Large deformation: ABAQUS Standard or Explicit? 1

[pjuneja]

I am trying to simulate the effect of gravity on an object (breast). The breast under-goes large deformations because of gravity, the pendulum length of breast almost doubles between the positions am interested in.

Initially I used static, general analysis and I got error "Error in job Job-1: Time increment required is less than the minimum specified".

Then I used to explicit analysis and I got result i.e. deformed breast which looks sensible. But it leaves me with a question whether my analysis is valid or not. Attached is plot for IE and KE, the KE/IE is not in the recommended range of 1-5% for most part of the analysis. In this curve I dont understand is why is the energy profile oscillating.

To understand the difference between standard and explicit, I drew and meshed a hemisphere and assigned it properties of breast tissue and applied gravity to it using standard and explicit analysis separately. Between the two analysis, I found that the deformation are quite similar though there is difference in the magnitude of deformation by about 5-20%. In explicit analysis again KE & IE had oscillating profile and the KE was not in the 1-5% of IE.

Any comments and guidance would be very helpful.

Thanks
Prab

 

[pjuneja]

Just a small additional information on my post, for explicit analysis I used the default settings in the ABAQUS CAE.

 

[IceBreakerSours]

Error in job Job-1: Time increment required is less than the minimum specified.

That is a symptom; not the cause. You must find out the reason behind non-convergence.

Then I used to explicit analysis

Not a good reason to use explicit analysis. I believe static or visco should be sufficient for this problem (unless impacts of some sort are involved.) In explicit, equilibrium is not enforced, which may explain the difference in displacements.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[MechIrl]

I agree with the above. Based on the description of your model you should be using Standard. Check your units and boundary conditions (make sure there are no unconstrained rigid body motions).

 

[pjuneja]

I agree with you, I have tried to find the reason behind it but couldnt figure it out in long time.

Attach is inp file for the standard analysis.

 

[IceBreakerSours]

I agree with MechIrl's suggestion. Check (and then double-check!) your units (dimensions <=> loads). And that includes the values for the neo Hookean material.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[pjuneja]

Units I am using are Length=mm; density =Tonne/mm3; neo-hookean coefficent = MPa ; acceleration due to gravity = mm/s2;

 

[IceBreakerSours]

Its the amplitude definition. You want the entire gravitational load applied immediately and keep it constant afterwards, which explains why the static solver went berserk and the explicit worked. If you let the loads ramp up in the default manner (which, to me, seems appropriate for the problem anyway), the model converges just fine. By the way, you do not need short increments as 1e-7 for the model to converge (particularly when linear elastic materials, no contact, general static steps are involved.)

And also, you might want to consider viscoelastic properties and the visco step for this problem, unless final equilibrium states are of interest to you.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[pjuneja]

Hi, Thanks it works as you say with default load ramping up.

I am interested in the final equlibrium state only.

Thank you again!