Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations MintJulep on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Material Model in Ansys for Elastic Perfectly Plastic Analysis 2
- Thread starter kevin314
- Start date
Generally, I agree with rb1957, but the limit load analysis you mentioned specifically requires perfect plasticity.
You should use a bi-linear elastic-plastic material model with zero tangent modulus. There are some good notes online:
There are also a bunch of threads here on various forums discussing this specific analysis:
You should use a bi-linear elastic-plastic material model with zero tangent modulus. There are some good notes online:
There are also a bunch of threads here on various forums discussing this specific analysis:
-
1
- #7
NRP99 - agreed. If there is no hardening, then the choice of a hardening algorithm is pretty much irrelevant.
I will note that even though a hardening algorithm is not specified for Elastic-Plastic Protection Against Plastic Collapse, I would recommend the multi-linear isotropic. And, the Elastic-Plastic Method for demonstrating Protection Against Failure From Cyclic Loading: Ratcheting specifically requires BKIN and EPP, but with nlgeom,on.
I will note that even though a hardening algorithm is not specified for Elastic-Plastic Protection Against Plastic Collapse, I would recommend the multi-linear isotropic. And, the Elastic-Plastic Method for demonstrating Protection Against Failure From Cyclic Loading: Ratcheting specifically requires BKIN and EPP, but with nlgeom,on.
- Thread starter
- #8
I agree I don't know your code, but limit load means stresses less than yield, right ? we have a slightly more tolerant description "no detrimental plasticity at limit".
if you have elastic-perfect_plastic material, then won't all your stresses be less than yield ?
if an elastic-perfect_plastic material sees yield, how does the FEA react ? I'd expect it would have a nervous break-down.
if the stresses are all below yield, what does it matter how stresses above yield are handled ?
another day in paradise, or is paradise one day closer ?
if you have elastic-perfect_plastic material, then won't all your stresses be less than yield ?
if an elastic-perfect_plastic material sees yield, how does the FEA react ? I'd expect it would have a nervous break-down.
if the stresses are all below yield, what does it matter how stresses above yield are handled ?
another day in paradise, or is paradise one day closer ?
- Thread starter
- #10
ok, then how does the FEM react if the stress is (or wants to be) above yield if the material is elastic-perfect_plastic?
to me elastic-perfect_plastic material has zero slope above yield strain.
another day in paradise, or is paradise one day closer ?
to me elastic-perfect_plastic material has zero slope above yield strain.
another day in paradise, or is paradise one day closer ?
- Thread starter
- #12
The stress strain curve has zero slope beyond the yield point. BPV code defines exactly what values to use for this yield point. Some of the stresses in the FEM appear to be slightly higher than the yield stress, but these resulting stresses and strains have no real physical significance. This is simply a go / no-go test. Either the model passes or it fails. This analysis for protection against plastic collapse can sometimes be easier and more straight-forward than the code's requirements for an elastic analysis.
-
1
- #14
kevin314 - you answer your question: yes.
rb1957 - thank you for your interest in the topic. In pressure vessels, there are stresses that, on a pseudo-elastic basis, would be classified as secondary and not primary. They do not lead directly to plastic collapse. Limit Theory uses an EPP model - and once stresses reach or exceed yield, the stiffness becomes identically zero. And hence the load causing the stress redistributes over a larger area. In simple geometries like cylinders or struts, indeed an ethnic analysis will provide the same answer. But not so in more complicated geometries. And Limit Load Analysis is a special type of LRFD, used extensively in structural analyses.
The theory is solid, as is the implementation. The goal is to find where the analysis fails to converge, with the last converged solution being the limit load. Adding a small non-zero slope buggers up that search for convergence failure. What you see as a flaw is actually a feature.
rb1957 - thank you for your interest in the topic. In pressure vessels, there are stresses that, on a pseudo-elastic basis, would be classified as secondary and not primary. They do not lead directly to plastic collapse. Limit Theory uses an EPP model - and once stresses reach or exceed yield, the stiffness becomes identically zero. And hence the load causing the stress redistributes over a larger area. In simple geometries like cylinders or struts, indeed an ethnic analysis will provide the same answer. But not so in more complicated geometries. And Limit Load Analysis is a special type of LRFD, used extensively in structural analyses.
The theory is solid, as is the implementation. The goal is to find where the analysis fails to converge, with the last converged solution being the limit load. Adding a small non-zero slope buggers up that search for convergence failure. What you see as a flaw is actually a feature.
rb1957
You need to understand limit load analysis to know why this method is used. I will put my imagination at work to explain this point.
Let us take an example of a cantilever beam with end load 'X'. The stresses in the cantilever are find out by elastic analysis. The average stresses in the beam are well below yield but at some concentration points stresses observed are above yield. Now you have checked the load X carrying capability strength of cantilever. You compare average stress of beam to yield stress divide by 1.5 to fix your design of dimensions of beam. Now the stresses near the concentration points are way higher or even singular than this and based on just average stress you are not convinced that beam is able to take load X. Even to find out average stress is also cumbersome and approximate near singular points or corners. Then how to check this load carrying capacity of beam if there are very high stress?
Now we use elastic perfect plastic curve for analysis. We define zero tangent modulus, yield stress as material property for this model. Then we apply 1.5*X as end load to beam. Why 1.5? Yield stress/1.5 is limiting stress for our beam as per design. We are checking our beam against the yield stress. So basically 1.5*X load means we are checking the yield load carrying capacity of beam for given designed dimensions. Analysis is run for this load and if the solution converges then the given load is less than yield load carrying capacity of beam and design is safe. And if solution is not converging then you need to alter loads and/or dimensions and/or material to check until your solution converges.
What does this mean exactly? The load is now close to yield stress load. The stresses at corners or singularity points will yield the metal and thereby permanent plastic strain will set. Now part of load is consumed to strain the metal at corners. Remaining load will now be taken by the other sections and it will also strain to some extent and there by getting the actual behavior of component material. So load will be distributed evenly in the body. After getting finite strain due to factored load, the solution stops and will return the results in terms of finite strain and stress. Mostly complete beam section is yielded and hence called plastic collapse.
Now if the load or dimensions of beam are such that beam is continuously straining under the load and follow the elastic perfect plastic curve's constant line path. This means for given load the solution is not converging because of no finite strains are calculated by FEA for given loads/dimensions. There is infinite straining of beam for given load. This means beam is experiencing overload or loads are beyond its yield load carrying capacity and we need to modify the loads or dimensions so that our solution converges means we get finite strains.
I think this is actual physics behind limit load analysis. The max stress levels for this material model obtained in the analysis should be yield stress. But in some cases due to numerical errors we get max stress slightly above the yield.
Anyone(TGS4 and other experts of forum-I request you to comment) having better thought? Please explain so that I also get better understanding of this.
You need to understand limit load analysis to know why this method is used. I will put my imagination at work to explain this point.
Let us take an example of a cantilever beam with end load 'X'. The stresses in the cantilever are find out by elastic analysis. The average stresses in the beam are well below yield but at some concentration points stresses observed are above yield. Now you have checked the load X carrying capability strength of cantilever. You compare average stress of beam to yield stress divide by 1.5 to fix your design of dimensions of beam. Now the stresses near the concentration points are way higher or even singular than this and based on just average stress you are not convinced that beam is able to take load X. Even to find out average stress is also cumbersome and approximate near singular points or corners. Then how to check this load carrying capacity of beam if there are very high stress?
Now we use elastic perfect plastic curve for analysis. We define zero tangent modulus, yield stress as material property for this model. Then we apply 1.5*X as end load to beam. Why 1.5? Yield stress/1.5 is limiting stress for our beam as per design. We are checking our beam against the yield stress. So basically 1.5*X load means we are checking the yield load carrying capacity of beam for given designed dimensions. Analysis is run for this load and if the solution converges then the given load is less than yield load carrying capacity of beam and design is safe. And if solution is not converging then you need to alter loads and/or dimensions and/or material to check until your solution converges.
What does this mean exactly? The load is now close to yield stress load. The stresses at corners or singularity points will yield the metal and thereby permanent plastic strain will set. Now part of load is consumed to strain the metal at corners. Remaining load will now be taken by the other sections and it will also strain to some extent and there by getting the actual behavior of component material. So load will be distributed evenly in the body. After getting finite strain due to factored load, the solution stops and will return the results in terms of finite strain and stress. Mostly complete beam section is yielded and hence called plastic collapse.
Now if the load or dimensions of beam are such that beam is continuously straining under the load and follow the elastic perfect plastic curve's constant line path. This means for given load the solution is not converging because of no finite strains are calculated by FEA for given loads/dimensions. There is infinite straining of beam for given load. This means beam is experiencing overload or loads are beyond its yield load carrying capacity and we need to modify the loads or dimensions so that our solution converges means we get finite strains.
I think this is actual physics behind limit load analysis. The max stress levels for this material model obtained in the analysis should be yield stress. But in some cases due to numerical errors we get max stress slightly above the yield.
Anyone(TGS4 and other experts of forum-I request you to comment) having better thought? Please explain so that I also get better understanding of this.
Hi
Interresting topic and I think there may be two different issues discussed as one.
First the method, Limit Load Analysis, you apply a load with a load factor and include a yield stress in the analysis. Nothing special with that, I would say it is common for a ultimate limit state analysis (ULS) with the safety factors on the load. If the safety factors were on the material it would be called allowable stress analysis in "my world". One thing is that the faliure seems to be defined by "no convergece". That could mean that the failure limit can be software dependant since different software packages can handle the convergence different. Perhaps there are specifics in the method regarding this. In my experience it is better to look at the deformations and se when the increase becomes "uncontrolable". But that is a side note.
In reality I would say the "convergence" is not a real failure mode but overstraining is. On the other hand, convergence issues usually give a lower limit than strain issues unless you use large deformations, a strong nonlinear solver and/or go explicit. I assume this is a small deformations method.
It is also said that you should use a perfectly plastic material, zero stiffness above yield. But how can you then get stresses above yield limit in the results? That was one question if I understood it correct?
I asked myself that same question some year ago I got a reasonable explanation from a software developer. It may be software dependant but his explanation was simple.
The solver computes the stresses at the integration points. The postprocessor (in that case) gives the stresses at the element corners. So if you have yield at one integration point and below yield at the adjoining point, the extrapolation to the corner can result in a stress above yield. It is a mathematical issue, not a physical issue.
I don't know if it helps anybody but the discussion interrested me.
Regards
Thomas
Interresting topic and I think there may be two different issues discussed as one.
First the method, Limit Load Analysis, you apply a load with a load factor and include a yield stress in the analysis. Nothing special with that, I would say it is common for a ultimate limit state analysis (ULS) with the safety factors on the load. If the safety factors were on the material it would be called allowable stress analysis in "my world". One thing is that the faliure seems to be defined by "no convergece". That could mean that the failure limit can be software dependant since different software packages can handle the convergence different. Perhaps there are specifics in the method regarding this. In my experience it is better to look at the deformations and se when the increase becomes "uncontrolable". But that is a side note.
In reality I would say the "convergence" is not a real failure mode but overstraining is. On the other hand, convergence issues usually give a lower limit than strain issues unless you use large deformations, a strong nonlinear solver and/or go explicit. I assume this is a small deformations method.
It is also said that you should use a perfectly plastic material, zero stiffness above yield. But how can you then get stresses above yield limit in the results? That was one question if I understood it correct?
I asked myself that same question some year ago I got a reasonable explanation from a software developer. It may be software dependant but his explanation was simple.
The solver computes the stresses at the integration points. The postprocessor (in that case) gives the stresses at the element corners. So if you have yield at one integration point and below yield at the adjoining point, the extrapolation to the corner can result in a stress above yield. It is a mathematical issue, not a physical issue.
I don't know if it helps anybody but the discussion interrested me.
Regards
Thomas
So youre just making sure that the stresses are able to redistribute enough to carry the load by using a material curve with zero tangent modulus? and conservatism is in this material model assumption?
i agree that relying on convergence or not is troublesome thing
i agree that relying on convergence or not is troublesome thing
i think that is a sort of answer ... that the stresses calculated (at integration points) are less than yield and the extrapolation to nodes could be slightly higher.
i'd expect in a model with zero slope material that if the calculated strain was higher than yield then the model would have a nervous breakdown ... and maybe that's the clue that your model fails ? because strain is really what most codes calculate. maybe you're using stress-based elements, that may work a little better.
still I can't see what the material curve above yield is giving you (since all calculated stresses should be less than yield), unless you use a failed run to tell you that things have failed ? I'd've thought the difference between the analysis stress at the integration point and the extrapolation to nodes should be small enough to neglect.
if you're saying your limit load analysis permits localised yielding (like ours does) then running the imperfect plastic material would give you the "real" answer around stress risers and let you say how the structure would react to limit load.
@NRP99, your explanation confused me. it sounded like you had a structure that passes, then you optimise it (with 1.5*limit, like our ultimate), then you rerun limit load to verify. Interesting, for us (with Aluminium structures) we'd fail this ('cause yield is less than 2/3 ultimate)
another day in paradise, or is paradise one day closer ?
i'd expect in a model with zero slope material that if the calculated strain was higher than yield then the model would have a nervous breakdown ... and maybe that's the clue that your model fails ? because strain is really what most codes calculate. maybe you're using stress-based elements, that may work a little better.
still I can't see what the material curve above yield is giving you (since all calculated stresses should be less than yield), unless you use a failed run to tell you that things have failed ? I'd've thought the difference between the analysis stress at the integration point and the extrapolation to nodes should be small enough to neglect.
if you're saying your limit load analysis permits localised yielding (like ours does) then running the imperfect plastic material would give you the "real" answer around stress risers and let you say how the structure would react to limit load.
@NRP99, your explanation confused me. it sounded like you had a structure that passes, then you optimise it (with 1.5*limit, like our ultimate), then you rerun limit load to verify. Interesting, for us (with Aluminium structures) we'd fail this ('cause yield is less than 2/3 ultimate)
another day in paradise, or is paradise one day closer ?
- Status
Similar threads
- Question