Learning Forum

[Gurra]

Hi,

 

I am new to Ansys Workbench. I have a two load step solution. In the first load step I apply a force on a beam and the beam bends in the free end. In the second load step I want to remove the force, but lock the free end in its position. How do I do that? I have tried to put the displacements to zero when the second load step begins, but that only makes the end jump back to its original position when the analysis starts. How do I manage this? Thanks. 

[peteroznewman]

There is the manual way and the automatic way.

The manual way is to write down the value of deformation of the tip at the end of step 1, then delete that force load and use a remote displacement in a two-step solution. On the remote displacement tabular data, you can type in the value you wrote down from the solution using a force load on line 1 and on line 2.  If your goal is to apply a force on some other face in the model in step 2, then on that Force load, it can be zero on line 1 and whatever value you wanted on line 2.

Note that you probably want a Remote Displacement and not a Displacement on the end face of a cantilever. That is because when you apply a Force load to the end face of a cantilever, the face will move down, and also rotate.  If you apply only Displacement, the face won't rotate and you will have different deflected shape. If you apply a Remote Displacement, and only type a value in for one component (say Y component), then the face is free to rotate.

If you put a Remote Force on that face first, and right click on that and Promote to Remote Point, you can get your Deformation result on that remote point. Then when you delete the Remote Force, you can reuse the Remote Point for the Remote Displacement and type in the value from the Remote Force deformation. This will give you the identical result.  

The down side of the manual way is if you want to study many values of force, the process is manual and you have to repeat the process of writing down the deformation each time before you can do the two step solution.

The automatic way involves inserting a Command Object that fixes a Degree of Freedom of a node (such as the remote point) at the current value. You have to know APDL code to put in the Command Object. The command is D.  Here is the URL link to the ANSYS Help on that command.

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_cmd/Hlp_C_D.html

Here are instructions on how to open ANSYS Help URL links on the Student license.

 

[Gurra]

Ah, thanks a lot. So, to sum up, if I am to do this inside Workbench (without Command objects) I simply must run the first load step, where the force is applied, and then see what the displacement becomes. Then add that displacement in the second load step. I guess using Command Object with APDL code is the best way. I understand it that I should add:

D,faceName,UZ,Value

Under which item in Workbench should I add a Command Object with this line? Should "value" be zero then in the second load step? Or will that just end up with the same result as adding zero in the table in Workbench?

 

Also thanks for clarifying the difference between disp. and remote disp, I appreciate that.