Can anyone help me include beam element 2d elastic 3. In the Preprocessor -> Element type -> Beam->i can see only 2d node 188 2d node 189 and 3d finite strain in Ansys 14.5. I am actually new to Ansys. So in watching the tutorials, they are using 2d elastic 3. When I am using beam 188 or beam 189 I am not able to add any Real constants. It is saying that these elements do not require real constants.
Hi, Nilanjan,
this popup comes from the trial to determine the BEAM3 element via
(GUI - Graphic User Interface) .
In order to work with old elements you have to work purely with APDL.
The example is below - just execute it (for example by pasting in command line, or by executing as a separate APDL file).
During Postprocessing after /POST1 you can execute line-by-line in order to see the result step-by-step.
It should work!
Regards,
Alexander
fini
/clear
!
/TITLE, Continuous Beam ! Title
! Parameters
a=1
b=0.5
c=2
d=1
q=500
M=500
P=1000
B1=0.1
H1=0.2
E = 2E11
nu = 0.3
/PREP7
! Geometrical model - lines wrt loading
K,1,0,0,
K,2,a,0,
K,3,a+b,0,
K,4,a+b+c-d,0,
K,5,a+b+c,0,
K,10, a+b,b
LSTR, 1, 2
LSTR, 2, 3
LSTR, 3, 4
LSTR, 4, 5
! Material parameters
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,E
MPDATA,PRXY,1,,nu
ET,1,BEAM3 ! Old but still working 2D FE
! options
KEYOPT,1,6,0
KEYOPT,1,9,9
KEYOPT,1,10,0
! Constants
R,1,B1*H1,(B1*H1**3)/12,H1,0, , , ! Area, moment of inertia, H1
!
LESIZE,All, , ,2,1, ! size - 2 elements
!
LMESH,ALL ! Mesh
FINISH !
!
/SOLU ! Enter the Solution processor
! Boundary conditins
NSEL,S,LOC,X,0 ! X = 0
D,ALL, , , , , ,UX,UY, , , , ! Fixed DOF - joint
NSEL,S,LOC,X,a
D,ALL, , , , , ,UY, , , , , ! Fixed DOF - movable joint
NSEL,S,LOC,X,a+b+c
D,ALL, , , , , ,ALL, , , , , ! Fixed DOF - clumped beam
! Loads
NSEL,S,LOC,X,a+b+c-d
F,ALL,FY,-P ! Force
NSEL,S,LOC,X,a+b
F,ALL,MZ,M ! Moment
! Distributed load
LSEL,S,LOC,X,0,a ! Select line
ESLL,S ! Select elements attached to the line
SFBEAM,ALL,1,PRES,q,q, , , , , ! apply distributed load to the elements
ALLSEL, ALL ! Select all
SOLVE
!
FINISH
/POST1
! Deformed shape
!
SET,FIRST
PLDISP,1
! Shear forces
! Table for the shear forces Node i: qyi
etable, qyi, smisc, 2
! Table for the shear forces Node j: qyj
etable, qyj, smisc, 62
plls, qyi, qyj ! Graphs
! Bending moments
ETABLE, MXI, SMISC, 6
ETABLE, MXJ, SMISC, 66
PLLS, MXI, MXJ
! Max absolute stresses
ETABLE, SI, NMISC, 1
ETABLE, SJ, NMISC, 21
PLLS, SI, SJ
!
These elements don't require real constants. You add the cross-sectional properties using the Section Properties. Does this help?
Hello,
It is easy but it has a trick, you should just use 3D element and constraint the third direction, i.e. you should equate displacement and rotation in third direction!
Yours,
@Angus Ramsay : Ya thanks a lot. I went to Section properties and changed the common section of beam to write the breadth and height of the beam.
@Reza Ghaffari : I am sorry. I did not get your idea. Could you explain to me one more time ?.
Hi Suraj, I think that Reza is simply giving you a tip about how to use 3D beam elements (188 189 etc) for a 2D problem - the answer being that you simply constrain the freedoms not required for the 2D problem to zero to avoid rigid-body motions in your model For example, if your beam lies in the xy-plane and along the x-axis then you would set UZ to zero at all nodes and this would eliminate rigid-body motions corresponding to translation in the z-direction, and rotation about the y-axis.
By the way, if you have the old APDL with 2D beam like BEAM3 with corresponding REAL contstants - it is still working. In ANSYS 14.5 it is no longer possible to activate 2D BEAM3 via Menu, but it is still there - correctly written APDL will work - you need old user guide for ANSYS.
At some points if you need 2D only with Moments and Force distribution it is even more transparant for teaching to use old BEAM3
As Alexander sais, you can still use BEAM3. Write in the command line for example:
ET,1,BEAM3
KEYOPT,1,6,0
KEYOPT,1,9,0
The first row defines that element 1 would be of type BEAM3. The other two define the element options - in this case keyoption 6 (membrane force + membrane output) set to 0 (exclude output) and keyoption 9 (output at extra intermed pts) also set to 0 (no intermed pts).
Once you have defined your element, real constant should be accessable through the menu.
Thanks a lot Tanya and Alexander sais. Sorry for the late response because of internet issues. When I tried it using the commands mentioned, I am getting an error message that it does not support Beam 3.
Hi Suraj,
As Tanya said first enter the Beam element by the following command line:
ET,1,3
Now your element will be added.
And then add the Real constants in the following order:
R,1,area,Moment of inertia,height(thickness),Shear z
E.g.: R,1,120,(0.9e3),30,(6/5)
Then you can proceed as usual.
It's really easy. You need to define a SECTION instead of Real constant. There you may input geometry characteristics and some other data. However, if you need to create a BEAM4, for instance, on a recent Ansys version, you may write a command line: et, 200, BEAM4 (Where 200 is the element type number). Then, you need to define a real constant set for this BEAM with: R,200, (parameters)
Regards
@Arun.. Still the problem is not solving. I am getting the same popup as Mr. Suraj told.. Please help me out.
Share a printscreen from your output window (black panel) or please share the *.err file and I may help you
Hi, Nilanjan,
this popup comes from the trial to determine the BEAM3 element via
(GUI - Graphic User Interface) .
In order to work with old elements you have to work purely with APDL.
The example is below - just execute it (for example by pasting in command line, or by executing as a separate APDL file).
During Postprocessing after /POST1 you can execute line-by-line in order to see the result step-by-step.
It should work!
Regards,
Alexander
fini
/clear
!
/TITLE, Continuous Beam ! Title
! Parameters
a=1
b=0.5
c=2
d=1
q=500
M=500
P=1000
B1=0.1
H1=0.2
E = 2E11
nu = 0.3
/PREP7
! Geometrical model - lines wrt loading
K,1,0,0,
K,2,a,0,
K,3,a+b,0,
K,4,a+b+c-d,0,
K,5,a+b+c,0,
K,10, a+b,b
LSTR, 1, 2
LSTR, 2, 3
LSTR, 3, 4
LSTR, 4, 5
! Material parameters
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,E
MPDATA,PRXY,1,,nu
ET,1,BEAM3 ! Old but still working 2D FE
! options
KEYOPT,1,6,0
KEYOPT,1,9,9
KEYOPT,1,10,0
! Constants
R,1,B1*H1,(B1*H1**3)/12,H1,0, , , ! Area, moment of inertia, H1
!
LESIZE,All, , ,2,1, ! size - 2 elements
!
LMESH,ALL ! Mesh
FINISH !
!
/SOLU ! Enter the Solution processor
! Boundary conditins
NSEL,S,LOC,X,0 ! X = 0
D,ALL, , , , , ,UX,UY, , , , ! Fixed DOF - joint
NSEL,S,LOC,X,a
D,ALL, , , , , ,UY, , , , , ! Fixed DOF - movable joint
NSEL,S,LOC,X,a+b+c
D,ALL, , , , , ,ALL, , , , , ! Fixed DOF - clumped beam
! Loads
NSEL,S,LOC,X,a+b+c-d
F,ALL,FY,-P ! Force
NSEL,S,LOC,X,a+b
F,ALL,MZ,M ! Moment
! Distributed load
LSEL,S,LOC,X,0,a ! Select line
ESLL,S ! Select elements attached to the line
SFBEAM,ALL,1,PRES,q,q, , , , , ! apply distributed load to the elements
ALLSEL, ALL ! Select all
SOLVE
!
FINISH
/POST1
! Deformed shape
!
SET,FIRST
PLDISP,1
! Shear forces
! Table for the shear forces Node i: qyi
etable, qyi, smisc, 2
! Table for the shear forces Node j: qyj
etable, qyj, smisc, 62
plls, qyi, qyj ! Graphs
! Bending moments
ETABLE, MXI, SMISC, 6
ETABLE, MXJ, SMISC, 66
PLLS, MXI, MXJ
! Max absolute stresses
ETABLE, SI, NMISC, 1
ETABLE, SJ, NMISC, 21
PLLS, SI, SJ
!
I AM NEW at ansys .add a have the same problem ..
I do not understand the previous answers
Can any one help me ,please?
BEAM3 was in old version now you can do same analysis in beam188 ,actually BEAM3 was only for rectangular cross section by providing cross sectional area in 'real constant' but in BEAM188 you can do analysis of beam having rectangular, circular or many different cross section by providing cross sectional information in 'section' instead of 'real constant'
If you use beam188 or beam189 then you add the beam cross sectional area using the beam tool rather than as real constants.
Good question.. Please share me the best answer might you trust...
Regards…
- Badges
- Science topic