×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Importing displacement boundary conditions.

Importing displacement boundary conditions.

Importing displacement boundary conditions.

(OP)
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?

RE: Importing displacement boundary conditions.

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 clown

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.

RE: Importing displacement boundary conditions.

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources