A transient analysis after a static analysis in Workbench, Mechanical application

  • 3.1K Views
  • Last Post 22 May 2020
  • Topic Is Solved
mutianzi1 posted this 21 April 2019

Hi. I was performing a transient analysis of a structure. Below is the time history of displacement of the structure. Due to the abrupt application of the load, there is a transient effect at the beginning of the time history (very large fluctuations).

To reduce the transient effects. I conducted a static analysis before the transient analysis, and the load for the static analysis is the same as the load in the first time step in the transient analysis. Below is the setup in Workbench. But I got the same results as the case that I only conducted transient analysis. Does anyone know how does this happen? Anything wrong with the setup? 

Thanks in advance. Any help is appreciated.

Order By: Standard | Newest | Votes
peteroznewman posted this 21 April 2019

Can your model be solved with only linear behavior?

If so, you can use Modal Superposition (MSUP) to solve the Transient and you can Pre-Stress the Modal with the Static Structural.

mutianzi1 posted this 21 April 2019

I guess not. I used bilinear material, and the large deflection is turned on. 

  • Liked by
  • sma4t
jj77 posted this 22 April 2019

Pre stress creates an initial stress that is translated to an equivalent stiffness matrix -Thus it does not initiate a solution (e.g., a transient one)

 

Read through the help manual and the section of Transient Structural Analysis and subsection about initiating and initial conditions.

 

Basically one needs to have two steps - first step where the initiation/initial conditions are established (no dynamic effects are considered thus using no time integration in first step), and then the other one (2nd step with dynamic effects) that continues from that state with the transient analysis. Typically in structure analysis gravity only is applied in that first step, and then any other transient loads are applied after that in the second step.

Below is an image of a cantilever beam that has gravity (1st step going up to 1 s), and then after 1 s a gradually increasing transient force is applied as can be seen in the second step.

See the help manual for more info

  • Liked by
  • peteroznewman
  • sma4t
peteroznewman posted this 23 April 2019

jj77 is correct that the Static Structural to pre-stress a MSUP transient does not cause any initial stress or deformation.

I read the online help as jj77 suggested and learned that a 3 step Transient solution is probably the best option.

For a simple example, say the static load is standard earth gravity (9.8 m/s^2) which causes a displacement of 0.1 m.

Here is what happens in a 2 step solve.

  • Step 1 ramps the gravity load on from 0 to 0.001 s with Time Integration Off.
  • Step 2 is the beginning of the transient load, with Time Integration On, but the model has been given a 0.1/0.001 = 100 m/s initial velocity at the end of step 1.

This causes as big or bigger problem with the beginning of the transient simulation as the sudden appearance of a gravity load. The problem could be mitigated by ramping on the load over 1 second, which would take a long time to compute, but the model would still have a 0.1 m/s initial velocity at the beginning of step 2. The 2 step solve is actually the method used to create an initial velocity in those problems where this is what is wanted.

The preferred way to accomplish an initial load with zero initial velocity is to have 3 steps.

  • Step 1 is the same as above.
  • Step 2 also has Time Integration Off and ends at 0.002 s. Since there were no changes in load from step 1 to step 2, nothing moved, which means the velocity at the end of step 2 is zero.
  • Step 3 has Time Integration On and begins with the initial deflection and stress, but with a zero velocity.

Attached is an  ANSYS 19.2 archive that shows a 3 step transient structural. The Static Structural analysis is just there for comparison and is not required for the Transient Structural to do its initial deformation.

Attached Files

  • Liked by
  • CassioEM
  • sma4t
mutianzi1 posted this 25 April 2019

Thank you for the suggestion! I will try now.

sma4t posted this 29 April 2020

mutianzi1, could you please add some relevant tags to this topic? I find the discussion very useful and I'm sure others who concern with transient analysis will find it useful, too.

Here's some suggestion for the tags: 

  • TRANSIENT 
  • WORKBENCH
    • STRUCTURAL-MECHANICS 

peteroznewman posted this 29 April 2020

I added two tags, but the discussion is already in the structural mechanics category.

  • Liked by
  • sma4t
Arj1995 posted this 22 May 2020

I have a problem of a 3D part consisting of hyperlelastic material along with metal parts. I need to find the natural frequency.I have currently used the prestress modal analysis tool. Also given non linear adaptive meshing. Still there is distorted elements and convergence. Please help.

Close