×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Contact 171 element

Contact 171 element

Contact 171 element

(OP)
I am trying to run a test problem involving Contact171 elements. It is a contact problem between two cantilevered beams. The upper beam bended over and touch the lower beam. But when I plot the von Mises stress, the lower beam has zero stress. It seems that I missed some settings for the contact pair. Here is my input:

/prep7  
! Top Beam  
*SET,X1,0   
*SET,Y1,15  
*SET,L1,100
*SET,H1,10  
! Bottom Beam   
*SET,X2,50  
*SET,Y2,0   
*SET,L2,100
*SET,H2,10  
! Create Geometry   
blc4,X1,Y1,L1,H1
blc4,X2,Y2,L2,H2
! define element type   
ET,1,plane42     ! element type 1   
keyopt,1,3,3        ! plane stress w/thick  
type,1              ! activate element type 1   
R, 1, 10            ! thickness 0.01
! define material properties
MP,EX,  1, 2000e3    ! Young's modulus   
MP,NUXY,1, 0.3      ! Poisson's ratio   
! meshing   
esize,2             ! set meshing size  
amesh,all           ! mesh area 1   
ET,2,contac48       ! defines second element type - 2D contact elements
keyo,2,7,1     ! contact time/load prediction   
r,2,200000,,,,10
TYPE,2              ! activates or sets this element type   
real,2      ! activates or sets the real constants  
! define contact nodes and elements
! first the contact nodes   
asel,s,area,,1           ! select top area  
nsla,s,1                 ! select the nodes within this area
nsel,r,loc,y,Y1          ! select bottom layer of nodes in this area
nsel,r,loc,x,X2,(X2+L2/2)! select the nodes above the other beam
cm,source,node           ! call this group of nodes 'source'
! then the target nodes
allsel                   ! relect everything
asel,s,area,,2           ! select bottom area   
nsla,s,1                 ! select nodes in this area
nsel,r,loc,y,H2          ! select bottom layer of nodes in this area
nsel,r,loc,x,X2,(X2+L2/2)! select the nodes above the other beam
cm,target,node           ! call this selection 'target'
gcgen,source,target,3    ! generate contact elements between defined nodes  
allsel               ! relect everything
finish  
/solut  
antype,0
time,1   ! Sets time at end of run to 1 sec
autots,on  ! Auto time-stepping on  
nsubst,100,1000,20 ! Number of sub-steps
outres,all,all  ! Write all output  
neqit,100  ! Max number of iterations   
nsel,s,loc,x,X1  ! Constrain top beam   
nsel,r,loc,y,Y1,(Y1+H1)
d,all,all   
nsel,all
nsel,s,loc,x,(X2+L2) ! Constrain bottom beam
nsel,r,loc,y,Y2,(Y2+H2)
d,all,all   
nsel,all
nsel,s,loc,x,(L1/2+X1) ! Apply load
nsel,r,loc,y,(Y1+H1)
f,all,fy,-100000
nsel,all
solve   
finish  

Did I missed something obvious?

Thanks a lot,

RE: Contact 171 element

Hi,

You are using Contact48 elements not Contact171 elements.

However the von mises stresses are not null.

After the solution copy/paste this in the command line:

/post1
set,last
PLNSOL,S,EQV,0,1
/contour,all,10,.551e-7,,2000
/replot

Regards,
Alex

PS: you mistyped /SOLU in your input code (/solut), see above.


RE: Contact 171 element

What Ansys version are you using? It seems that the old contac48 elements are no longer avalable in the 8.1 version that I am using.

In my opinion, the contact elements in your modell have too much penetration. You can see that if you set the display scale to 1 (/dscale,all,1). However I could't list the actual penetration for this elements.

I have used the conta175 point to surface elements insted of the contac48 elements. The penetration I get is relatively small (see input code below)


fini
/clear,start
/prep7  
! Top Beam  
*SET,X1,0   
*SET,Y1,15  
*SET,L1,100
*SET,H1,10  
! Bottom Beam   
*SET,X2,50  
*SET,Y2,0   
*SET,L2,100
*SET,H2,10  
! Create Geometry   
blc4,X1,Y1,L1,H1
blc4,X2,Y2,L2,H2
! define element type   
ET,1,plane42     ! element type 1   
keyopt,1,3,3        ! plane stress w/thick  
type,1              ! activate element type 1   
R, 1, 10            ! thickness 0.01
! define material properties
MP,EX,  1, 2000e3    ! Young's modulus   
MP,NUXY,1, 0.3      ! Poisson's ratio   
! meshing   
esize,2             ! set meshing size  
amesh,all           ! mesh area 1   
et, 2, conta175, , , , , , , 1, , , 1    ! contact algorithm: augmented lagrangian. (keyopt(2)=0)
! contact stiffness update: each substep based on mean stress of underlying elements
! from the previous substep. (keyopt(10)=1)
r, 2, , , 0.1, 0.01    ! Kontact stiffnes and penetration
et, 3, targe169    ! 2-d target element

TYPE,2              ! activates or sets this element type   
real,2      ! activates or sets the real constants  
! define contact nodes and elements
! first the contact nodes   
asel,s,area,,1           ! select top area  
nsla,s,1                 ! select the nodes within this area
nsel,r,loc,y,Y1          ! select bottom layer of nodes in this area
nsel,r,loc,x,X2,(X2+L2/2)! select the nodes above the other beam
esurf    ! generate contact elements
! then the target nodes
type,3        ! activate target elements
real,2        ! same real for the target elements!!
allsel                   ! relect everything
asel,s,area,,2           ! select bottom area   
nsla,s,1                 ! select nodes in this area
nsel,r,loc,y,H2          ! select bottom layer of nodes in this area
nsel,r,loc,x,X2,(X2+L2/2)! select the nodes above the other beam
esurf    ! generate target elements
allsel               ! relect everything
finish  
/solu
antype,0
time,1   ! Sets time at end of run to 1 sec
autots,on  ! Auto time-stepping on  
nsubst,100,1000,20 ! Number of sub-steps
outres,all,all  ! Write all output  
neqit,100  ! Max number of iterations   
nsel,s,loc,x,X1  ! Constrain top beam   
nsel,r,loc,y,Y1,(Y1+H1)
d,all,all   
nsel,all
nsel,s,loc,x,(X2+L2) ! Constrain bottom beam
nsel,r,loc,y,Y2,(Y2+H2)
d,all,all   
nsel,all
nsel,s,loc,x,(L1/2+X1) ! Apply load
nsel,r,loc,y,(Y1+H1)
f,all,fy,-100000
nsel,all
solve   
finish  
/post1
set,last
PLNSOL,S,EQV,0,1
/contour,all,10,.551e-7,,2000
/dscale,all,1
/replot

RE: Contact 171 element

(OP)
Thanks mihaiupb. I am using 9.0. I am using this tutorial example to get myself familiar with contact elements.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources