Hello everybody,
I'd like to model an elastic supported beam with a crosssection in Ansys. I need to change the stiffness of the springs under the nodes seperately. Does anybody know, how to automatically create springs on every node of the model? I'd prefer a solution directly in Workbench, but as far as I know I have to do a Do/Endo loop in APDL that selects the single node and create a COMBIN 14 for it. Is that right or are there other solutions possible? Could you please show me the coding commands, as I haven't worked with APDL so far.
Thanks a lot!
Can you share your Ansys model in cdb format?
Can you provide the stiffness of the springs?
Is it a planar model?
I'd take a stiffness of 22500 N/mm for starting. I'm using a line body with an assigned cross section so the model is kind of planar. I'm probably going to refine the element size. I'm using Ansys 2019 R3.
I'm really looking forward to your answer.
Alina, I attach a matlab file. If you have a lot of node placed on a surface you have to export the node in an ascii format (nodi.txt) and then, by reading this file, this routine creates an input Ansys macro (Modello_test.mac) that generates the model. Then you can modify real costant etc.
The combin 14 direction is the same for all the nodes (in this case z) and in this routine version all springs have a length of 1.0 (mm). But you can modify the routine as you prefer
Filippo Cianetti
Hello Filippo,
I tried to solve my problem now multiple times, but it still does not work. Could you please explain your method a little bit more detailed? How do I export the nodes? So far I only know how to get the nodenumber/Maximum of nodes (Command *get). And I have understood you correctly that I have to read the macroscript in Workbench? But how do I create the spring elements under the nodes?
Sorry, I'm really new to Ansys and scripting.
Thanks
Alina,
my routine writes a macro file for APDL and so to be read in this evironment to create the springs but I think could be used also into Workbench. To export the nodelist file from APDL is to digit NLIST. The output could be directed to external file by digit before NLIST the command /OUTPUT,NOMEFILE,EXT
I hope that I've explained it better than in the previous message.
Filippo
I solved the problem in APDL as shown:
nplot
FINISH
/PREP7
*get,Nodenumber,node,,count
!Create new nodes at the distance of the following spring legths
*do,i,1,Nodenumber
N,k,nx(i),ny(i)-100,nz(i),,,,
k=_return
*enddo
*get,Nodenumberneu,node,,count
!Fixation of the new nodes
*do,i,Nodenumber+1,Nodenumberneu
FLST,2,1,1,ORDE,1
FITEM,2,i
!*
/GO
D,P51X, , , , , ,ALL, , , , ,
*enddo
!Create the spring element
!*
ET,2,COMBIN14
!*
KEYOPT,2,1,0
KEYOPT,2,2,2
KEYOPT,2,3,0
!*
R,1,insertspringstiffness, , , , , ,
RMORE, ,
!*
DOF,UY
Type,2
!Insert springs beneath the beam
!Watch out to have the node numbering in the new nodes in the same order as the nodes of the beam
*do,i,1,Nodenumber
E,i,i+Nodenumber
*enddo
eplot
Of course this simple code only works for 2D beams. For my 3D modelling I had to specify it a lot. But hopefully, this code helps others, that-like me at that time-have just started APDL.
- Badges
- Science topic
- Similar topics
- Engineering
- Mechanical Engineering