×
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

problem with multiple displacement load step

problem with multiple displacement load step

problem with multiple displacement load step

(OP)
I'm performing a two load step analysis. In the first step I'm pre-loading the structure at two key points (points 1 and 3) by applying a displacement condition. In the second step, once the structure is preloaded, I'm actuating the structure from a third key point (point 4), again by a displacement condition (no force is applied). The problem is the following, during the first load step, point 4 suffers some displacement from its initial position, now, during the second load step I would expect the point 4 would displace from its actual position (solution given by first load step) to the given displacement condition, but instead, ANSYS snaps the structure to a configuration where point 4 is again in the initial position and then applies the given displacement, while the pre-stress is still in consideration. This ANSYS files attached as well as a figure, where the displacement of point 4 is plotted against the pseudo-time. the upper figure shows the actual result, the lower figure shows, what I would be expecting and I'm not getting.

RE: problem with multiple displacement load step

What you describe is exactly how it should occur. Remember that enforced displacement (using the "d" command) is always relative from a node/s initial (undeformed) position.


------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: problem with multiple displacement load step

(OP)
Thanks Drej for your answer.

Do you have any idea, how can I make then, that the second load step applies the displacement condition, starting from the deformed position after the first load step?

Or this is just not possible?

RE: problem with multiple displacement load step

In your first step, you apply UX displacements to KP 1 and 3, and since KP 4 is unconstrained in the UX it is allowed to move by -2.19 units. Then, you attempt to apply a displacement of -1.5 units to KP 4. Since you did not constrain KP 4 in the first load step, ANSYS will immediately bring the KP back to its original position and THEN apply the UX of -1.5 units. I don't know the details of your model, but if you want to bring KP from -2.19 to -1.5 without the snap back to zero, you will need to apply a displacement of -2.19 at KP 4 in the first load step and then in the second load step apply UX at KP 4 of -1.5.

As I say, I'm not sure of your model details. Maybe you need to consider applying a UX constraint of zero at KP 4 in the first load step, and then applying your actuation at KP 4 in the second?


------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: problem with multiple displacement load step

(OP)
Now, I've run the analysis including a displacement condition of -2.19 for kp4 at the first load step, keeping conditions at kp1 and kp3, and kp4 is behaving as I want, but now the problem is that I'm getting a force reaction different to zero for kp4 at the beginning of the second load step.

Should be zero, don't you think? (because displacement of -2.19 is the displacement for equilibrium at kp4 just with pre-loading at kp 1 and 3)

Thanks again for your help!

RE: problem with multiple displacement load step

Not really. This is a non-linear model and is therefore path dependent, so it is perfectly reasonable that the reaction is non-zero. How much is non-zero?

The important thing is that your boundary conditions represent those in your physical system.


------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

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