Need advice getting either Standard/Explicit to converge
Need advice getting either Standard/Explicit to converge
(OP)
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!





RE: Need advice getting either Standard/Explicit to converge
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
RE: Need advice getting either Standard/Explicit to converge
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!!
RE: Need advice getting either Standard/Explicit to converge
RE: Need advice getting either Standard/Explicit to converge
RE: Need advice getting either Standard/Explicit to converge
Forever Young.....
RE: Need advice getting either Standard/Explicit to converge
RE: Need advice getting either Standard/Explicit to converge
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.....
RE: Need advice getting either Standard/Explicit to converge
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
RE: Need advice getting either Standard/Explicit to converge
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!
RE: Need advice getting either Standard/Explicit to converge
Rob Stupplebeen
RE: Need advice getting either Standard/Explicit to converge
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?
RE: Need advice getting either Standard/Explicit to converge
Rob Stupplebeen
RE: Need advice getting either Standard/Explicit to converge
RE: Need advice getting either Standard/Explicit to converge
Rob Stupplebeen
RE: Need advice getting either Standard/Explicit to converge
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.