Output Results Stresses 1

[Boghi1990]

Hi,

I have run a structural analysis to investigate the Circumferential, Radial & Axial Stresses in a pipe wall. In the stresses output results, there are listed several types of stresses(Von Mises Stresss, Principal Stresses and Tensor Stresses). Which of these do I need to look for in order to get the circumferential, radial and axial stresses?

Any suggestion or advice would be appreciated.

Regards,

One Point

 

[burningDiesel]

No offence, but if you are asking this question, your entire solution is probably wrong anyway. Hand over the problem to someone who at least knows something about mechanics.
But to answer your question, you need the stress tensor (s11 , s22, ...) at the local orientation (so you need a cylindrical transformation). Circumferential stress is usually max principal for general cases.

 

[Boghi1990]

Cheers,

Since you have been very helpful & thoughtful answering to my question, I want to ask you a few more "dumb" questions.

Why you need to up the model with a cylindrical co-ord system, in order to investigate the hoop and radial stresses? What about Von Mises stress? Is it a cylindrical coordinate system required to investigate the Von Mises stress?

I would appreciate any suggestion.

Thank you,

One Point

 

[rb1957]

a thick skin is sometimes necessary ...

i ask you, in what direction is the von Mises "stress" ? radial ? circumferential ?? neither ??

FEA give you results in the element axes. if these are aligned to the direction of interest then you can extract the numbers you want.

i suspect that your model uses solid elements, yes? if you model was shell elements then you could set up the elments with fore-thought to get the results you want.

these questions are Very basic ... are you sure you aren't a student ?? ... 'cause as we know "student posting" is not allowed.

Quando Omni Flunkus Moritati

 

[trainguy]

I usually snicker (or block my ears) when someone starts a sentence with "no offence" because the next comments are pretty much guaranteed to offend...approximately 100% of the time. And that was a conservative estimate.

tg

 

[IceBreakerSours]

Fair criticism can play a motivating role, if one wants to learn.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Boghi1990]

Hi rb1957 ,

I am not a student. I know that Von Mises Stresses are not related to any direction. Last time I worked on a FEA stress analysis was about 6 years ago. Since then I have been involved only with a few FEA heat transfer analyses and hydraulic analyses in my job.

I looking to investigate if the thermal stresses caused by the temperature load are OK for the material and thickness of these steam piping. The temperature load was determined from a previous transient heat transfer analysis. The physical domain of this FEA analysis is a straight run of pipe a bend and Wye fitting. I started first with a straight pipe to get an idea of the thermal stresses. I am using 3D solid elements(brick) and the same mesh for both the heat transfer analysis and structural analysis. The only load assigned in the structural model is the thermal load.

I need to determine the appropiate restraints/constraints, so the model is both statically stable and realistic(not over constrained). I know that 3D solid elements do not have rotations. I have constrained one end of the pipe in axial direction only( nodal constraint) and at the end of the pipe I applied a vertical constraint(nodal constraint), to prevent the pipe going down. I am not sure if these restraints are enough to prevent rigid body motion, and also if they realistically simulate the system? Attached is a print screen of the FEA structural model I have set up.

Regards,

One Point

 

[rb1957]

1) i assume most of your cross-section is lagging material (it looks very thick). if so, is this effective in carrying load ?

2) i'd've used shell elements for the pipe (so i could align the element directions). using solids, you'll need to create a cylindrical co-ord system to extract the stresses you want; consult your user manual.

3) i don't think you've constrained rigid body motion. i think you've got a bunch of axial (lets call it x-direction) constraints which'll take out three degrees of freedom. (test, which ones ?) and your vertical constraint will take out another; leaving two unconstrained. (hint, what about lateral forces ?)

4) if you'd explained your situation more fully i think you'd've gotten less "commentary"; your last post suggests you're less of a student and more of a lapsed "worker".

Quando Omni Flunkus Moritati

 

[EngAddict]

Discretisation errors could lead to the model being unstable, plus your restraints are not symmetrical, so I like to restrain the three DOF. If it suits your analysis you may choose to use springs in some directions to prevent over-stiffening your model. However most software should produce suitable results if these resultant forces are quite small.

 

[EngAddict]

Continued..

Not sure if your restraints reflect your actual model but I assume two nodal restraints don't. Also, for the last few releases of Algor you don't have to have the same mesh in your thermal and static analysis, so as required you can add mesh refinement in your areas of high stress.

Try and run the analysis, if it does not solve then it is unrestrained. Check your displacements though. If your piping is also pressurised then you will need to apply the internal pressure and pressure thrust, so to resist your thrust you would want to restrain the end face in the axial direction. If you only have the thermal gradients through the thickness then select three points, one in each direction, and it should work fine. If you are after restrained free end expansion then it will be harder to accurately analyse with this simplified model.

 

[Boghi1990]

Hi EngAddict,

What does it mean "select three points, one in each direction.."?

What does it mean " If you are after restrained free end expansion.."?

When I apply the restraints, is it better to select surfaces or nodes?

Regards,

One Point

 

[EngAddict]

I mean the minimum would be 3 nodes, one for each translational DOF. i.e. select one node to retrain your x-translation, another node for your y-translation, etc.

In piping systems that experience thermal expansion where the end of the pipe is restrained from freely displacing, such as at a shoe or a vessel, you get displacement limited thermal stresses. They are displacement limited because small displacements at these restraints, usually through local yielding, relieve the stress and are therefore self-limiting in nature. However to accurately model the system you would need to include your full piping and the end conditions.

Node restraints (at least in Algor) will disappear after you re-mesh so are a pain to use if you are using an iterative process. You will also get infinite stress at this restraint since you have a singularity at this location. But if you are not interested in the stress at this point it may be perfectly acceptable. Realistically you wont have infinite stiffness over zero area so it doesn't accurately capture your real model anyway. Probably a surface or an edge would usually be better but for contact cases in linear analysis you may need to run a few iterations to make sure you don't overly restrain the model.

 

[TERIO]

Assuming this is related to your thread Thermal Stress Analysis Constraints then you have already done the system level stress analysis with restrained free end expansion (in CAESAR II).

What criteria are you using to evaluated the acceptability of the stresses you calculate?

 

[rb1957]

"the minimum would be 3 nodes, one for each translational DOF. i.e. select one node to retrain your x-translation, another node for your y-translation, etc." ... this won't restrain the 6 degrees of rigid body motion.

"When I apply the restraints, is it better to select surfaces or nodes?" ... you need to be very carefull constraining surfaces; it's very easy to over-constrain the surface and introduce spurious reactions.

Quando Omni Flunkus Moritati

 

[Boghi1990]

EngAddict,

I have defined a cylindrical coordinate system. I then assigned the local coordinate system to nodes at one end of the model. I have applied nodal constraints (Tx =0, Ty=0, Tz=0) to prevent the rigid body motion of the model. I am not sure though if these constraints are properly simulating the boundaries of the model.

I have attached here the print screen results for some of the results. I am using Von Mises Yield Criterion.

The Von Mises stress and displacement magnitude seem quite small. Is that because of the way I have assigned the constraints?

 

[rb1957]

to nit pick, you don't have x,y,z freedoms in a cylindrical system, but r,theta,z.

i'd fully constrained the face axially (x?) and constrained one node in y and z and another (diametrically opposite) in z.

how much elongation did you expect ? (ie hand calc ?)

Quando Omni Flunkus Moritati

 

[Boghi1990]

rb1957,

In my previous analysis one of the physical properties(Young Modulus of Elasticity) was wrongly defined. It was 28 lbf/in^2 instead of 28*10^6 lbs/in^2. I have corrected that input and I have changed a bit the restraints. I have constrained 6 nodes on one end of the model for Tx=0, Ty=0 and Tz=0. In the software I am using (Autodesk Mechanical Simulation) these constraints are shown as Tx, Ty and TZ. A cylindrical coordinate system is assigned to these constraints. Attached are some print screens of the nalysis aresults.

The stress results (Von Mises Stresses)are highers in the vecinity of these restraints. I am still not sure though if these nodal constraints I have applied are realistic and if they prevent body rigid motion.

Any suggestions to what values I need to check the Von Mises Stresses? Do I need to compare Von Mises stresses against Min Yield Strength or to Maximum Allawable Stress for this low allow steel material(A335 P22)?

 

[TERIO]

The constraints do not look right. The real pipe can grow radially. See the comments by corus in the other thread for some advice on constraints. The constraints do prevent rigid body motion (since the pipe didn't fly off the screen). Also, I'm guessing your temperature distribution is axisymmetric in which case a 2-D axisymmetric model often makes life a little simpler.

What size pipe and what length of pipe are you modeling? What is the temperature distribution through the pipe wall thickness? It's hard to have an idea if your stress is reasonable without it.

As a check, for a cylindrical shell with a linear temperature gradient, ΔT, the axial stress at the surfaces should be EαΔT/(2(1-ν)). If your distribution is not linear the this will be somewhat different (if you linearize the stresses it should be close).

Some notes on what to compare to:
- These stresses are at least somewhat additive to your expansion stresses from the piping analysis and should probably not just be considered alone.
- If you look at a current vessel code (say Section VIII, Div 2, Table 5.6) it will tell you that for a radial temperature gradient the equivalent linear stress distribution is secondary stress, while the nonlinear portion is peak stress. Secondary stresses are generally limited to twice yield while peak stresses are evaluated for fatigue.
- In nuclear piping (NB-3600) stresses due to thermal gradients are only included in the peak stress check (i.e., the linear part is not considered secondary like in vessels). There is a separate check on the linear part to prevent ratcheting.

 

[rb1957]

"The constraints do not look right. The real pipe can grow radially." ... exactly, you are over constraining the pipe. pls read my post on 11 july 16:13. you have too many y- and z- constraints. your x- constraints react Fx and My and Mz rigid body motions y- and z- constraints react Fy, Fz and Mz. for this you need 3 (only) constraints ... 1 in y- and z- to react the forces and another in either y- or z- placed to react Mz (ie if you choose a 2nd y- it should be offset in z from the other y- constraint).

clear as mud ?

Quando Omni Flunkus Moritati

 

[Boghi1990]

TERIO,

One pipe is 12 inch (thickness 2.4375 inch), and the other pipe is 18 inch (thickness 3.7 inch). As I have mentioned before, I am analysing now only a stright section of the pipes (500 mm) to investigate the distribution of the stresses in the pipe walls. The full model will include two bends and a Wye fitting and 500 mm pipe sections at each end.

Attached is a print screen of temperature profile in the 12 inch straight run of pipe taken at the last time step of the transient thermal model.