Uneven stress levels around a cone

davefo · October 2018

See the attached image and file. Does anyone know why the stress around the cylinder varies. I expected a near constant value. How do i get a more constant peak stress ring?

Victor · October 2018

I think it's because the surface there is faceted with flat 6 element wide facets, rather than being curved.

There are sometimes also cases where shells have these kinds of alternating stresses and you may have to ignore those localized regions or average them.

davefo · October 2018

I thought it might be that so i tried to use smooth but than moves the nodes alone the cone surface instead of keeping them on the same horizontal plane.
Is there anyway to force smooth to keep the Y co-ordinate and smooth the X and Z

davefo · October 2018

see attached where i hoped to be able to generate a better curve fitting mesh, by creating an iges file. why is each part of the iges being meshed seperately with very little nodes in common. How do i get it to mesh properly with each part joined where they touch?

Also note the local axes for RSA components. How Do i get these to be correct i.e. either U or V radial.

davefo · October 2018

How do you do the averaging?

Victor · October 2018

Separate surfaces is a problem that happens with IGES files. It's better to use STEP format instead.

To set the element axes so U is the radial direction, make another element orientation in Loads & Constraints with these values:
X: x
Y: 0
Z: z

davefo · October 2018

i'm getting really confused now. i've got the iges to mesh and repaired the cracks. Then i've run the analysis with the same load and constraints but get different von mises stress.
Then when i find the max stress point and refine it the value just increases every time i refine it further. What am i doing wrong?, see attached

Also see attached screen capture showing max a

nd min. How ca the save point be both?

Victor · October 2018

Ever increasing stress with refinement indicates an infinite stress concentration. For stress at the connections between shell elements, you could use a solid mesh with the correct details of the geometry and radii, or some other technique like a code or hand calculations - possibly using forces obtained from the FEA model.

Find Max/min only looks within the current selection, so ensure nothing is selected before using it. This feature is useful to exclude uninteresting stress concentrations.

davefo · October 2018

A bit over my head, I don't know much about fea. Do you mean I should redo the whole model as solids?

disla · October 2018

Hi davefo

I’m getting soft Von Misses result.
Check the deformed view of your result to see if it has sense. If it blows to hell or goes out of your axis center your BC are probably wrong and Stresses are nonsense.
It is not mandatory but preferably build a conformal mesh between shell and stiffener. The easiest way is to draw a 2D section and revolve it.

If your stiffener is not a supporting element I would suggest you to re-orient it. Think it as a beam. The reinforcing material is recommended to be as far to the vessel shell as possible to increase second moment of inertia.
Keep also in mind that in order to be effective the stiffened area should be at a “small” distance from the weakest areas (cone transition).

Victor · October 2018

It depends what you want. If you're trying to find the maximum stress anywhere simply by using FEA, then you'll need to model the joints with their details like weld fillets, fasteners, and internal corner radius on angle sections since those details can have a big effect on maximum stress. That requires solid elements because of the complicated geometry and stress field.

But in reality, there are probably localized high stresses you don't care about and don't need to model accurately because they won't lead to failure, or that you can calculate some other way. Those decisions about what to ignore are more engineering than FEA.

davefo · October 2018

for clarification, what i am trying to find out for the client is at what internal pressure the model experiences permanent deformation. The mid level ring angle is not only intended to be a stiffener it is there as the main vertical support the top and bottom angles and the vertical plate are for connection of individual pieces as well a stiffening. The client has stated that 5mm deformation would be classed as unacceptable deformation. I have assummed that permanent deformation would occur when the stress level exceeds yield i.e 275N/mm², but I am unsure when and where this happens. Is it when any element stress reaches 275 or when a node stress reaches 275, or it it more correct to assume permanent deformation only occurs when both sides of the plate thickness reach 275 at the nodes on the outer face, ie both tension and compression stresses are at yield
I have tried created a solid model, see attached. And think it is at the yield point, when permanent deformation would occur, although the deflection is much lower than 5mm.

Victor · October 2018

At mesh convergence, the node and element stresses will be the same. Any difference is error in one or both. Usually, the node stresses are more accurate because they're a smoothed version of the element stresses, which eliminates discontinuities that are usually not realistic.

von Mises stress exceeding yield at any location will mean permanent deformation as long as the material follows the von Mises yield criterion. But maybe your client has a more practical definition of "permanent deformation" that excludes some unimportant one?

Now that it's solids, you really need to use quadratic elements (hex20, wedge15, etc). Linear solid elements in Mecway are poor at bending and some components of their stress are constant through their thickness which means you would need many elements in the thickness direction to capture differences between one side of the plate and the other. So quadratic elements are much more efficient in terms of mesh density.

The maximum stress in this model is very close to or at the connection between the angle support and the cone so you definitely need to refine the mesh in that region until it doesn't change, but there are also stress singularities there (what I earlier called infinite stress concentrations), so you have to ignore those and look at the values some fixed (not reducing with mesh refinement) distance away from them.

davefo · October 2018

Thanks yes i thought the critical stress level appeared to be at the joint between the cone and the mid angle support, I struggling to fine a way to refine the mesh in that region and expand the mesh away from it where it doesn't need to be as small as it currently is. Any suggestions.

The clients doesn't have any other definition of the permanent deformation. He just needs to give a value to his buyer.

Victor · October 2018

If you made the 2D section with Automesh 2D, you can add a local refinement in there which is located at a specified node number.

If it's from a flat STEP or IGES file, that's a bit easier. Right click a node and choose New local refinement which makes a sphere of refined elements next time you generate the mesh.

Regardless of how the mesh was made, you can select the elements to refine and use Mesh tools -> Refine x2 but it makes some not very well shaped transition elements and you can't turn it off later.

davefo · October 2018

I refined the mesh a couple of times and the stresses appeared to converge but also increase. I found the max point and refines x2 a few times and now the stress values just keep increasing again but are still not converging.I give up this is impossible!

Victor · October 2018

Sorry for the frustrating experience. Ever increasing stress there is normal behavior and with that fine mesh, you probably have good results elsewhere. It's at a sharp re-entrant corner which is a stress singularity so it's theoretically infinite. You have to ignore these stresses because they're a consequence of not modelling the geometry of the joint accurately - the real structure won't have perfectly sharp corners like the model does.

If you still have the persistence, you can switch to nonlinear analysis and define a plastic material so you can see if the inevitable yielding that occurs in this pathological case of a perfectly sharp corner is self limiting or if it leads to large scale deformation.

Sergio · October 2018

Just one tip, use three second order element in thikness, lineal elements can underestimate the deformation for sheet metal parts. Your part is very regular, can be easily meshed as a revolution mesh.

disla · October 2018

Hello davefo,

Don’t underestimate what you got. You problem is not trivial at all.
I dare you to find a code which analytically solves the transition between a skirt and a cone with the supporting line "in the cone" itself.
It is not by chance that 99.99 % of the supports for vessels are located in the cylindrical area or at least, transition area.
Google some images of “silo skirt support” and check how many of them have the skirt resting in the middle of the cone as yours. Your skirt is very special.
Also, the cone has a half apex angle of 30º which is the limit in where most codes feel comfortable.

The FEM is giving you good information from my point of view . You have a dangerous closed ring of peaks stress through all the thickness on a thin shell that in my opinion will hardly be able to redistribute stresses to other areas allowing a safe path (maybe with a belt).

Do not feel frustrated and don’t be discourage, peak stresses are “the daily bread” in FEM.

davefo · October 2018

Thanks to all of you for he encouragement and advise, I am a qualified Chartered Structural Engineer here in England, so am used to design of structures, but have zero experience of Finite element analysis. The client is a local fabrication company that makes these vessels and has no idea how to provide the answer his buyer asked for so came to me. He is aware that this is new to us also, So I am trying to help him out.

I think i'll leave the mesh as it without further refinement and reduce the pressure load. since the deflection is no where near the 5mm limit I'll also run it with increasing pressure until i get 5mm deflection then advise him on the theoretic yield pressure limit and theoretic deflection limit pressure.

I'll try remeshing surface with 3 element through the thickness and revolve again

DaveStupple · October 2018

Hi davefo, stick with it, there's a lot of knowledge on this forum, and plenty of patience. Take a look at the following as a nice example of increasing stress in a sharp corner with mesh refinement:

https://mecway.com/forum/discussion/362/mesh-convergence/p1

Here's the text link, in case that one does not work:

https://mecway.com/forum/discussion/362/mesh-convergence/p1

davefo · October 2018

I'm also looking at getting a reference book on fea. since i would likely only use fea for structural type problems. Do you have any recommendations on what to buy

davefo · October 2018

Victor
I tried Non linear static and get some errors, I.e. bonded contact and member orientation
What do i need to change these to to get it to analyse?

DaveStupple · October 2018

Dave, have you tried selecting CCX solver in the Analysis branch? Both types of constraint become available in the menus.

davefo · October 2018

never used ccx so dont know what i'm doing with it, tried it but get the following warnings and no results

*INFO reading *STEP: nonlinear geometric
effects are turned on

*WARNING reading *STATIC: a nonlinear analysis is requested
but no time increment nor step is specified
the defaults (1,1) are used

STEP 1

Static analysis was selected

Nonlinear material laws are taken into account

Newton-Raphson iterative procedure is active

Nonlinear geometric effects are taken into account

*INFO in gentiedmpc:
failed nodes (if any) are stored in file
WarnNodeMissTiedContact.nam
This file can be loaded into
an active cgx-session by typing
read WarnNodeMissTiedContact.nam inp

*WARNING in gentiedmpc:
DOF 3 of node 14 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 15 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 2 of node 16 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 16 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 19 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 20 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 23 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 24 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 25 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 33 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 34 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 3 of node 35 is not active;
no tied constraint is generated
*WARNING in gentiedmpc: no tied MPC
generated for node 90087
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90088
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90175
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90389
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90390
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90429
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90541
master face too far away
distance: 9.5216759056826472E-005
tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90656
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90658
master face too far away
distance: 1.0484692903400816E-004
tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 90988
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 91071
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 91453
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 91459
no corresponding master face
found; tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 91583
master face too far away
distance: 1.0454032460183171E-004
tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 92061
master face too far away
distance: 1.0412599186349070E-004
tolerance: 9.4836489698703799E-005
*WARNING in gentiedmpc: no tied MPC
generated for node 92228
master face too far away
distance: 1.0166276223055881E-004
tolerance: 9.4836489698703799E-005
Decascading the MPC's

*INFO in cascade: linear MPCs and
nonlinear MPCs depend on each other
common node: 92290 in direction 2

*ERROR in cascade: zero coefficient on the
dependent side of an equation
dependent node: 14 direction: 1

DaveStupple · October 2018

OK, that didn't help. CCX can be very daunting, but if you are lucky Mecway takes care of everything and it all gets done behind the scenes. The first couple of warnings might be addressed by selecting Quasi-static and then put in a duration and time step. Each step I think is solved as non-linear static following on from the last, so you end up with a sequence of solutions. Some of the other warnings about tied and face too far away might need you to select TIE or Elastic in the Bonded Contact dialogue. This post might help. Sorry I don't have definitive answers for you, you might have to wait for Victor

disla · October 2018

Could you post the file? Previously clean the solution for lighter file.

Sergio · October 2018

Have checked the step, is a very bad quality shape probably created from a stl then converted to step (due to the big faceted triangled faces). In my opinion will be better to recreate the geometry in the cad because is a simple cilinder, than trying to mesh as is now.

Regards

Victor · October 2018

Don't use the internal solver for nonlinear. It's inferior to CCX in just about every way.

*INFO and *WARNING messages are often normal and harmless. These ones look OK.

*ERROR is what makes it fail. This one looks like it might be the same problem as the "incompatible constraints" message that the internal solver gives on bonded contact and displacement on the same nodes. If it's solid elements, check node 14 to see if it is. If it's shell elements, the node number might not match the input model. With CCX, you may be able to avoid it more easily by selecting the Elastic option in bonded contact and entering a high stiffness value.

davefo · October 2018

Sergio
? main step file used is only the profile shape of the cone and angles that i have then meshed and revolved. two other step files are the stiffeners which have been surface meshed then extruded 5mm.

Victor
tried elastic instead of tied changed bolts material from circular to rectangular bar, changed rsa material to rectangular bar, changed isotropic material to plastic material with yield of 275 mpa sectant modulus of 0.5% of E, ticked quasistatic with time of 1s step of 0.5s
it takes about 60 iterations to solve, but stiffeners aren't connected and there are no stress results only deflection s and external force. whats this?

disla
files attached.

Victor · October 2018

No stress usually means it didn't converge.

The stiffener comes away because the stiffness of the bonded contact joint is too low. I changed it to 1000 GPa/m and it stays pretty close.

I also changed the pressure load from constant to ramped by replacing "92.6" with "92.6*t". That not only makes it easier to converge, but if it fails, you can sometimes see successful solutions before the failure and get an idea of what went wrong. It now only takes 6 iterations.

Mecway

Forum

Uneven stress levels around a cone

Comments

Howdy, Stranger!