List nodal stress with Beam4

[Lorens]

Hi I need to find a way to list all nodes, with its corresponding Maximum stress (direct stress + bending stress), with the nod number.

Any help are appreciated!

Kindly Paul-Martin

 

[Drej]

Take a look at the following (note the use of the ETABLE and PRETAB commands for this purpose):

allsel,all,all
esel,s,enam,,4
! create element table with SMAX and SMIN
! SMAX Maximum stress (direct stress + bending stress)
! SMIN Minimum stress (direct stress - bending stress) 

ETAB,my_SMAX_i,nmisc,1  ! SMAX at node i
ETAB,my_SMAX_j,nmisc,3  ! SMAX at node j
ETAB,my_SMIN_i,nmisc,2  ! SMIN at node i
ETAB,my_SMIN_j,nmisc,4  ! SMIN at node j

pretab,my_SMAX_i,my_SMAX_j,my_SMIN_i,my_SMIN_j

------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Lorens]

What i get with that interesting set off commands are ..

STAT CURRENT CURRENT CURRENT CURRENT
ELEM MY_SMAX_ MY_SMAX_ MY_SMIN_ MY_SMIN_
1 2700.9 2700.9 -2700.9 -2700.9

Which is nice, but not what I was seeking for, you see i need to find the axial stress in a cut, for the place of that cut have I placed a node that is why I need a nodal solution with the maximal axial stress, but it seems like that is easier said then done.

But thank you for your reply!

 

[Drej]

That is a nodal solution. And do you want axial stress or maximum stress? If you know your node number you can easily find the stress in this listing as follows.

Using the ETAB method you get a list of element number and stress for each node in that element. You cannot directly get access to the stress listing for BEAM4 (usually achieved through PRNSOL), which means you have to use the element table.

So if you want axial stress, add the following to the above:

etab,my_SDIR,LS,1,6     ! axial stress

then, if you know the node number, let's say it's 1234, just use:

nsel,s,node,,1234
esln,s
elist

Which will list the element(s) connected to your node of interest. Go to the listing of ETAB stress and find that/those element(s). The two nodal stresses for each element are listed, and should be the same. There you have your axial stress.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com