XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Combin14 for modal 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
zhongfeng.wang
User


Joined: 10 Jul 2013
Posts: 10
Location: Kuala Lumpur

PostPosted: Mon Nov 11, 2013 8:27 pm  Reply with quote

Dear XANSYS friends,

I am trying to use combin14 to model interaction between multispan pipeline (around 100m) and seabed (contact length varies from few meters to 10meters). I defined pipeline as PIPE16 element and at where it contacts with seabed, I draw horizontal and vertical lines (perpendicular to the pipeline with 100mm length) @ 1m spacing and assign combin14 to them. I then fixe both ends of the pipeline and all ends of the springs.

After I run modal analysis, i found out that it does not matter what stiffness i assign to those springs, the mode shape and natural frequencies are not changing.

Below shows part of the script I wrote, and this is after i define the geometry.

I understand that i have not model the friction so i have tried to use conta178 in another try (also does not work), but at moment really want to figure out why the stiffness of combin14 does not affect the modal analysis results.

Thank you very much in advance.


Define geometry....

!* Assign element atributes

ET,1,PIPE16
ET,2,combin14
keyopt,2,2,2,

R,1,OD,nomwt, , , ,
R,2,6

UIMP,1,EX, , ,29000,
UIMP,1,DENS, , ,eqwt,
UIMP,1,ALPX, , ,6.5e-6,
UIMP,1,PRXY, , ,0.3,

LSEL,S,LINE,,1, 17 ,1
LATT,1,1,1

Lsel,inve
LATT,1,2,2

LSEL,ALL
ESIZE,10,0,
LMESH,ALL

LSCLEAR,ALL
NLGEOM, OFF

Apply load....

/SOLU
lsclear,all
lssolve,1,1,1
FINISH

/SOLU
PSTRES,on
ANTYPE,2

MSAVE,0

EQSLV,sparse

MXPAND,30, , ,1
!IRLF,-1

LUMPM,0

MODOPT,LANB,30,0,0, ,ON

/STATUS,SOLU

SOLVE
finish
save
Back to top
View user's profile Send private message
zhongfeng.wang
User


Joined: 10 Jul 2013
Posts: 10
Location: Kuala Lumpur

PostPosted: Mon Nov 11, 2013 8:34 pm  Reply with quote

Just noticed my signature does appear. Hope this time works...
_________________
Wang Zhongfeng - Structural Engineer
Genesis Oil and Gas Consultants Malaysia Sdn Bhd
Level 6, Menara JCorp, 249 Jalan Tun Razak, Kuala Lumpur, 50400
Tel (Direct) +60 3 2028 3037 | Office +60 3 2028 3000 | Fax +60 3 2145 4434
Back to top
View user's profile Send private message
jerzy.cwifeld
User


Joined: 02 May 2013
Posts: 39

PostPosted: Tue Nov 12, 2013 12:20 am  Reply with quote

Hi
The modal analysis do not accept any non-linearity's

Regards
Jerzy
+46 73 7305104
-----Ursprungligt meddelande-----
Från: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] För zhongfeng.wang
Skickat: den 12 november 2013 04:28
Till: xansys@xansys.org
Ämne: [Xansys] Combin14 for modal analysis

Dear XANSYS friends,

I am trying to use combin14 to model interaction between multispan pipeline (around 100m) and seabed (contact length varies from few meters to 10meters). I defined pipeline as PIPE16 element and at where it contacts with seabed, I draw horizontal and vertical lines (perpendicular to the pipeline with 100mm length) @ 1m spacing and assign combin14 to them. I then fixe both ends of the pipeline and all ends of the springs.

After I run modal analysis, i found out that it does not matter what stiffness i assign to those springs, the mode shape and natural frequencies are not changing.

Below shows part of the script I wrote, and this is after i define the geometry.

I understand that i have not model the friction so i have tried to use conta178 in another try (also does not work), but at moment really want to figure out why the stiffness of combin14 does not affect the modal analysis results.

Thank you very much in advance.


Define geometry....

!* Assign element atributes

ET,1,PIPE16
ET,2,combin14
keyopt,2,2,2,

R,1,OD,nomwt, , , ,
R,2,6

UIMP,1,EX, , ,29000,
UIMP,1,DENS, , ,eqwt,
UIMP,1,ALPX, , ,6.5e-6,
UIMP,1,PRXY, , ,0.3,

LSEL,S,LINE,,1, 17 ,1
LATT,1,1,1

Lsel,inve
LATT,1,2,2

LSEL,ALL
ESIZE,10,0,
LMESH,ALL

LSCLEAR,ALL
NLGEOM, OFF

Apply load....

/SOLU
lsclear,all
lssolve,1,1,1
FINISH

/SOLU
PSTRES,on
ANTYPE,2

MSAVE,0

EQSLV,sparse

MXPAND,30, , ,1
!IRLF,-1

LUMPM,0

MODOPT,LANB,30,0,0, ,ON

/STATUS,SOLU

SOLVE
finish
save






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

____________________________________________________________________________
Privileged/Confidential information may be contained in this message and is intended solely for the use of the addressee. If You receive this mail by mistake, You may not use, copy or distribute it to anyone else.<br/>Please erase the message and notify us immediately.

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
zhongfeng.wang
User


Joined: 10 Jul 2013
Posts: 10
Location: Kuala Lumpur

PostPosted: Tue Nov 12, 2013 12:23 am  Reply with quote

Thanks Jerzy for the reply. I only apply stiffness and no damping value has been given, so I presume this is still linear case?

Cheers,


Wang Zhongfeng - Structural Engineer
Genesis Oil and Gas Consultants Malaysia Sdn Bhd
Level 6, Menara JCorp, 249 Jalan Tun Razak, Kuala Lumpur, 50400
Tel (Direct) +60 3 2028 3037 | Office +60 3 2028 3000 | Fax +60 3 2145 4434



From: <Jerzy.Cwifeld@okg.eon.se>
To: <xansys@xansys.org>
Date: 12/11/2013 03:20 PM
Subject: Re: [Xansys] Combin14 for modal analysis
Sent by: xansys-bounces@xansys.org



Hi
The modal analysis do not accept any non-linearity's

Regards
Jerzy
+46 73 7305104
-----Ursprungligt meddelande-----
Från: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org (xansys-bounces@xansys.org)] För zhongfeng.wang
Skickat: den 12 november 2013 04:28
Till: xansys@xansys.org
Ämne: [Xansys] Combin14 for modal analysis

Dear XANSYS friends,

I am trying to use combin14 to model interaction between multispan pipeline (around 100m) and seabed (contact length varies from few meters to 10meters). I defined pipeline as PIPE16 element and at where it contacts with seabed, I draw horizontal and vertical lines (perpendicular to the pipeline with 100mm length) @ 1m spacing and assign combin14 to them. I then fixe both ends of the pipeline and all ends of the springs.

After I run modal analysis, i found out that it does not matter what stiffness i assign to those springs, the mode shape and natural frequencies are not changing.

Below shows part of the script I wrote, and this is after i define the geometry.

I understand that i have not model the friction so i have tried to use conta178 in another try (also does not work), but at moment really want to figure out why the stiffness of combin14 does not affect the modal analysis results.

Thank you very much in advance.


Define geometry....

!* Assign element atributes

ET,1,PIPE16
ET,2,combin14
keyopt,2,2,2,

R,1,OD,nomwt, , , ,
R,2,6

UIMP,1,EX, , ,29000,
UIMP,1,DENS, , ,eqwt,
UIMP,1,ALPX, , ,6.5e-6,
UIMP,1,PRXY, , ,0.3,

LSEL,S,LINE,,1, 17 ,1
LATT,1,1,1

Lsel,inve
LATT,1,2,2

LSEL,ALL
ESIZE,10,0,
LMESH,ALL

LSCLEAR,ALL
NLGEOM, OFF

Apply load....

/SOLU
lsclear,all
lssolve,1,1,1
FINISH

/SOLU
PSTRES,on
ANTYPE,2

MSAVE,0

EQSLV,sparse

MXPAND,30, , ,1
!IRLF,-1

LUMPM,0

MODOPT,LANB,30,0,0, ,ON

/STATUS,SOLU

SOLVE
finish
save






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

____________________________________________________________________________
Privileged/Confidential information may be contained in this message and is intended solely for the use of the addressee. If You receive this mail by mistake, You may not use, copy or distribute it to anyone else.<br/>Please erase the message and notify us immediately.

+-------------------------------------------------------------+
| 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 Nov 12, 2013 6:02 am  Reply with quote

For the combin14 you have used keyopt(2)=2, which means that you have a 1-D longitudinal spring-damper (with only UY degree of freedom). If your pipeline is parallel to the Y axis and is fixed in both ends, your combin14 elements will not be working as you expect them to. You need them to provide stiffness in directions perpendicular to the pipeline, that is, X and Z directions (assuming your pipeline is parallel to the Y axis).
You say that you are defining lines perpendicular to the pipeline, and meshing them with combin14 elements. That means that your combin14 have non-coincident nodes. Therefore, I would suggest that you use keyopt(2)=0.
Best regards,
Jose M. Galan
Assistant Professor
Dept. Engineering Construction
Universidad de Sevilla


El 12/11/2013 04:28, zhongfeng.wang escribió:
Quote:
Quote:
Dear XANSYS friends,

I am trying to use combin14 to model interaction between multispan pipeline (around 100m) and seabed (contact length varies from few meters to 10meters). I defined pipeline as PIPE16 element and at where it contacts with seabed, I draw horizontal and vertical lines (perpendicular to the pipeline with 100mm length) @ 1m spacing and assign combin14 to them. I then fixe both ends of the pipeline and all ends of the springs.

After I run modal analysis, i found out that it does not matter what stiffness i assign to those springs, the mode shape and natural frequencies are not changing.

Below shows part of the script I wrote, and this is after i define the geometry.

I understand that i have not model the friction so i have tried to use conta178 in another try (also does not work), but at moment really want to figure out why the stiffness of combin14 does not affect the modal analysis results.

Thank you very much in advance.


Define geometry....

!* Assign element atributes

ET,1,PIPE16
ET,2,combin14
keyopt,2,2,2,

R,1,OD,nomwt, , , ,
R,2,6

UIMP,1,EX, , ,29000,
UIMP,1,DENS, , ,eqwt,
UIMP,1,ALPX, , ,6.5e-6,
UIMP,1,PRXY, , ,0.3,

LSEL,S,LINE,,1, 17 ,1
LATT,1,1,1

Lsel,inve
LATT,1,2,2

LSEL,ALL
ESIZE,10,0,
LMESH,ALL

LSCLEAR,ALL
NLGEOM, OFF

Apply load....

/SOLU
lsclear,all
lssolve,1,1,1
FINISH

/SOLU
PSTRES,on
ANTYPE,2

MSAVE,0

EQSLV,sparse

MXPAND,30, , ,1
!IRLF,-1

LUMPM,0

MODOPT,LANB,30,0,0, ,ON

/STATUS,SOLU

SOLVE
finish
save






+-------------------------------------------------------------+
| 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-mod@tynecomp.co.uk) |
+-------------------------------------------------------------+



Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
zhongfeng.wang
User


Joined: 10 Jul 2013
Posts: 10
Location: Kuala Lumpur

PostPosted: Tue Nov 12, 2013 6:35 pm  Reply with quote

Hi Jose,

Thank you very much for your detail explanation. Now it makes sense to me that I did not define the horizontal spring direction and that it why it gave me some strange results. My pipe is in x direction so I only defined the vertical spring direction but missed the horizontal z direction one.

I defined the horizontal springs separately and used keyopt(2) = 3 with different spring stiffness values (just to make it more accurate) and it works now. I am pretty sure keyopt(2) also works but thought i have to use different stiffness values so have not given it a try.

It would be great if you could help me on the other concern. I understand that normally node to node contact is suitable for small deflection/movement but not quite sure if my case here still belong to the category. It is a 3d problem and at the contact region, I tried to get unified stress based on 1in deflection for modal analysis. And for strength analysis, i would expect the deflection more than that. I chose to use combin14 just for simplicity compare with those node to surface contact types.

Thanks again for your help on this Jose,

Cheers,
_________________
Wang Zhongfeng - Structural Engineer
Genesis Oil and Gas Consultants Malaysia Sdn Bhd
Level 6, Menara JCorp, 249 Jalan Tun Razak, Kuala Lumpur, 50400
Tel (Direct) +60 3 2028 3037 | Office +60 3 2028 3000 | Fax +60 3 2145 4434
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