XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Use of pilot nodes for contact coupling
 
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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jul 08, 2014 9:21 am  Reply with quote

Dear Mr. Samarakkody,

Regarding your question, in the Ansys help on TARGE169, in the section
"TARGE169 Assumptions and Restrictions", you will find the following
comment:

"For each pilot node, ANSYS automatically defines an internal node and
an internal constraint equation. The rotational DOF of the pilot node is
connected to the translational DOF of the internal node by the internal
constraint equation. You cannot use constraint equations or coupling on
pilot nodes." (ansys 11)

"For each pilot node, ANSYS automatically defines an internal node and
an internal constraint equation. The rotational DOF of the pilot node is
connected to the translational DOF of the internal node by the internal
constraint equation. ANSYS Inc. recommends against using external
constraint equations or coupling on pilot nodes; if you do, conflicts
may occur, yielding incorrect results." (ansys 15)

You do not mention the physical connection that you try to model. Since
this first step only includes the columns (without the beams), for
stability reasons their connection has to be rigid (i.e. moment
resistant) or semi-rigid. The rigid connection can be represented by
using coincident nodes at the connections. You mention that you tried
that model first, so I guess that you have rigid connections. For
semi-rigid connections you will need to add an intermediate element
which represents the joint stiffness. For example, you could do so with
MPC184 revolute joints, where you can specify the joint rotational
stiffness.

I have looked at your selection and killing sequence, and it does not
seem right. I would suggest that you review it

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 07/07/2014 07:56, dilrukshie.samarakkody escribió:

Quote:
Dear ANSYS experts,

I am trying to use beam to beam contact pairs with BEAM 188 to model the construction of three columns (three storeys) (to be later applied to a framed structure)

What I have done is:

1. created an MPC contact between one beam tip and an extra node (pilot) created at the same location (N,xxx,yyy,zzz)

2. created another MPC contact between the other beam 188 element and another extra pilot node at the same location + small offset
- finally created a coupling (CP) on all DOFs between both pilot nodes. The contact created use a CONTA175-TARGE169 pair for the Pilot Node to Contact pairing.

3. Finally to make one of these contacts disappear ( ~ KILL) I modified its PINBALL real constant to a very small value.

4. To activate it upon floor construction I changed the pinball realconstant to the distance between the two pilot nodes
RMODIF,xxxx,6,PINBALL_VALUE

So basically to simulate the construction:
I kill all elements in the 3 columns, and restrain all DOF of nodes,then floor by floor activate the
elements in columns and change the pinball value for the contact at the connection between the activated floors.

I have put nodal loads at the top of each column and the loads don't seem to transfer through the connections to the columns below.
Each column seem to behave like separate sections.

Part of the APDL script I am using to input the contact and target pairs ****************************************************

!* Creating Geometry************************
!*Key points for the lines
K,1,0,0,0,
K,2,0,3.6,0,
LSTR, 1, 2
LSEL,S,LOC,X,,0
LGEN,3,ALL, , , ,3.6, , ,0

!**** ASSIGNING THE MESH ATTRIBUTES TO CFT COLUMNS

LSEL,S,LOC,Y,0,3.6
LATT,1, ,1, , , ,1
LSEL,S,LOC,Y,3.6,7.2
LATT,2, ,1, , , ,2
LSEL,S,LOC,Y,7.2,10.8
LATT,3, ,1, , , ,3
ALLSEL,ALL
LESIZE,ALL, , ,4, , , , ,1

!****MESHING THE ELEMENTS ***********************************************
ALLSEL,ALL
LMESH,ALL

!Generating pilot nodes and contact elements
n,1000,0,3.6,0
n,1001,0,3.6,0
n,1002,0,7.2,0
n,1003,0,7.2,0
n,1001,0,3.7,0
n,1003,0,7.3,0

! Define surface-based constraint type of pair
MAT,4
R,3
REAL,3
ET,3,169
ET,4,175
KEYOPT,4,12,5
KEYOPT,4,4,3
KEYOPT,4,2,2
KEYOPT,3,2,0
KEYOPT,3,4,111
TYPE,3
! Create a pilot node
TSHAP,PILO
E,1000
! Generate the contact surface
NSEL,NONE
NSEL,A,,,5
NSEL,A,,,2
!NSEL,A,,,0
CM,_CONTACT1,NODE
TYPE,4
ESLN,S,1
ESURF

! Define surface-based constraint type of pair
MAT,4
R,4
REAL,4
ET,5,169
ET,6,175
KEYOPT,6,12,5
KEYOPT,6,4,3
KEYOPT,6,2,2
KEYOPT,5,2,0
KEYOPT,5,4,111
TYPE,5
! Create a pilot node
TSHAP,PILO
E,1001
! Generate the contact surface
NSEL,NONE
NSEL,A,,,6
NSEL,A,,,8
!NSEL,A,,,0
CM,_CONTACT1,NODE
TYPE,6
ESLN,S,1
ESURF

! Define surface-based constraint type of pair
MAT,4
R,5
REAL,5
ET,7,169
ET,8,175
KEYOPT,8,12,5
KEYOPT,8,4,3
KEYOPT,8,2,2
KEYOPT,7,2,0
KEYOPT,7,4,111
TYPE,7
! Create a pilot node
TSHAP,PILO
E,1001
! Generate the contact surface
NSEL,NONE
NSEL,A,,,10
NSEL,A,,,7
!NSEL,A,,,0
CM,_CONTACT1,NODE
TYPE,8
ESLN,S,1
ESURF
! Define surface-based constraint type of pair
MAT,4
R,6
REAL,6
ET,9,169
ET,10,175
KEYOPT,10,12,5
KEYOPT,10,4,3
KEYOPT,10,2,2
KEYOPT,9,2,0
KEYOPT,9,4,111
TYPE,9
! Create a pilot node
TSHAP,PILO
E,1001
! Generate the contact surface
NSEL,NONE
NSEL,A,,,11
NSEL,A,,,13
!NSEL,A,,,0
CM,_CONTACT1,NODE
TYPE,10
ESLN,S,1
ESURF
!** Appling Multipoint constraints to pilot nodes
NSEL,S,,,1000
NSEL,A,,,1001
cp,1,all,all
NSEL,s,,,1002
NSEL,A,,,1003
cp,7,all,all
!Removing contact
RMODIF,3,6,-0.0001
RMODIF,4,6,-0.0001
RMODIF,5,6,-0.0001
RMODIF,6,6,-0.0001
!Run analysis with construction sequence
!*
FINISH
/SOL
ALLSEL,ALL
NSEL,S,LOC,Y,,0
D,ALL,ALL,0
!ACEL, 0, 10, 0
ALLSEL,ALL,ALL
TIME,604800 ! Sets TIME value (optional for static analyses)
RATE,OFF
NLGEOM,ON ! Turns large-deflection effects on
NROPT,FULL ! You must explicitly set the Newton-Raphson option
ESEL,ALL ! Selects elements to be deactivated in this load step
EKILL,ALL ! Deactivates selected elements
ESEL,S,LIVE ! Selects all active elements
NSLE,S
NSEL,INVE ! Selects all active nodes
NSEL,U,NODE,,1000 ! Selects all inactive nodes (those not attached to any
NSEL,U,NODE,,1001
NSEL,U,NODE,,1002
NSEL,U,NODE,,1003
! active elements)
D,ALL,ALL,0 ! Constrains all inactive DOFs (optional)
NSEL,ALL ! Selects ALL nodes
ESEL,ALL
OUTRES,ALL,ALL
SOLV
!
TIME, 604900
NLGEOM,ON
AUTOTS,ON
NSUBST,20,50,20
ESEL,S,MAT,,1
EALIVE,ALL
NSLE,S
DDELE,ALL
NSEL,R,LOC,Y,3.6
D,ALL,UZ,0,,,,ROTX,ROTY
NSEL,S,LOC,Y,0
D,ALL,ALL,0
ESEL,S,MAT,,1
NSLE,S
NSEL,R,LOC,Y,3.6
F,ALL,FY,-1200
ALLSEL,ALL
OUTRES,ALL,ALL
SOLV
!
RATE,OFF
TIME, 1209700
NLGEOM,ON
AUTOTS,ON
NSUBST,20,50,20
ESEL,S,MAT,,2
EALIVE,ALL
NSLE,S
NSEL,U,LOC,Y,3.6
DDELE,ALL
NSEL,R,LOC,Y,7.2
D,ALL,UZ,0,,,,ROTX,ROTY
ESEL,S,MAT,,2
NSLE,S
NSEL,R,LOC,Y,7.2
F,ALL,FY,-1200
RMODIF,3,6,-0.2
RMODIF,4,6,-0.2
ALLSEL,ALL
OUTRES,ALL,ALL
SOLV
!
RATE,OFF
NLGEOM,ON
AUTOTS,ON
NSUBST,20,50,20
TIME, 1814500
ESEL,S,MAT,,3
EALIVE,ALL
NSLE,S
NSEL,U,LOC,Y,7.2
DDELE,ALL
NSEL,R,LOC,Y,10.8
D,ALL,UZ,0,,,,ROTX,ROTY
ESEL,S,MAT,,3
NSLE,S
NSEL,R,LOC,Y,10.8
F,ALL,FY,-1200
RMODIF,5,6,-0.2
RMODIF,6,6,-0.2
ALLSEL,ALL
OUTRES,ALL,ALL
SOLV
!
SAVE, file,db,
!

Do you have any suggestions as to what could be going wrong here or any suggestions of a method to implement the storey connections at the time steps I require during solution?
(Tried birth and death option only with common nodes at the junctions and no contact target elements, this gives high deformations at the first connecting element in the floor activated)

Thank you for reading !!!

With Kind Regards,

------------------------
Dilrukshie Samarakkody | PhD student
School of Built Environment and Civil Engineering
Science and Engineering Faculty
Queensland University of Technology
GP campus S831-13
email d1.samarakkodyarachchilage@qut.edu.au

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