________________
Jack Callaghan
Mechanical Engineering Student
Northumbria University
Back to top
View user's profile Send private message Send e-mail
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Mon Dec 08, 2014 4:10 pm  Reply with quote

On Dec 8, 2014, at 1:04 PM, jack.callaghan wrote:

Quote:
You mention performing a static analysis of the structure with only the prstress of the stays (no applied axial force), then buckling analysis. I am quite new to ANSYS so I apologise for my ignorance, but could I do that by applying the forces on the column and crossarms that would be generated by the stays (using trig to calculate) and solving, then apply the -1N column axial force and performing buckling analysis? This would mean I would not put a prestress across the cables.

For ANSYS Classic the approach is to do a static analysis of your loading system with stress stiffening activated, then do the buckling pass to get the load factor, which is the ratio of the buckling load to the applied load. In theory the load factor applied to the static results will give you the stresses and deformations at the buckling load. As I mentioned you have to be very careful if you apply two or more independent loads because the load factor is applied to the original static solution.

Let's suppose you have a column subject to an applied load and gravity loading. You do the static analysis with a dummy applied load (=P) and the weight (=W) as calculated by ANSYS. Then you do a buckling analysis using the results from the static loading. The resulting load factor (=LF) applied to the static analysis results provides the buckling load of the structure under the factored applied load (=LF x P) and the factored weight (=LF x W). This may not be what you want.

Your question isn't clear as posed, presumably you're asking if you can apply the actual stay loading statically and use a dummy load for the axial force. In view of the foregoing you can't impose separate independent loading like that, so the way I told you probably wasn't right. However I expect using calculated forces to model the stay loading will give you about the same results as simulating the preload with a link element or some other artifice, because the column is much stiffer than the stays.

I expect you need to iterate on the stay loading so that the calculated buckling load factor times the stay load gives you the known applied stay loading at the actual axial load at buckling (= the product of the load factor x the dummy load)--basically a trial and eror solution. The stay preload probably won't vary much with axial loading because the stay stiffness is much less than the column stiffness. So you'd impose a dummy axial load equal to the service load and stay loads equal to the nominal stay loads. Then run the buckling analysis and
calculate the approximate stay loads at buckling = load factor x the input stay load for the static analysis. Change the input stay loads and repeat the initial static and the buckling run 'til you get an acceptable match. I suspect you can make the process converge quickly by dividing the calculated stay loading by perhaps half the load factor for each successive iteration.



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