I think solid element is not meant to be used just one layer.
This shell model has Stri65 thin shell elements. Does calculix supports this?
No, only S6. And of course, those aren’t real shells in CalculiX, but expanded ones.
In fact, sometimes it’s even a good idea to use composite shells (via keywords) with the same material to have more layers and thus more integration points across the thickness, but that’s mainly for models with plasticity.
Hi,
Interesting problem. I keep doing some tests. I have some hypothesis which I’m trying to clear one by one.
Mode shape is right so I’m first thinking:
_Abaqus element is less stiff. (That’s my first option)
S4 and S4R elements fail for me with shells. S4R is not suitable for LBA in my experience. It gives smaller Buckling factor or doesn’t give anything at all.
_Abaqus treats the triple shell connection in a different way. Less stiff. We know ccx generates Knots when the thickness between elements is different.
-I discard an error at the documentation. You reference different results for the same set up in ANSYS and Nastran.
-Is corrosion applied to the Skirt?. (You didn’t)
My result is 11 with small differences depending on the set up.
I’m also considering if Abaqus apply some inertia release to the preload step. It would have sense cause at the workshop test the anchor is not fixing the base yet and the equipment should be modeled as completely free with minimum BC to avoid rigid body.
Anyone having some other possible source of this difference please comment.
NOTE: Just as a curiosity. 147 KPa gives BF 7.42. Maybe there is some conversion factor or units missunderstunding. I have not discarded it yet known there are Snail Slungs involved.
Hello,
Thank you for looking into this as well. I did not apply corrosion to the skirt as I do not believe that would cause a significant difference and typically in terms of pressure vessel design that is targeted at the process side.
See this link to another forum where this was discussed some years ago. This has a couple of different solutions: one from Ansys as well as another user used MSC Nastran.
The sketch is clear there. Can read the dimensions. And a stp model.
I’d like to try s4r element.
No wonder, Abaqus has true shells. I wanted to try US3 in CalculiX, but it doesn’t work with buckling:
*ERROR in e_c3d_US3: no second order
calculation for this type of element
►░Sä$☻ Óf~
$☻ _US3: no second order
In Abaqus, it’s a very good, versatile element, but again - it’s a true shell formulation there so a bit hard to compare.
Not by default and inertia relief is rarely used at all in Abaqus. The screenshot from Abaqus shows BCs at the base on both translational and rotational DOFs.
Has the Abaqus solver follower force effects included into the solver. Is there a chance to deactivate them to compare.?
Abaqus has the FOLLOWER parameter for that. It’s enabled by default for distributed surface loads (apart from general surface tractions) and disabled for concentrated forces. Of course, this only applies to analyses with Nlgeom:
By definition, the line of action of a follower surface load rotates with the surface in a geometrically nonlinear analysis. This is in contrast to a nonfollower load, which always acts in a fixed global direction.
Btw. Abaqus takes preload into account even if the static step has Nlgeom disabled, but enabling it makes Abaqus use the deformed geometry from the preceding static step as the base state. Here, the static step doesn’t have Nlgeom.
It looked like every one was having so much fun with this silo I had to take a look. I took the shell of the tank, meshed that then simply extruded the skirt so the connection provided coincident nodes and then put a shell offset to try and reproduce the required geometry with no requirements for tied connections. With 16000 elements (apporx 3.6 in) I get this with S4R
and this with S8R shells
(i did the analysis in MW as that was where i found it easiest to manipulate the model into a single part)
is it possible the tie connections being used in some analysis have had an influence on the results?
But it was solved with CalculiX, not Mecway’s internal solver using improved shells, right ?
Sure, it’s better to avoid them in such cases. I’ve mentioned that at the beginning of this thread: Issues with linear buckling analysis following ASME PTB-2022 example problem - #6 by FEAnalyst
Hello, I also get around that using S4R, but when I reduce mesh size my buckling factors reduce drastically. Did yours stabilize around 8?
Also, if you ran it with MW solver vs calculix, does it yield the same results?
It cuts the buckling factor by a 10% but that doesn’t seems an option. Deformed shape on the ASME report would have shown that skirt deformation.
Hi jim - i did try with the MW internal solver (which I understands uses shells as shells) with 1.9in elements and 3.8in elements i get pretty close to 12. In fact with all the shell models i ran i got very nearly 12 with -only the S4R elements showed any difference - 8.1 with 3.8in and 2.8 with 1.9in - close to ur experiences I think. When I have time I will extrude to solid and see what I get.
That looks like a nice mesh. I am not sure why the meshes did not line up in my earlier model other than having them as parts and not as one unit.
I was able to run this model without the skirt support using the 3/2/1 constraint method and get a BF of about 9.8. So it’s the lowest I’ve gotten so far.
Need to apply -14.7 psig now.
Which tool is easy to do this? PPM or fc?