Importing displacement boundary conditions. 1

[sd300]

Dear All,

I'm trying to apply a displacement boundary condition to a static structural model. It's taken from medical images and it can't be approximated by a simple function.

I have a file with all the node numbers and the displacements (generated externally) I want to apply to them and was hoping there was a straight forward way to import them to ANSYS.

What is the best way to go about this?

 

[JaStKn]

Hi!

First you have to read the file into ANSYS. The best way is the usage of the *tread command to do this. *vread or *mread are the other ways. By using the *tread command you do'nt have to define the format of the file )

Of course you must define a table or an array before reading the file. (*dim command)

If you have the data in the table (first column node numbers, second and following columns displacements) you can define the boundary conditions for every node using a do-loop.

e.g:

*do,i,1,n
d,table(i,1),ux,table(i,2)
d,table(i,1),uy,table(i,3)
d,table(i,1),uz,table(i,4)

*enddo

Or via implied do loop

d,table(1:n,1),ux,table(1:n,2)
d,table(1:n,1),uy,table(1:n,3)
d,table(1:n,1),uz,table(1:n,4)

(this is the faster way)

hope this helps, best regards .... Stefan.

 

[feavnik]

Hi there,
try this

*dim,dx,,40
define your data in an array. Select the line, area or volume on which the nodes of interest lies.
NN=0
*get,numloop,NODE,0,count
*do,i,1,numloop
*get,nodeload,NODE,NN,NXTH
d,nodeload,uy,dy(i)
NN=nodeload
*enddo

This stuff works. I've used this.

Cheers
FEAVNIK