Ansys meshing

  • Thread starter engr86
  • Start date
  • #1
2
0

Main Question or Discussion Point

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?
 

Answers and Replies

  • #2
minger
Science Advisor
1,495
2
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,
 
  • #3
Mech_Engineer
Science Advisor
Gold Member
2,572
171
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.
 
  • #4
2
0
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?
 
  • #5
minger
Science Advisor
1,495
2
That's probably the easiest way. As mentioned though, you need to line mesh. Put keypoints [K,num,x,y,z] at all the intersections. Then draw lines from keypoint to keypoint [L,kp1,kp2]. Then, you define your sectypes as I mentioned above.

At this point, I'll give the obligatory RTFM for defining beam sections.

At that point, simply LMESH the lines, apply boundary conditions and solve. From the sound of it, you need to spend a few days and just go through the help, do some test cases, get accustomed to the software.
 

Related Threads on Ansys meshing

  • Last Post
Replies
1
Views
12K
  • Last Post
Replies
11
Views
16K
Replies
1
Views
19K
Replies
0
Views
694
Replies
5
Views
3K
Top