*Tie and surfaces?

[lukerickert]

Hi Everyone

I am working on a model that is primarily surfaces but has a few solid parts. I was having trouble so I read the documentation (imagine that and see that *Tie only works with solid elements. I am using PrePoMax 1.1.1 (which I think is using calculix 2.16)

Is there a work aground? (other than running it with just surfaces and combining the parts that tied and then doing a secondary analysis or submodel for just solids? It has been awhile but I seem to remember doing connecting solids and surfaces in Abaqus.

thanks

Luke

[SergioP]

Hi @lukerickert ; I was able to use TIE for gluing solids to solids, shell surfaces to shell surfaces; shell surfaces to shell edges, shell edges to solid and shell surface to solid with no problems, sometimes I has to increase the tolerance or reduce the element size to make it work.
Where I have failed was in some cases where I have a kind of sandwhich with three shells, in those cases what I do is model the middle part with solid elements (I’m using three hexa elements normally), and then I can glue the three parts as well.

Regards

[Calc_em]

Check these threads:

Is contact of beam and shell allowed in CCX?

hi, i’m modeling contact analysis of beam and shell faces, try a simple model but did not succeed. anyone has experiences, are the solver CCX allowed this analysis type? or something i miss at input decks. [CGX_beamplatebonded] bellows are input files, thank you. ** Objective : Beam to Shell Contact *NODE 1,0,0,0 2,100,0,0 3,100,100,0 4,0,100,0 5,50,25,10 6,125,50,10 *ELEMENT,TYPE=S4 1,1,2,3,4 *ELEMENT,TYPE=B31 2,5,6 *ELSET,ELSET=eplate 1 *ELSET,ELSET=ebeam 2 *SURFACE,NAME=splate 1,SPOS *SU…

Case with 2 connected plates of different materials not working

Dear all, I’m in trouble with an apparently super-silly case of two connected consecutive plates (of different material) subjected just to their weight and with an extremity which is fixed. The plates are modeled with shell elements. As you can see from the attached figures, the nodes at the plate-to-plate interface are conformal. The problem is that CCX leads to a solution that seems not to consider as attached the two plates (as you see from the super-high displacements of one of the two plat…

Tie constraint is really versatile and can be used for beam-solid, beam-shell or solid-shell connections as well. Here’s an example:

As you can see, the deflection is well represented but the stresses become distorted. The same happens in Abaqus and that’s why Abaqus offers shell-to-solid coupling functionality which eliminates this issue. Unfortunately, CalculiX doesn’t have such a constraint implemented.

[lukerickert]

Here is a super simple example, two surfaces tied on the edge loaded with gravity, the model is definently not happy

type or **
** Surfaces ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Surface, Name=Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Master, Type=Element
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Master_S2, S2
*Surface, Name=Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Slave, Type=Element
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Slave_S4, S4
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Slave_S3, S3
*Surface, Name=Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Master, Type=Element
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Master_S4, S4
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Master_S3, S3
*Surface, Name=Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Slave, Type=Element
Internal-1_Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Slave_S1, S1
**
** Physical constants ++++++++++++++++++++++++++++++++++++++
**
**
** Materials +++++++++++++++++++++++++++++++++++++++++++++++
**
*Material, Name=S185
*Density
7.8E-09
*Elastic
210000, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
**
** Sections ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Shell section, Elset=Internal_Selection-1_Shell_section-1, Material=S185, Offset=0
1
**
** Pre-tension sections ++++++++++++++++++++++++++++++++++++
**
**
** Constraints +++++++++++++++++++++++++++++++++++++++++++++
**
*Tie, Name=Shell_part-1_to_Shell_part-2-1, Position tolerance=0.05, Adjust=No
Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Slave, Internal_Selection-1_Shell_part-1_to_Shell_part-2-1_Master
*Tie, Name=Shell_part-1_to_Shell_part-2-2, Position tolerance=0.05, Adjust=No
Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Slave, Internal_Selection-1_Shell_part-1_to_Shell_part-2-2_Master
**
** Surface interactions ++++++++++++++++++++++++++++++++++++
**
**
** Contact pairs +++++++++++++++++++++++++++++++++++++++++++
**
**
** Initial conditions ++++++++++++++++++++++++++++++++++++++
**
**
** Steps +++++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Step-1 ++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Step
*Static
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
**
*Boundary, op=New
** Name: Fixed-1
*Boundary
Internal_Selection-1_Fixed-1, 1, 6, 0
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Cload, op=New
*Dload, op=New
** Name: Gravity-1
*Dload
Internal_Selection-1_Gravity-1, Grav, 999, 0, -1, 0
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
*Node file
RF, U
*El file
S, E
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
paste code here

[Calc_em]

Enable adjustment and try increasing the position tolerance. Use frequency extraction analysis for tests so that you can easily determine whether parts are properly connected or not.

[lukerickert]

I think the issue may have to do with the automatic interaction finding functionality not working properly with edges. If I define the edge tie manually it appears to work, I hadn’t noticed that the automatic function was only for surfaces and not edges as it selects both of them. I guess this functionality will improve with development.

Luke

[Calc_em]

As long as the Search Contact Pairs tool detects the surfaces/edges and creates contact pairs/tie constraints (depending on your choice), it works properly. So far, I haven’t noticed any limitations in this detection, it works even in cases where equivalent tool in Abaqus can’t help. If constraints are created by this tool but don’t work properly in the analysis then it’s not a fault of the tool but likely effect of wrong setup or limitation of the constraint (rather unlikely). The tool automatically applies some settings regarding adjustment and tolerance but you can (and in this case should) modify them before the constraints are created or after that (you can always modify them in the model tree).

[Matej]

I can only confirm that the Search Contact Pairs tool does nothing a user cannot do manually. It is only used to find the geometry that is close enough and assigns some initial values to the constraints/contacts.

In your image called SETUP both of the shell parts are coloured yellow. Did you also try to define the tie constrict between one surface and one edge?

[lukerickert]

Thanks Matej
I think the issues come down to trying to use surfaces extracted from solids, Solidworks doesn’t have the tools create high quality surfaces like CATIA (I think Onshape is actually better for surfaces than Solidworks). I am just recreating the parts as surfaces from scratch simplified and clean which seems to work. It is too bad Dassault doesn’t share the surfacing tools between packages but I guess that is why big companies will pay something like 10x the cost of Solidworks for CATIA V6

Luke

[xyont]

hi,

i reproduce your models but using tied contact type instead of tie constraint, stress discontinuity and transition become represent well. also someone can use layered shell element match the number of element along thickness to refined. some of disadvantages of these features are in large deformation were activated by default.

[Calc_em]

That’s an interesting alternative, good to know that it works better than tie constraint in this case (even though the latter should be much more efficient computationally). So far I haven’t tried this type of interaction for solid-shell connection but it’s very promising in such applications and seems to be the best alternative to unimplemented shell-to-solid coupling.

[xyont]

thanks are due to Jaro Hokkanen (2014) who implemented Tied Contact features, found this on report document and CalculiX unique feature which treat beam and shell element are represented by solid element.

although coupling features generally used by many commercial application, still facing a problem in equilibrium and displacement compatibilities, it has limitation (Edward L Wilson, 2008 - reff. links) and someone need to be concern.