×
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

Boundary from the results of previous step?

Boundary from the results of previous step?

Boundary from the results of previous step?

(OP)
Hi,

I want to enforce a *BOUNDARY condition (displacement) that is dependent on the results of a previous step.
For instance, if I plastically deform a material and then unload the material, plastic deformations exist. I then want to displace a certain node 1 inch based on the results after unloading.

I have tried to  used dummy nodes with the *Equation option, but for this to work, I would have to make the equation active after the previous step. Or does anyone know of a way that I can specify a boundary condition that is a movement from the previous step result and not using the FIXED condition. Any help would be greatly appreciated. Thank you.

RE: Boundary from the results of previous step?

I may be completely missing the point here but isn't it this simple?

*STEP, NLGEOM
[PLASTIC DEFORMATION LOAD STEP]
*ENDSTEP
*STEP
[PLASTIC DEFORMATION UNLOAD STEP]
*ENDSTEP
*STEP
*STATIC
*BOUNDARY
node,dof,,<distance>
*ENDSTEP

RE: Boundary from the results of previous step?

Displacements are carried on to the next step. gwolf is correct though you might need a OP=NEW option here and there.

corus

RE: Boundary from the results of previous step?

(OP)
Thank you for the replies gwolf and corus. You are both correct. The problem is that I don't know what the <distance> is. I know what its magnitude has to be in "comparison" the previous step result.

For instance, I want Node 10 to move 1 inch from where it was after Step 2. The problem is I do not know where Node 10 will be after Step 2. I want to run all steps but right now I have to stop the analysis before programming Step 3.

I currently would run Step 2 with a *RESTART, WRITE option, and then perform a *RESTART, READ and displace the node 1 inch from the result of Step 2. It works but being able to program this for the same analysis over night would be beneficial. RIght now, to run my files overnight, I need to get up about every 3.5 hours.

RE: Boundary from the results of previous step?

Idea 1: Use a contact definition in your model. Contact area = target position for node

Idea 2:Activate a nonlinear spring in the last step by using *MODELCHANGE,ADD. This spring should act between the node and the target position. Choose nonlinear spring stiffness so that there a huge nodal force if node isn't at target position.

Pam  

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