Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Appropriate failure model for beam elements and LAW36 material?

Hello everyone,

I may be in need of a failure model in conjunction with either P3 or P18 beam elements and a LAW36 tabulated plastic material. The material is a plastic to the likes of polyamide, or something more ductile like a tough resin. The built-in failure method of LAW2 or LAW36 cannot be used as, according to the documentation, the total strain is not calculated in beam elements, which is necessary for the failure model. Can someone help figure out which failure model is appropriate for this kind of application? My knowledge about them is unfortunately very limited, and almost all failure models mention only solid and shell compatibility, with some stating nothing of the sort, which leaves the question of beam compatibility open. A very simple "element is deleted or disconnected above x strain or y stress" behaviour would be sufficient.

Find more posts tagged with

English

HyperMesh

Radioss

v2021.0

Accepted answers

PaulAltair

Hi, if you want to use LAW36, then only BEAM type18 is compatible, none of the /FAIL failure models are compatible with beam elements, this is stated in the failure models compatibility table, the in built failure in LAW36 should work with Beam type 18 though I think, I did a quick test and got failure...

All comments

PaulAltair

Hi, if you want to use LAW36, then only BEAM type18 is compatible, none of the /FAIL failure models are compatible with beam elements, this is stated in the failure models compatibility table, the in built failure in LAW36 should work with Beam type 18 though I think, I did a quick test and got failure...

Very simple example, but these Type18 beams inserted in crush cans, shown here, stress/strain plotted in green, failure occurs where expected

Ingeniorator

Hi, if you want to use LAW36, then only BEAM type18 is compatible, none of the /FAIL failure models are compatible with beam elements, this is stated in the failure models compatibility table, the in built failure in LAW36 should work with Beam type 18 though I think, I did a quick test and got failure...

That's very interesting, thanks for pointing it out. I think the reason why this behaviour did not show up in my previous models might be the way stresses and strains are calculated in the elements and reported in Hyperview. For example, in my lattice model in compression, there's complete layer collapse and von Mises stress is reported to be higher than 300MPa in the beam elements, whereas plastic strains don't even reach 0.1%. X stresses are between +200MPa and -150MPa, while the max stress in the stress-strain curve is approx. 120MPa.

I tested the behaviour a bit, here's an example of a 1mm diameter beam in bending. The von Mises stress reaches 64MPa, but only 0.55% plastic strain, whereas the failure strain was defined to be 0.1% in the LAW36 definition. Still, here the first element on the left failed prematurely and was deleted.

On the other hand, with the same model in tension, the last element fails upon reaching the failure strain defined via the stress-strain curve (0MPa stress at 3% strain). Again, the values of the contour plot differ a lot from the query in Hypergraph. How come?

PaulAltair

What combination of EpsPmax, EpsT and EpsM are you using on the LAW36? (EpsPmax is effective in any direction, whereas T and M are tensile only)

Can you share your tensile/bending test models? I might be able to diagnose your question more easily, to me the curve and animation look not so different? Are you showing your eroded elements there? element 1 is still visible despite you saying it was eroded? Remember in Animation you are only getting the output at snapshots in time, so typically, you won't ever see the maximum plastic strain if the element is deleted (as it will have been deleted 'between' animation states)

Ingeniorator

What combination of EpsPmax, EpsT and EpsM are you using on the LAW36? (EpsPmax is effective in any direction, whereas T and M are tensile only)

Can you share your tensile/bending test models? I might be able to diagnose your question more easily, to me the curve and animation look not so different? Are you showing your eroded elements there? element 1 is still visible despite you saying it was eroded? Remember in Animation you are only getting the output at snapshots in time, so typically, you won't ever see the maximum plastic strain if the element is deleted (as it will have been deleted 'between' animation states)

Thank you for your help. I have attached both files. Remember that both use different values for failure strain, it was done just to see what happens.

The first picture does not show the state in the last animation step, but one before. At this point, the leftmost element was not yet been eroded.

beamFailTest2_0000.rad

beamFailTestBend_0000.rad

PaulAltair

Thank you for your help. I have attached both files. Remember that both use different values for failure strain, it was done just to see what happens.

The first picture does not show the state in the last animation step, but one before. At this point, the leftmost element was not yet been eroded.

Ok, the failure method you had adopted in the bending model is the correct one (set EpsPmax on the LAW36) you shouldn't set the stress/strain curve negative slope (back to zero) as you had in the tensile one. Attached I have modified your models a little (fixing a small timestep and increasing output), there is an .mvw session file there too, to load the results in. For Bending, you need to look at the individual integration points plastic strain for it to make sense (as the averaged is nil due to being on the neutral axis), I set the failure low enough that you see a break now in one of the models in bending.

Beam_Failures_110322.zip

Ingeniorator

Ok, the failure method you had adopted in the bending model is the correct one (set EpsPmax on the LAW36) you shouldn't set the stress/strain curve negative slope (back to zero) as you had in the tensile one. Attached I have modified your models a little (fixing a small timestep and increasing output), there is an .mvw session file there too, to load the results in. For Bending, you need to look at the individual integration points plastic strain for it to make sense (as the averaged is nil due to being on the neutral axis), I set the failure low enough that you see a break now in one of the models in bending.

Thanks again for your insight, it's incredibly helpful!

So regarding Eps_p_max, should it take precedence over Epsilon_F for element failure? I was a bit confused by the graph below, as it suggested to me that Epsilon_F would be the ultimate measure of element erosion. The second comment on the doc page, however, is clearer in its functionality. Consequently, it looks like it would be correct to not provide EPS_t and EPS_m values to ignore the stress reduction portion and go straight to element deletion, correct?

As for the negative stress-strain-slope, it was mentioned in comment 1 of the doc page: If the last point of the first (static) function equals 0 in stress, default value of $ε_{p}^{m a x}$ is set to the corresponding value of $ε_{p}$ . So I tried that to see what happens with this setting. Why do you think this setting is incorrect?

Do you know the numbering order of the integration points per cross section? I did not find details on it, only the image below which is not very clear, in my opinion.

For the larger models I'm working on, the third beam node is defined by a single orientation node for all beam elements, with the node being either at the origin (0, 0, 0) or very far away, out of convenience. Since they are all oriented differently, it's not possible to provide orientations that coincide nicely with the global coordinate system. This does make it difficult to judge where each integration point is situated at for each element (i.e. is point i near the neutral axis, the side in tension, in compression, somewhere inbetween?), so it looks like their position is only distinguishable via their relative stress values.

Edit: I encountered an odd error in another beam model where the time step jumped to 1e+06 seconds in the very first step and the simulation subsequently finishes, which is very odd. This happened with CST_0 as well as CST_2, with a calculated minimum time step of approx. 4.2e-7s. Would you happen to know what could cause this?

Edit 2: I have got some more problems with this model, and I can't figure it out for the life of me. It's attached to the reply. It's a compressive test of a lattice for verification of the failure model of LAW36. It runs fine enough with P3 beams and LAW1 linear elastic material (until it hits the energy error limit as it runs with AMS and a 0.05s time step to speed the full model with P18 and Law36 up), but P18 beams and LAW36 does not. No matter if the concerned layer is compressed via an imposed velocity on all layer nodes or a rigid wall, only the first layer moves (as it should) but no other elements are affected? With an RBE2 fixed BC on the bottom and RBE2 spider on top with an imposed velocity will not start at all. No idea what's happening...

verification.hm