Need advice getting either Standard/Explicit to converge 1

[bues0022]

I am having some troubles with my model and am hoping that someone on here can lend some advice. I am attempting to model a balloon-expansion of tissue. My model consists of a 1/4 geometry "donut" of material. The ID (initial incision point) is 5mm, thickness=5mm. I want to expand out at 30 PSI. The outside edge of this slice of tissue is at 100mm. Using ABAQUS standard I am having a very hard time achieving convergence when I get closer than 2-orders of magnitude away from 30 PSI. Using Explicit, I am getting an oscillation that shows waves of stress moving through the material like ripples in a pond. Also, when I get close to the 30 PSI for my input load in Explicit, I am getting "excessively distorted elements", how do I fix this? I suppose this is similar in nature to a metal forming technique, only I'm prescribing a pressure rather than a force, and I am using a hyperelastic material model. I'm relatively new to using the programs, so perhaps I'm missing something? Any help would be great!

 

[rstupplebeen]

Can you post your file?

What strain are you achieving in standard? Evaluate you material model and see if it accurately predicts out that far.

In explicit try applying the pressure slower (ramp over a longer step size). Explicit is sensitive to noise and chatter. Assuming you can get it relatively low you can filter your results so that the animation is prettier but be careful because a heavy filter will turn your results to garbage or hide the fact that the results are garbage.

I hope this helps.

Rob Stupplebeen

 

[bues0022]

My material model is a stress/strain data set that has been pull-tested to breakage. I do not see strain levels past my material model.

I haven't yet tried using adaptive meshing in Standard, is that something that might help convergence with a higher load?

I ran another model in Explicit yesterday with a much lower mass scaling. The model took a VERY long time to run, and achieved similar oscillatory results as before. I'll try posting up my files. One will hopefully be my Standard model I've been working with, the other will hopefully be my Explicit model. I am trying to eventually get my load up to 200,000 Pa. I'm only at 20,000Pa right now.

In the mean time, I'll try changing how I apply the pressure, to see if that changes anything. Thanks for any help!!

 

[bues0022]

This is the ABAQUS Standard model I am working with.

 

[bues0022]

This is the ABAQUS Explicit model I am working with.

 

[williwang]

did you use adaptive meshing?

Forever Young.....

 

[bues0022]

I tried using adaptive meshing with the Explicit solver, but ran into errors with element selection. I am trying to also find out what element I should use with hyperelastic materials, AND adaptive meshing. Any thoughts?

 

[williwang]

I am not sure it is good to use Explicit or not.

Rstupplebeen is right. For explicit, you need to smooth your load.

For adaptive meshing, I guess you have to use implicit. But I am not very sure. I will check it out later.

Forever Young.....

 

[rstupplebeen]

I looked at your model and here is a list of suggestions.
1. Your material model is throwing an error due to incompressability Ogden3 looks like a decent choice.
2. This could be an axisymmetric analysis (washer applying pressure to the center)
3. You are fixing the outside of the washer and have 2 symmetry planes. I believe that the fixing of the outside is nonphysical. Constrain 1 point in the Z then possibly the outside radially.
4. I believe that the default elements should work for this.

I hope this helps.


Rob Stupplebeen

 

[bues0022]

1) I didn't know that even if I put in the stress/strain data for a hypelastuc material that I still needed to choose a model type and input the coefficients. I'll take a look at it. Also, I specified density, but not Poisson's ratio, explicit says it input a standard one for me. This seems odd. Should I find a more accurate poisson's ratio?

2it is axisymmetric, but I don't know how to do that. I'll check on that.

3) I'll also try this.

4) thanks!

 

[rstupplebeen]

In the property module go to material->Evaluate to see Abaqus's suggestions for the material model. Pick the lowest order one that looks reasonable.

Rob Stupplebeen

 

[bues0022]

I was away from internet access over the weekend, so here's an update:

I am getting results! Ramping the load from 0 to full over the entire time period. This is helping reduce "rippling" of pressure waves. I am using adaptive meshing, it seems to be helping because I no longer get errors of excessive distortion. I haven't tried new material models (see below) or other BC's. I'll check on those after I get a full complete simulation.

With regards to material models:
I had done that, but apparently those results didn't transfer in the file. I re-evaluated the material, and the Marlow model is by far the closest (actually right now because it's just reproducing the data). I have selected the Marlow model to use. Is this not an accurate way to do things?

When I am using the Marlow model with hyperelasticity and Explicit, it wants a Poisson's ratio and density. I input a density, but shouldn't the Marlow model account for the Poisson's ratio?

Now, however, I can only run about 84% of the process before I get errors that I have too many iterations. What would be the cause of this?

 

[rstupplebeen]

I believe that you would need volumetric compression data for the Marlow model to predict compressibility. You only have simple tension and compression data.

Rob Stupplebeen

 

[bues0022]

Alright, so I've made all the changes that were suggested, and I still can't get my model to comlete at 30Psi. My model makes it to 87%, then fails. Why? I get an error that says my material is unstable, does that have something to do with it? I'm confused since this isn't that complex of a model. In fact, after this comdel is complete, I'll need to add more features - including some contact features. Thoughts?

 

[rstupplebeen]

Tech support might be the most appropriate course of action. They are the most helpful in the industry. If you can't or are too stubborn to do that try running with slightly different: meshes, material models, boundary conditions then submit all of the jobs and come back when they are done. A DOE sort of black box methodology turning the dials quite often will find a numerically stable sweet spot. Just remember as always to validate your results. I hope this helps.


Rob Stupplebeen

 

[bues0022]

I think I may have figured out my problem. I kept getting errors and the simulation would quit at about 85%. I tried the maximum pressure of 150,000 Pa instead of 200,000 - and the simulation completed without any problem. 0.15Mpa is 75% of .2Mpa which is less than the 85% where the model used to fail. I believe this is because I was getting strain values which were higher than what my material model was able to predict. When the strain values went above my data points the simulation quit because it didn't know what to do. Does this seem like a plausible explanation? What do I do next to my material model to allow it to finish? Do I put one point straight horizontal (same stress value but much higher strain) from the last point? Then I can identify where this value is and see by how much my model fails. I seem to remember something about a failure criterion in ABAQUS Explicit. How does this work?

I think I'm finally on the right track with this, now I need a little direction on where to go from here with the failure modes and analysis.