Move a rigid body up and down

[ab110]

Hi All,

I want to move a rigid body up (for instance 70 mm) and then move that down -70 mm to come back to initial position. I created a simple model and put two steps for that (the model is attached). As you can see, when you put -70 mm in second step, it will not move -70 mm from this position at the end of first step and it will go to position -70 mm from starting the analysis (starting the first step). I could solve this problem by putting 0 for movement in second step. But, I am wondering if there is an option to set in ACAQUS so that the amount of movement in each step follows the previous step, not movement regarding initial position of analysis. I appreciate if someone can answer this question.

C,
A

 

[akabarten]

Hello,

if there is an option to set in ABAQUS so the amount of movement in each step follows the previous step, not movement regarding initial position of analysis

There is no option which You can turn on and after it Abaqus/Standard will set displacement boundary respect to last position not respect to initial position.
But there is a workaround for this, please use velocity type boundary condition.

...
** step 1
*BOUNDARY, TYPE=VELOCITY
node_id, 2,2, 70.0
**
** step 2
**
*BOUNDARY, TYPE=VELOCITY, OP=NEW
node_id, 2,2, -70.0
**

It will give you movement as you wish.
As long you keep step "time" equal 1.0 you do not have to worry about any calculation what velocity value you need to use to get your rigid body in specific position.
Just set velocity value to displacement you wish.

You can also use boundary condition with amplitude.
In this case you can achieve your movement in one step.

By the way displacement boundary condition in Abaqus/Explicit works as you expected.

Regards,
Bartosz

 

[ab110]

Thanks akabarten for your help.