Surface vs. element loading

[cgbridges]

Hey all --

To give a very brief background - I'm attempting to model a fracture by first finding the stresses in certain elements, then making a second file without those elements defined. In the second file, the neighboring elements have an applied stress equal to that held by the removed elements. My plan is to release that stress, creating the fracture.

Since I'm using shell elements, it seemed best to use edge loading. I've figured that I should use either *DSLOAD with EDNOR, or *DLOAD with EDNORn, but am having probelms figuring out the difference between element loading versus surface loading.

Unfortunately, trying each method has not resulted in success - one returns answers that make no sense; the other returns answers that work fine for a small model but blow up in a large one. [Also, the best I can find in the ABAQUS manual is that the n in EDNORn is the direction of load (such as global 2 or whatever), but I wasn't sure if that was right.]

Can anyone explain the difference to me, or give a reason why it might not be working? Sorry to have so many questions wrapped up in one.

 

[xerf]

Your approach seems complicated to me.

I understand that you want to replace a removed (failed) element by an equivalent stress distribution on the edges of the neighbouring elements. I do not think obtaining the equivalent stress distribution is trivial.

The stress tensor for an element is computed at integration points. And you basically need to convert the stress values at the integration points into tractions applied on the edges of the neighbouring elements.
I think it should be simpler to convert the stresses in the failed element into nodal forces.

But...
1. how abaout if you have several connected elements failing simultaneously ?
2. do you evaluate the failure criterion at the end of the loading path? what if they fail at 0.5*maximum load ?

Probably, it can be even simpler if you could use the built-in ABAQUS capabilities such as the "element removal" described in
ABAQUS Analysis User's Manual -> "19.2.3 Damage evolution and element removal for ductile metals"

 

[Yoman228]

You may want to try this, model the fracture as there is a long crack in it already. Then use beam element to hold them together. The beam element simulated the bonding of the material before it crack, then remove one beam at a time in each step to simulate the cracking.

 

[xerf]

...or you can use cohesive elements.

 

[Yoman228]

I heard rumor that cohesive elements does not work too well for details crack analysis from the people who is specializing in modeling crack. But I could be wrong as it was just a rumor and I did not do any validation.

 

[cgbridges]

My previous method was to use *MODEL CHANGE to remove the elements; however, I could never get the model to converge after about half the elements were gone (I reduced the initial time step to 0.00001, I believe).

The idea with applying the edge loads was that I took the stresses at integration points 1 and 5, averaged them, multiplied by the thickness of the plate, and applied them back on. I tried it with a simple model and got agreement on the order of 0.1%.

To get the actual fracture event, I would then reduce the loads slowly or quickly, all at once or individually, depending on what I wanted to look at / what seems to represent the actual event best. Also, using loads rather than *model change was supposed to allow me to either run it under *dynamic or *static (*model change doesn't seem to respond dynamically).

I've also looked a bit at *failure strain (I think; I'm doing this from memory) and I think the things you mention, xerf (*damage initiation, maybe?).

Yoman, at one point I was considering using springs between the nodes. I started with them having a very high k, just to see if it would run with them in place, with the intention of making them inelastic somehow at the time when I want the fracture to occur, but I couldn't get convergence then, even with no load on the springs. I could try beams, however; springs are just so much less computationally expensive.

I'm willing to try other things to model the fracture; my main concern is time and ease of modeling - the model runs around 2 hours right now; we have one that uses fracture elements that takes more like a week, which doesn't meet our goals.

Thanks for the ideas!