How to connect paltes with hinges without merging nodes?

Dear forum,

I want to mesh several plates lying next to eachother without merging the nodes and connect them with line hinges (see picture).

I am using
but that doesn’t seam to work with edge nodes, only internal nodes.

Can someone please help me out here?


  1. Define SPTs with numbers for each plate, e.g.:
    Spt No 11 x 0 0 0
    Spt No 12 x 0 1 0
    Spt No 13 x 2 1 0
    Spt No 14 x 2 0 0
    Spt No 21 x 2 0 0 $ Spts with explicitly different nr at same coordinate do not merge
    Spt No 22 x 2 1 0
    Spt No 23 x 4 1 0
    Spt No 24 x 4 0 0

  2. Define SLNs with numbers for each plate, e.g.:
    Sln No 1112 Npa 11 12
    Sln No 1213 Npa 12 13
    Sln No 1314 Npa 13 14
    Sln No 1411 Npa 14 11
    Sln No 2122 Npa 21 22 $ Sln explicitly connected to different Spts → doesn’t merge
    Sln No 2223 Npa 22 23
    Sln No 2324 Npa 23 24
    Sln No 2421 Npa 24 21

  3. Define SARs using the SLNs, e.g.:
    Sar No 10
    SarB Type out NL 1112,1213,1314,1411
    Sar No 20
    SarB Type out NL 2122,2223,2324,2421

  4. Add a constraint or spring between the adjacent lines, e.g.:
    Sln No -2122 $ - for altering an existing Sln
    SlnS RefT >Sln Ref 1314 Ca 1000 $ Coupling/spring to line
    $ Some support conditions at the ends as well:
    Spt No -11 Fix F $ Either pointsupport
    Sln No -1112 Fix F $ Or linesupport

Also check out the teddy example in your installation folder:
C:\Program Files\SOFiSTiK\2023\SOFiSTiK 2023\sofimshc.dat\english\area_models\separated_slabs.dat

Thank you @sfr, this helped a lot.

However, it assumes that I’m working with structural areas. If I want to apply this on a mesh, how can I do that?

My example is the way to go if you are using sofimshC (IMO), which uses structural elements (like SARs)

If you are using sofimshA it is the same principle:
Generate a meshed area for each part and connect the relevant edges.

I assumed you are working with sofimshA/structural areas since you tried SAR ... XFLG 'PLA'

I’m working with sofimsHC indeed. Anyways, I adapted my workflow, and now it works fine.

I’ve stumbled upon the next problem however. How do I decide the rotational spring stiffness. The spring stiffness should be the same as the bending stiffness of the plate itself, i.e. EI [Nm²]. However when I look in the sofimshc manual, the unit should be kN/rad, which I don’t understand.

Could you @sfr possibly explain this aswell?