Two FEA runs and different results for the same model !!! 4

[fifo62]

Can anyone give me some input on FEA with ANSYS to fix a potential case of conflict I'm in between?

From a Contractor my Company got an equipment, a quite slender header with a complicate geometry. The Contractor is responsible both for design and construction. The equipment is intended for a very critical service. For many reasons related to the overall plant design, that it is not interesting to explain here, the same equipment has been recalculated by one other Contractor.

Now, the "original" FEA from the equipment's supplier says that practically there are no deflection (0,2 mm on a length of 3,8m) and the header remain straight under any possible design load case.

The second FEA check says something completely different: the equipment under any load case shows important deflections (up to 14mm at middle length on 3,8m) that may affect functionality and integrity.

The two FEA were carried on by ANSYS (Version 11 and version 12.1). Both run with a linear analysis. The model's geometry has been shared by the contractors, also used elements of the mesh are practically the same (they meshed independently but type and n° of elements are aligned), internal and external loads were agreed too. Error were not found both in geometry and loads application. All design and boundary condition are the same. Eventually, when they separately run the FEA the result are different: one says yes it works, the other says no!!!! Unfortunately it is not possible to have the Contractors working together (it's now a wall against wall because of different interest and contractual constraints / they both say they are right).
In general, with such geometry and loads, I expect to see a deflection, but, I'm not able to understand how it is possible to have so different figures. Somewere an error should be found and I imagine is something very fundamental in setting up for the FEA run.

I need to sort out with a conclusion on this critical equipment and not being me trained on ANSYS I would like to know if there is any specific set up for the program that may affect the behavior showing, emphasizing or hiding the displacement. I would like to propose proper question to the Contractors to investigate these aspects of their FEA.

Any advice is welcome, thanks in advance.

 

[rb1957]

contractors can lie ! it's odd that the 2nd contractor would rerun someone else's model unless the part looked obviously "not up to par".

take the second dataset to the first contractor and ask him to run it (and you witness this). take a copy of all ouptut files back to your office. ask the 2nd contractor to run the 1st contractor's file to see where the difference is ... there are many ways of tweaking a model (control cards, PARAM codes, AUTOSPC, ...).

it's a little odd that under any loadcase you get 14mm deflection, it might be worth looking into that (where is the deflection ? why is it, what's driving it ? ...)

 

[mgage]

If the boundary conditions, loads and geometry are the same in both models, then I would look at the material properties. Possibly different units or a typo?

 

[johnhors]

Isn't this why you should do a hand calculation as a sanity check?

http://www.Roshaz.com

 

[fifo62]

Thank rb1957 / Thank mgage / Thank johnhors

-The second contractor when runs the model find the worst deflection (14 mm) with the pressure only load case (other external loads seems are acting as stabilizing the body). The model looks sensible to any load variation and reacts as expected. Deflection varies case by case.
-The re-run made by the second contractor was encouraged by us in the context of the design activities completion and because the supplied equipment was looking poor and not well justified by design.
-The maximum deflection is at the middle length of the header for any load case, ( length about 3,8 m / Ø219 mm / thk 8.18 mm / Des.Pres. 44 bar(g)) (attached a sketch to show the equipment)
-Material and all other design data were checked by Contractors and found correct for both FEA run.
-Calculation by hands is very difficult, ...at least for me.
-What is driving the deflection: to me is the difference in rigidity caused by the presence of nipples (see attachment). The internal system of forces caused by the pressure will be balanced by stresses (and strain) of the body which, when axial symmetry is respected for the body than deforms symmetrically.In case of a different material distribution not respecting the axial symmetry the deformation should be in reason of the position of the neutral axis for said material distribution.The presence of the nipples it cause local stiffening that reduce deformation capability for the material surrounding the holes. Superposition of a number of local effects seems cause a global effect.
-This type of deflection (bending in horizontal plane dir.-X) can be found also by applying external loads, e.g. introducing errors in loading the model when "pressure only" and "end effects" are considered. This type of error in loading should lead to a stress distribution associated to the bending varying along whatever cylinder generatrix is chosen, far from discontinuities and neutral axis. If on the contrary the bending is associated to an internal system of forces I expect to find a constant distribution of the stress values along the same cylinder generatrix. Considering thsi above and to investigate for anomalies in loading the model, some stress linearizations in different position, along a generatrix, has been requested to the second contractor that is indicating the deflection: these stress values were found constant, so this seems enough to consider the bending purely associated to the internal pressure.
- No thermal loads are acting.

This to give you some input on the approach I used for this matter. I hope to be correct with this.
Unfortunately, from what I'm reading in your replies, to understand what is going on with the two FEA and their differences it appears more complicate than a simple switch on / off of a black box, especially if people are not cooperating. My concern is that if an important deflection will be confirmed than the interface flanges and the nozzles attachment may fail being the associated piping quite rigid and the header at the limit anyway. I have a good homework to think about for the week end.

Any other advice is welcome, thanks to all.

 

[rb1957]

so flow in through the four pipes and out distributed through the small nipples ... how much restraint (Y-direction) do the four pipes give to the header ?

 

[CharlieM80]

Re-Check the constraints on the mounting plates or ends. Is it possible one contractor has it restrained xyz on both ends, rather than xyz on one end and yz on the other? In other words, simply supported beam with a pivot at each end rather than a pivot one end and a roller on the other.

If the part is not allowed to expand axially due to applied pressure, you may be seeing it bow due to fixing the ends axially.

 

[4Pipes]

As Johnhors said, always do a manual check - a 3.7m simple beam, a 3.7m encastre beam and PD/2T before you even start.

Is the model exactly as you show? i.e. External connection only at the supports at each end with no connections to the 4 flanges on top of the header or to the nozzles.
a) Is the deflection different in the pressure case in -x
b) ditto -y? (35 mm for 6" Nozzles or 16mm if 4" nozzles?)
c) Are the deflections different in the dead weight case?

If the answer is Yes, Yes or No, No then I would look at how the ends of the nozzles and branches have been modelled. One calc might have compensating PxA or blank ends for each nozzle. The other calc with higher -x, -y might have open ends.

If your nozzles have an ID of 25mm, have been modelled open ended, with simple supports each end of the header then the -x deflection will be about 14 mm at centre span.

 

[trainguy]

Another vote here for the dead weight case - one contractor may have assumed gravity, and the other one not. Check reactions for all load cases and compare.

Another possibility - confirm that both contractors have the same nodal/ elemental averaging settings when plotting contours, etc.

Finally, I would take each model and run a simple unit load case with boundary conditions that you define. Then compare results.

tg

 

[fifo62]

Thanks for all this input. I carried on some further investigation on their basis.

I give evidence to the following hoping to be able to clarify around what is coming from you:
-One of model is bending in horizontal plane direction -X, this might be probably due to the different rigidity on one side caused by the double row of nipples. The other model, as said doesn't deflect and remain straight. Contractors don't share conclusion.
-The model is exactly as shown.
-The restraint given by the four 6"connecting pipes is very robust in all direction X,Y,Z (n°4x6" short pipes, 1.2 meters length, departing from the same pipe collector 18" / doesn't allow differential displacement in between side nozzles and central nozzles this may lead to overstress)
-Axial expansion allowed for both model(checked and found correct / contractors shared result)
-With different pressure follows different deflection in -X
-I have no data in Y direction.
-Weight considered by both.
-Saddle reaction checked and found correct both model (share result)
-End effects, compensation PxA, checked and share by Contractors

I realized it is not and easy problem in investigating FEA set up and associated details having also to face with contract constraint and not cooperating attitude form one party. (Different release of the program they say are also not allowing to transfert files and run in between workstations)
Now probably, the only possible solution, is to proceed with NDT with strain gauges on site, together with a visual inspection during the test. This should cut any uncertainties and I think that eventually will be my advice to the my company. Thanks again.

 

[Twoballcane]

I can not open files, but it seems you need to correlate to another data point. You will have to get somebody to do the hand calcs to see if one of them is at least going in the right direction. You’re just spinning your wheels till you do. If you do not understand the physics behind your analysis, your FEM is useless. GIGO.



Tobalcane
"If you avoid failure, you also avoid success."

 

[fifo62]

Thanks Twoballcane

The physics? I expect to have deflection but it is not easy to propose a model that is acceptable by all parties and on which no one at the end can says...ohh! this is not realistic.

I personally consider that a model constituted by a two halves cylinder of different thickness in order to represent the increased rigidity we have by the side of the nipples, (....this is literature not my opinion) should be a good point to theoretically establish the behaviour of a system like this. To directly take in charge the nipples and holes is impractical and I think really complicated. The model should only give an indication about the direction we are. (Figures for the specific case can't be easily determined even having agreed on this model). Well, in approaching the case with such a model and writing the few necessary equations to address the longitudinal length variations than we need to admit that the two halves model has to deflect (see attachment). Now as said the problem is that this model although in line with the second FEA is not completely accepted as representative and I don't have any better or better argument to convince that this model represents the nipples effects.

Thanks to all you again

 

[rb1957]

sorry but it looks like we're going round in circles.

you have two models of the same structure giving different results. there is something fundamentally different between the models. If you've checked a bunch of stuff that's the same for both models then, as Sherlock Holmes would have said ... "when you have eliminated the impossible, whatever remains, however improbable, must be the truth?"

reality check ... which result do yo think is right ? do you expect the pipe to deflect in a manner consistent with one of the models ?? or neither ??

 

[Twoballcane]

rb has a good point. You should check both models side by side, line by line, down to the run time. It is either something is different or one has been fudged.

Tobalcane
"If you avoid failure, you also avoid success."

 

[4Pipes]

fifo62,

Could you give some dimensions and details of the nozzles as they have been modelled - diameter, thickness, taper, etc

 

[Elabbasi]

The difference in results could be due a difference in the way the pressure is applied by both Contractors. If a constant pressure is applied on all internal surfaces of a closed volume, then there should not be any net force (summed over the whole model) in any direction regardless of the complexity of that volume.

In that case, the difference in stiffness between the two sides of the cylinder should not cause this bending type deformation reported by Contractor #2. It should just cause the weaker side to bulge out locally a little more than the stiffer side. Even if there is some bending, based on the pipe geometry and applied pressure that you provided, the displacement should never reach 14 mm (unless the pipe material is very soft which I doubt).

You however have multiple opening that causes a net force on the pipes in the -X and -Y directions even if the pressure is constant. That net force definitely causes bending - the type of deformation that Contractor 2 reports.

You should look more closely at how/where each Contractor applies the pressure. In addition you can make a simple check by summing up all reaction forces in the model in each direction. The net force vector should give you an indication of how the pressures are applied.

I hope this helps.

Nagi Elabbasi

http://www.veryst.com

 

[rb1957]

"That net force definitely causes bending" ... unless the pipe flanges support the beam ...