Hi,

Increase the time period in step then introduce the amplitude base on it.

Hi,

Increase the time period in step then introduce the amplitude base on it.

HI Emad

How are you?

the time period is 0.1 and the amplitude is already introduced

Should I increase the time period more than that?

This is a quasi static problem. Hence the time period T should be estimated from the first natural frequency f of the object. It should be T >= 1/f. For your object I guess T=0.1 is long enough. You need to check other inputs (speed of punch, etc.) to fix the error.

Hi Nguyen

I estimated the time period from the natural frequency and introduced amplitude according to that.

I coudnt figure out the error

here is the input file of the explicit one

According to my experience, to get results compatible with the quasi static analysis, the time period should be larger than the time needed for P (and possibly S) waves to travel along your whole model and return back. I was faced with similar problem when modeling different geophysical tasks.

Dear Ayad

To have a quasi static problem using Explicit solver, you need to pay attention to the Kinetic to internal energies ratio which should not be more than 10%. it means you can  have a stable solution like standard solver if and only if the above ratio is dealt. then you can give whatever time period you desire and any Mass scaling or velocity you want as long as you have that ratio driven.

you can plot the internal and kinetic energies in one single plot using the data created in the History output after simulation and look if the solution is stable. 

I personally think that your attached solution is not stable enough.

best wishes 

You are using linear reduced-integration elements. Please check your hourglass controls and check for hourglassing in general (see the getting started manual on how to do this). Did you by chance use fully integrated elements in standard? That would easily explain the higher stiffness.

Hi Ayad,

From the Fig. of the explicit simulation, I think speed of the punch was too large (left side of the plate was bent and the contact was unsymmetrical). You should check the movement of punch.

I had a look in your model and saw:

- Besides mass scaling factor 9, you increase material density 1000 times. This help to reduce time step (mass scaling), but as Shahram said, you need to assure that when increasing density the kinetic energy must be smaller than (5-7)% of strain energy.

- You use explicit to simulate stamping (step PM0) and spring back (step PM1). The "time period" for PM0 should be 0.1, not 10. After stamping and during springback you may need to damp the dynamic effects to assure a quasi static solution.

- Contact of the plate with tools should be activated in PM1.

- The Output interval should be larger, if you want to see a smoother process of deformation.

Good luck!

Thanks guys for your reply

Shahram and N. Huynh

your comments helped me to understand many things and I think I am on the right truck

However, I got one more problem. During the analysis I always get this ERROR "Excessive rotation of nodes in node set ErrNodeExcessRotation-Step1."

What does it mean?

I tried to refine the mesh and still got the same problem

Dear ayad

pay attention to the BCs you have used. Maybe there is a fault BC in that node or maybe there is two different Bc in that node where they contradict with each other. Also look at the purpose of using that node too. Maybe you can do that  in other  ways.

I think it  is  because  of Bc contradiction.

I faced similar problem. I am working my thesis on composite structure which is subjected to monotonic loading. I want to use abaqus/explicit step. but I couldn't get the exact tabular amplitude data with out considering dynamic effect.

can anyone help me please?