Isochronous stress strain curves instead of direct creep analysis

[M.hmk]

Is it possible to use Isochronous stress strain curves instead of direct creep analysis(with a creep material model) to analyze systems that operate in creep range?

I want to obtain the amount of strains for a system which operate in creep range after 10000 hrs.
Therefore I want to perform static non-linear analysis with use of Isochronous stress-strain curve related to 10000 hrs as material model. Is it right?

Thanks in advance.

 

[mskds545]

Isochronous stress-strain curves are a great tool in the right situation. You will generally get pretty good agreement between an isochronous stress-strain curve model and a time-explicit model if your creep law follows a simple von mises flow relationship between strain rate and equivalent stress, you aren't incuding any kind of damage model, your loads are proportional and monotonic, and your temperatures are uniform and constant. You might be able to handle some more complicated multiaxiality okay if you write your own flow rule for the plastic analysis.

You should run a few simple geometries with isochronous curves and the equivalent time-explicit model to get a feel for when they do well and when they don't. If you keep the element count low, you can do this pretty quickly. Koves and Zhao wrote a series of papers 10-odd years ago where they did this, and they also develop a technique for handling non-proportional loading with isochronous curves. Also check out Marriott's 2011 paper "Isochronous Stress/Strain Curves -- Origins, Scope and Applications." He says "Firstly, it should be stated that the isochronous curve approach is wrong" and then spends 7 pages discussing how useful they are. Also read his book with Penny, which covers reference stress methods extensively. Get the 2nd edition, which is heavily updated.

One thing to keep in mind with creep is that there is always a more detailed model and never enough data. You can get widely varying answers using different published approaches and data for geometry and loading that vary only slightly from those they were developed with. The best data is operating experience, so adhere to well established design rules whenever possible.

-mskds545 at gmail dot com

 

[M.hmk]

@mskds95
Many thanks for your response.
Did you ever use the method mentioned in para. 10B.5 of ASME FFS-1 2016 to obtain Isochronous curves? Is it a good solution?
In this method, I have problem with Δcd (adjustment factor for creep ductility) and also with
Δsr (adjustment factor for creep strain rate). the first one must be in a range of +0.3 and -0.3 (based on brittle or ductility behavior) and the second one in a range of -0.5 to +0.5.

my main problem is that the results are completely dependent to these factors and with a little change in the amount of the factors, the creep strain changes a lot.I don't know what the amount of these coefficients should be.

The comments will be appreciated.
Thank you.

 

[TGS4]

It could be anywhere in that range, and so most creep analyses work to bracket the solution with the range of those coefficients. As mskds545 eloquently put it, you can indeed get widely varying answers.

It is likely that if you need something better than that, then you need to be doing your own Omega testing on the subject steels.

 

[mskds545]

Yes, I have used that method, and I have learned a lot about the expected behavior of components by using it. So, in that respect, I have found it to be a useful method. But always keep in mind that you're really just looking at shadows on the wall of the cave (true of any engineering analysis, but triply so in the creep range) and creep really is that stochastic. The codes use large design margins in the creep range for a reason. Consider how critical your component is. Make the component more robust if you can so that you're certain it will work. If at all possible, include controls beyond mechanical design margins to protect personnel if it is safety critical. And, if there are no other options and you can't convince yourself it is okay, run some creep tests on the actual material like TGS4 suggested. Make sure you have somebody involved with sufficient expertise to understand the effects of test acceleration, and the actual geometry and loading conditions.

-mskds545

 

[M.hmk]

Many thanks for the comments. So let me tell you my problem in detail.

In one of our projects, there is a piping system which operates in creep range. These are the characteristics:

Design Temp. = 675 C // Design pressure = 3900 Kpa // Material = A312 TP321H // Pipe OD = 34” (thickness=71 mm) & 24”(thickness = 50 mm) //

Unfortunately after only 3 weeks operation, major cracks revealed in most of the girth welds and this caused the system to shutdown. Our material specialist believes that it could be because of low quality of welding procedures and also high amount of pipe wall thickness causes the welding procedure is unsure and insecure. Therefore he recommends reducing the pipe size and wall thickness by considering the process conditions to improve the welding procedures.

Besides the concerns that our material specialist mentions, I believe that these cracks could be because of high amount of inelastic strains considering both plasticity and creep responses. I discussed this with my manager and he agreed to I work on it. After that, I started to read a lot of papers regarding this subject and also about elastic follow-up caused by plasticity and creep. After reading these papers, I concluded that best method to evaluate the degree of elastic follow-up and also the amount of the strains is FEA to simulate inelastic response of the system and it is possible by using of isochronous curves. Because isochronous curves include both plastic and creep strains. Therefore I started to find a resource to find a suitable isochronous curve related to the material and temperature of this piping system and I found out that there is a method in Para.10B.5 of ASME FFS-1 2016. When I wanted to use it, I faced the problems that I mentioned in my previous post and I decided to start this thread. Now, I want to have your recommendations.

Do you think if evaluation the amount of strains is a solution to predict the location of cracks?

Is there any acceptable magnitude that the maximum strains shall not exceed? (For both weld and base material areas)

Based on MPC project omega creep method I found the required factors A0 to A4 and B0 to B4 related to mentioned material referring to table 10B.1 of ASME FFS-1 2016. But I need your suggestions of amount of Δcd and Δsr based on what I described.

Also I have attached an excel sheet about creep strain calculation based on MPC project omega creep method . The amounts of A0 to A4 and B0 to B4 have been determined in Mpa for type 321H material.

Your comments will be appreciated.

 

[r6155]

1)If the problem is in the weld, then think about the welding procedure. Forget calculations.
2)Also think in A-376 instead of A-312
3)Relaxation cracking can occur in P-No. 8 materials not only in cold-formed areas but also in welds where highlevel
residual tensile stress exists. PWHT may be advisable to avoid relaxation cracking.

Regards

 

[mskds545]

First, I agree with r6155 and your material specialist that it is probably the welds. You would need some seriously bad elastic follow-up to cause a creep rupture failure in 3 weeks. That said, isochronous stress-strain curves are a good tool for investigating elastic follow-up, but the omega model is based on low stress levels near the ASME allowable stress (see API 579 Table 10B.1 Note 2) so it isn't the best model for investigating quasi-sustaining thermal stresses that are much higher than that. You can try it and see what it predicts, but remember that you're extrapolating into a range where the creep behavior will be very different. At higher stress levels, you'd expect more secondary creep. You can probably find steady state creep rates in data sheets or text books and fit them to a Norton-Bailey law to generate alternative isochronous curves. Don't expect it to be overly accurate -- just use it to understand the behavior, and do a broad sensitivity study. I wouldn't focus on the strains (except for comparison to the elastic strains to see if you have much elastic follow-up occurring). Ductility exhaustion is tricky with stress relaxation because the ductility is so sensitive to strain rate, and there's never any data available. I'd probably use creep-rupture data with a life fraction summation, considering some weld strength reduction factor as well. Compare it to a similar relaxation problem without the follow-up. That should give you some idea about how much the follow-up could have contributed to the reduced life, if at all.

-mskds545

 

[M.hmk]

@r6155
You are probably right. But there are a lot of papers which show how elastic follow up caused by creep condition causes severe cracks. Therefore I think it is reasonable to investigate the system based on this aspect.
@mskds545
As you recommended I started to use Omega-model to see what it predicts, although I understand what you mentioned about low accuracy of this model at high stress levels. I will definitely use other methods (such as Norton-Bailey) as well. To start, I decided to be conservative and therefore I used minimum properties (lower scatter band) with 100000 hours. I determined Δsr equal to -0.5 and Δcd equal to 0.
Based on the initial elastic analysis, the stresses were on the elastic range. Therefore for creep analysis, I decided to use simpler elastic-creep omega model instead of elastic-plastic-creep model. So this is my material model: €(t) = σ/E – ([ln(1- Ωἐt)]/ Ω)
I also have attached the excel sheet of calculated inelastic strains. As you see I selected 8 Mpa as a specific yield point to use in FEA since the inelastic creep strain is approximately zero at this stress level. (Although the yield point of A312 TP321H at 675 C is 96.6 Mpa).
It will be appreciated if you check the excel file and give me your comments.

 

[r6155]

I always objected to solving manufacturing problems with calculation procedures.
The problem is in the lack of quality control at the manufacturer.
The first thing that fails is the visual inspection.
I was always present in all the processes of retests, when the original test fails
Typical errors: orientation of test specimens, transfer of marks, storage of electrodes, humidity in bevels, difference between PQR and production welds, etc….etc.

Regards

 

[M.hmk]

Following on from the previous post:
Apart from material considerations, I also want to have your comments about my analysis method.
Indeed, I did the initial elastic analysis through CAESARII software. You can see the piping system in the attached figure. Based on this analysis, all of the stresses are in the allowed limit determined by B31.3 code. However as I mentioned before, major cracks revealed in most of the girth welds, after 3 weeks.
One of the locations of these cracks is near the elbow that I have shown in the attached figures.
The elastic analysis done by CAESARII indicates that the highest code stress in operating condition (weight + Pressure + Temperature) is at this elbow.
Therefore I decided to perform FE creep analysis for the mentioned elbow, using Abaqus software. Indeed I extract the boundary conditions (B.C) of both ends of this elbow with help of caesarII and then implement them in my Abaqus model. I have modeled the elbow with 2 straight pipes attached to the both ends of elbow. You can see the model in the attached figures. I also used C3D20R elements and 3 elements thru the thickness.
But I am not certain that what kind of B.Cs I should use? Force or Displacement?? And also I do not know how I should use them in abaqus?
These are the extracted boundary conditions from CaesarII analysis for both ends of attached straight pipes:

Displacement type B.C:
End A: Dx=63mm / Dy=65mm / Dz = 460 mm / Rx=0.1284(Deg.) / Ry=-0.6417(Deg.)/Rz=-0.0419(Deg.)
End B: Dx=87.2mm / Dy=34mm / Dz = 481 mm / Rx=0.0241(Deg.) / Ry=-0.3746(Deg.)/Rz=-0.129(Deg.)

Force type B.C:
End A: Fx=38169(N) / Fy=56862(N) / Fz = -48629 (N)/ Mx=288613(N.m) / My=-443384(N.m) / Mz=253780(N.m)
End B: Fx=-38169(N) / Fy=-28855(N) / Fz = 48629 (N)/ Mx=-180930(N.m) / My=551068(N.m) / Mz=-60767(N.m)

Imagine you want to apply these BCs in your abaqus model. How do you do this?
For example for force type: Do you apply the extracted forces on both ends of your Abaqus model? Or
Do you fix the end A(B) and then apply the end B(A) extracted forces on the other end ?
These questions are also applicable to the Displacement BC type if you want to use this type.
Do you apply the extracted displacements on both ends of your Abaqus model? Or Do you fix the end A(B) and then apply the relative displacements to the end B(A) ?

Thank you for your comments.

 

[mskds545]

I'm not sure how you evaluate elastic follow-up by modeling a single elbow. Elastic follow-up is an interaction between the elastic piping and the elbow where you believe the creep strain is accumulating. If you treat it as a force, you're assuming essentially infinite elastic follow-up is occurring. If you treat it as a displacement, you're assuming no elastic follow-up is occurring. Real elastic follow-up is in between. You need to model the whole thing. Sorry, but I can't help you with the detailed calculations or check your spreadsheets for accuracy.

-mskds545

 

[M.hmk]

@mskds545

You are right. With help of this method (applying force boundary condition) I am able to obtain very conservative upper bounds of inelastic strains and as you mentioned the real strains are lower and need the behavior of the entire structural system.
But modeling of such a complex piping system in Abaqus, is time consuming or maybe impossible.
Do you think there is another solution to obtain accurate strains?

 

[r6155]

Can you send us some photos of craks?

Regards

 

[M.hmk]

@r6155
Our company is currently closed because of corona virus and I don't have access to the information. I will send as soon as possible

 

[r6155]

Good luck to all of you.

Regards

 

[mskds545]

I don't know what your abaqus model of just the elbow adds here. If you're going to just assume that the thermal stress doesn't relax at all in the elbow, can't you just take your caesar results and compare them to a larson-miller curve? It seems unlikely that fully-sustaining thermal stresses would be acceptable. If they are, that would rule out elastic follow-up as a potential contributor. But if you want to investigate whether or not follow-up is occurring, you're going to need to model more of the system. Why use continuum elements? Why not pipe elements?

-mskds545

 

[M.hmk]

Do you mean to use continuum elements for the elbow and pipe elements for other parts of the system and then to connect continuum and pipe elements to each other?? I don't know if it is possible in Abaqus. Please advise me.

Also I think the elastic follow-up always occurs and with help of inelastic analysis and by including the whole of the system, the accurate degree of that could be obtained. The severe condition is when there is not any relaxation (reduction in load) and I agree with you, it rarely happens. But even if this is the case, the inelastic strains can still be in allowable range that can be evaluated maybe with para. 5.3.3 of SEC.8 Div-2 Part 5.

Your comments will be appreciated.

 

[mskds545]

I don't use abaqus, but I'm sure you can combine pipe and continuum elements with it. I wouldn't recommend that here, for where you are with this problem, but that's your call.

I've never seen any literature that suggests the strain limit formulation in 5.3.3 is meaningful for the evaluation of creep strains, and that is not permitted under 5.1.1.3. What are you basing this approach on?

-mskds545

 

[M.hmk]

Please take a look to PVP2014-28797
It has been mentioned on page 10.