Abaqus Standard: Overconstraint + Negative Eigenvalues 1

[looyongabaqus]

hi, i am using Abaqus standard to model a reinforced beam-column connection subjected to a tip load at the end of the beam.

i first applied a gravity load followed by a tip load at the end of the beam. halfway through the application of the tip load, abaqus standard stop and give 2 errors.
1) overstraint at certain nodes of my longitudinal reinforcement
2) negative eigen values

i did research on this and some pple are saying that the problem might be insufficient number of boundary conditions (in the right places) to prevent rigid body motion under the action of the applied forces. i checked and change some of my boundary conditions but the same error occurs. the deflection of the end of the tip of the beam when Abaqus stop is still very small and it should not be that the force applied is too great.

i hope someone can offer me advice. appreciate it, thank you.

rgds,
joseph

 

[rstupplebeen]

Could you post an image of your boundary conditions?

Rob Stupplebeen

 

[looyongabaqus]

hi,

i have attached an image of my boundary conditions in pdf. however, i have solve the problem of overconstraint. Abaqus standard will not allow embedded nodes to be tied by surface-based tie. my reinforcement are embedded elements within the concrete structure and my concrete structures are made up of different parts surface-tied together. I have since redid my concrete structures.

however, my negative eignevalues still remain.

i have did 3 different models with the following different conditions.

1) (Coarse Mesh)0.1m; NLgeom Off; 10 increments at 0.1sec each: Abaqus Standard completes analysis with 0.4mm deflection at tip of beam.

2) (Fine Mesh)0.025m: NLgeom Off; 10 increments at 0.1sec each: Abaqus Standard stops running with Negative Eigenvalues errors and Numerical Singularity warnings.

3) (Coarse Mesh)0.1m: NLgeom On; 10 increments at 0.1sec each: Abaqus Standard stops running with Negative Eigenvalues errors and Numerical Singularity warnings.

i) I am not sure why with a finer mesh (compare 2 to 1), the program stops running.
ii) I have material non-linearity and so i think NLgeom should be on. But the errors starts to occur when I switch NLgeom on.

As I cannot post more than 1 attachment with this reply, I have only attached the diagram of the boundary conditions.

I really appreciate you writing in. I hope you can offer me advice on the above too. Thank you.

Best Regards,
joseph

 

[corus]

With pinned restraints the structure can rotate, and hence you get negative eigenvalues. Use symmetry or use a 2d plane stress model.

corus

 

[rstupplebeen]

Based on your image I do not understand what is tied to what. Can you change the coloring of your model (parts, materials)?

Why would you need to tie embedded nodes? Think of tie as glue sticking 2 faces together.

I hope this helps.

Rob Stupplebeen

 

[looyongabaqus]

Hi guys, thank you for the posts. I am going to post my input file if it can help you to understand better what I am modeling.

Hi Corus,

I was thinking over your suggestion. I think symmetry might be difficult because of my loading. As for 2d plane stress model, I am not really sure how to work on that? Will it affect my material models for my concrete and steel?

I also tried to do encastre for the base of the column to the floor but it does not help.

Hi Rob,

As my connection has slightly different dimensions to my beams, so I tried to model the connection, beam and column as 3 different parts and surfaced-tie them together. When I do that and embed my reinforcement through them, I get warnings of overconstraint from Abaqus as they do not allow embedded elements to be tied by suface-tied (here my reinforcement intersect the suface-tie). So I redo my entire concrete structure as just one part and this solve the problem of overconstraint. I should have explain it clearer in my reply.

Thanks guys again for the post. Cheers!
joseph

 

[rstupplebeen]

In your assembly use Instance>Merge/Cut to join the main structure and the 2 pads. Now you do not need the TIE constraints.

Try to run the model without the stiffeners first then add them back.

Change your step size to variable. These are my usual settings I start with however my usual application is very different.

*Step, name="beam loading", nlgeom=YES, inc=10000
beam loading
*Static
0.01, 1., 1e-08, .1

This may be a better starting point for you
*Step, name="beam loading", nlgeom=YES, inc=1000
beam loading
*Static
0.1, 1., 1e-05, 1.

Rob Stupplebeen

 

[looyongabaqus]

Hi Rob,

1) I tried to to use Instance>Merge/Cut but could not comprehend how to do it. Abaqus will prompt you for a new part and after that you will need to select all the instance to be join together. After this, there is only one new instance containing the entire structure. All the other instances are gone. I am having problem with this because I need to mesh the reinforcement and the concrete separately as they are different elements. In the end, I did not do this step.

2) I tried both running the model with and without the reinforcement (stiffeners). And I tried inc=10000 and inc=1000.
With reinforcement, I get the same results as before.
Without reinforcement, the program ran and stopped at about 0.403sec into the beam loading phase.

I tried a few different increments but get the same results as above. Please see my pdf for screenshots of the results.

Thanks for replying.

 

[rstupplebeen]

If you choose to keep the edges the body boundaries will still be there. I think for your case I had to merge the meshes.

Do you have nonlinear geometry on?

Rob Stupplebeen

 

[looyongabaqus]

hi rob, i had the nonlinear geometry on. im trying to work on my boundary conditions. not too sure if it will help. i will let u know if i am able to get something. thanks.

 

[looyongabaqus]

hi rob,

I tried to use the following for my loading steps:
Static General> Automatic Stabilization> Use damping factors from previous general step> Use adaptive stabilization with max. ratio of stabilization to strain energy to strain energy: 0.05

I think this works in solving the diverging, numerical singularity issues as it introducing a damping to the model.

However, the results that I got from the modeling is only about 5% of the actual test results. So it is kind of strange.

I am thinking if i did something wrong somewhere in my model.

Rgds,
Joseph

 

[rstupplebeen]

Occasionally if I get too far ahead of my self in the complexity of a model I restart. Create a new model and only add 1 level of complexity at a time. I usually start with what I envision will be the most difficult part (contact, damage, nonlinear materials). I hope that helps.

Rob Stupplebeen