Very broad question.
You should better specify the context, as there can't be a unique answer.
Generally speaking I would say that it is impossible to do such connection maintaining a correct representation of stresses near the junction, especially on solid side. However this should not be of much importance, but it all depends on what you are doing.
My position is that a finite element model should never be thought as a as realistic as possible representation of a real thing, but as something tailored for determining and studying only the phenomena (stresses) relevant to the situation being studied. prex
motori@xcalcsREMOVE.com
I am interested in trsnsfering some Moment from shell to solid and am not bothered about the stress distribution in the immediate neighbourhood of this shell-solid connection.
Hi k3,
if you use NASTRAN after version 69, there is a special element called RSSCON, that was developed to handle such problem. Off course, you can still use the MPC to connect 2 elements with different stifness. I think, there must be exist such elements in other FEA-Programs, because this is a crusial issue.
The easiest way to do it is to overlap at least one row of plate elements with the solid elements so that the plate moments are reacted by a plane of nodes (rather than a line of nodes) on the solids. The issue you will have to decide for yourself is whether modelling that way really reflects what's going on in the real structure.
MPC is abbreviation of Multi Point Constrains, i.e joints some DOFs together, but this the term used in MSC/NASTRAN, i haven't heard it in ANSYS.
It likes that you should do like what KSWpe said with some considerations. Below i citate the explanation from ANSYS (section 4.4 of ANSYS documents):
1. Shell-to-solid submodeling is activated by setting KSHS to 1 on the CBDOF command (Main Menu>General Postproc>Submodeling>Interpolate DOF) and the BFINT command (Main Menu>General Postproc>Submodeling>Interp Body Forc). This feature is not applicable to offsets used with SHELL91 or SHELL99 (KEYOPT(11) 00).
2. Cut boundaries on the submodel are the end planes that are normal to the shell plane (see Node Rotations). Nodes on these cut boundaries are written to the node file [NWRITE] (Main Menu>Preprocessor>Create>Nodes> Write Node File).
3. To determine the DOF values at a cut boundary node [CBDOF], the program first projects the node onto the nearest element in the shell plane. The DOF values of this projected point are then calculated by interpolation and assigned to the corresponding node. Interpolated temperatures [BFINT] are calculated based on the average temperature at the midplane of the nearest shell element.
4. In a structural analysis, only translational displacements are calculated for the cut boundary nodes, but their values are based on both the translations and rotations of the projected point. Also, the node is rotated such that the nodal UY direction is always perpendicular to the shell plane, as shown in Node Rotations. A UY constraint will be calculated only for nodes that are within 10% of the average shell element thickness from the shell plane. This prevents over-constraint of the submodel in the transverse direction.
5. The .CBDO file written by the CBDOF command will consist of two blocks:
- a block of NMODIF commands (indicating node rotation
angles) and DDELE commands (to delete UY constraints)
- a block of D commands (to apply the interpolated DOF
values).
6. You must read in the .CBDO file in PREP7, because the NMODIF command is only valid in PREP7. To do so, enter the preprocessor, then use one of these methods:
Command(s): /INPUT
GUI: Utility Menu>File>Read Input from
Dear Kiran,
U can interface the shell to solid using rigid elements but before that make a patch( thin layer of shell) over the face of the solid where u want to connect. Its very easy to model using Hypermesh/PATRAN. Regarding MPC what zuardy said is right. It means multi point constraint term used in MSC/NASTRAN. But depending upon model u can interface using single point constarint also i.e one to one node corresponding nodes of shell and solid.
And I haven't worked in ANSYS so I can't help u.
bye.
Two options one has in connecting a solid to a shell although one has been already quoted i repeat that as a first option
first option: Overlap some rows/columns of shell elements with that of solid elements .with the fact in mind that only there are overlapping DOFS corresponding to the three displcement components. There is no transfer of rotational components. This is justified in that the displacement DOFS being apart by a distance of length of element account for rotation components coming in.
Second option: Is by penalty function approach, although u can have a rigid spring with high stifnnes to transfer the displcements.
The solution all depends on what kind of load transfer that is expected between the solid and shell. If join is assumed to be rigid and with the external loading causing no much predominant twist at the joint the use of above two options is valid.
raj
kalya76@yahoo.com
Well i belive one another option of connecting a solid and a shell. In terms of FE program i suggest my view point.
In Assembling the stifnesses one can make the extra components coming from the shell as zero.and just have the cumulative effect correponding to displacement components.
One anothe rway is have a transition element may be a tetrahedron with varying DOFs..seperate formulation is required for this
