I haven’t found documentation regarding connections between shells which have different thickness and also much more advanced shape than presented in you tube especially T joint or Beam which is consist of shell walls and top and bottom flanges all as shells (box section). How to create in Search Contact Pairs tool connection with " incompatibilie mesh " - T joint between shells also I need to know how to create tie constraint between solids is also node to node compatible mesh required ?
best regards
Hello Michal, I don’t know much about incompatible mesh connections, but in SolidWorks Help they point that:
Bonded contact is achieved only with constraint equations.
Unfortunately, I didn’t find anything about it in CCX documentation, but the same approach should probably be made. Maybe the contact algorithm already considers incompatible mesh? If possible, I would use “compound geometry” on PrePoMax to achieve compatible mesh and decrease the number of potential problems.
The Search Contact Pairs tool works also in less standard cases so give it a try with your models and check the pairs it suggests. Tie constraint is also really versatile and it’s commonly used to connect incompatible meshes, also consisting of elements with different degrees of freedom (e.g. connecting shells with solids or shells with beams). However, in some cases tied contact might be better: PrePoMax (CalculiX FEA) - Tutorial 15 - Shell-to-solid connection - YouTube
There’s a chapter about handling of shells in various cases (including so called knots) in CalculiX’s manual.
I just followed along with Tutorial 15. It appears that in v1.3.4 both methods of connection shown in the tutorial give virtually the same results. Is this correct? If this is the case, is it valid to use either of the methods for shell to solid connections?
prefer tied contact instead of constraint or using offset due to displacement compatibility reasons of connected surface part…
tied use contact algorithm and it seems the best approach to connecting beam, shell (expanded) and solid or mixed element…
also, it’s a good news latest versions does not triggered NLGEOM to activated by default.
Is the stress distribution also the same ? Are you sure that you defined everything in the same way as in the tutorial ? I don’t think that CalculiX was improved in this regard since the time the video was recorded. Moreover, even in Abaqus there can be differences like that when tie constraint is used instead of the advised shell-to-solid coupling.
not mandatory, you may also reading the same question & answer in CalculiX forum.
i did not found any validation documents, can Abaqus connect properly of varying or incompatible section types ? e.g pipe section (shell element) with solid circular (solid element) subjected to any loading cases and plastic condition.
For shell edge to solid surface connections shell-to-solid coupling constraints give good results. For other connections, tie and coupling constraints are sufficient. You can find some tests in Abaqus verification guide, for the aforementioned constraint types. For example, tests for coupling constraints include beam-to-shell and beam-to-solid interfaces.
this is verification not validation i seek, verification only shown how these approach or methods works.
validation is different task, it must contains sketch of problem and target values, explaining cause of discrepancy and notes in limitation of the methods itself.
This article may also be useful for reference: https://www.fidelisfea.com/post/tie-vs-shell-to-solid-coupling-in-abaqus-what-is-the-difference-and-which-should-you-use
i’m only questionable the coupling features in many commercial FE available, since many researcher also given notify about it’s not properly transferring stress and displacement in compatibility manners. below an example,
CalculiX element and tied features has fulfilled the gaps, can be generalized for any cases and challenging another coupling implementation exist.
The stress distribution along the contact line varies slightly between the two methods, but the difference is not enough to be significant. I have reviewed the inp files, and I believe they are set up correctly. I have attached the inp and frd files for both connection methods. Please confirm if I have set them up correctly.
Analysis-1 used tie connection, and Analysis-2 used tied contact.
Tutorial-15.zip (7.5 MB)
It seems that it’s highly sensitive to the selection of master and slave surfaces. Shell edge should be the master region and solid surface should be the slave region.
still merge nodes is required to avoid duplicate node coordinates and connecting by tie constraint.
this can be eliminate another problems i.e when using shell element and penalty contact exist at there due to expansion and knot generates
Thank you for the feedback. I didn’t pay any attention to assignment of the master and slave. If I remember correctly, I just went with the assignments given when using the contact search function in PrePoMax. (Although I may have mistakenly switched the assignments.) I will more carefully check master and slave assignments from now on.
I reviewed the inp files I previously attached and found that the edge actually was assigned as the master. However I found the following in the Calculix 2.19 Manual.
Based on this information, I will use a Contact connection when dealing with shell elements.
I do not have access to Abaqus, but I suspect it may not handle TIE connections exactly the same.
Thank you for development of PrePoMax and creation of the very helpful tutorials. I am enjoying not dealing with the opaque world of the commercial FEA software we were using. Transparency of the inner workings is very helpful.
manual can be use as references for general cases, may slightly differs in actually. it left the user to verify and validate the model independently.
Yeah, CalculiX’s documentation mentions this serious limitation of tie constraint but in practice you don’t have to worry about this since it works really well with all these types of elements 
In Abaqus tie constraint is even more versatile and very useful for connections between different types of elements.
right, CalculiX shell element will be expanded to solid by the solver internally, so an expanded surface based on edge definition was properly generates.
this way of working also similar to beam element, yes i can confirm by my past experiences it can be tied with shell element also…