# Ansys meshing

engr86
I'm using anysis to model a 3-d object. i'm using a series of beams. however, when i try to mesh the beams, it says that it's unable to do that. When I add a shell, anysis meshes the model. How do I create a mesh with only beam objects?

BEAM elements must be meshed on lines, using the LMESH command with the proper TYPE, REAL, and SECN set prior. The following is a full example of a static analysis using beam elements
Code:
/prep7

!--insert materials here
SECTYPE,1,BEAM,CSOLID
SECDATA,1.0,8,2

!--define geometry
k,,0,0,0
k,,10,0,0
l,1,2

!--mesh the line
type,1
real,1
secn,1
lmesh,1

!--boundary conditions
ksel,s,kp,,1
nslk
d,all,ux,0.0,,,,uy,uz,rotx,roty,rotz

ksel,s,kp,,2
nslk
f,all,fx,-100

allsel,all
/solu
antype,static
save
solve
save
finish

edit: You can use the command /ESHAPE,1 to turn on the element shaping which allows you to "see" what the beams look like. This can be important when you start using orientation nodes and need to see which way unsymmetric elements are facing. Good luck,

Gold Member
When you say a 3-D object, is it a truss structure with lines that are defined in 3-D? Beams can only be meshed to lines; if your object is a volume or surface, you cannot use beam elements to mesh it.

engr86
I'm trying to model a 3-d object (a frame with t-bars) and I thought that defining 3d beams would be the best way. Is there an easier way?