# Rotational dof's release. "-->Internal<---" steel connection

Comming from here.

Please, I would like to know ¿how one could release one specific rotational degree of fredom of a T conection between two beams (or beam column)? .

Or seen in the other way.

¿How to constrain everything but one specific rotational degree of fredom of a T conection if one builds the nodes relationship from zero.

That would cover internal steel conections without relative internal rotational stiffnes in a specific direction. By internal I mean connection inbetween members not external BC.

I know how to build the displacements constrain by means of *equation but the relationship between rotational degrees of freedom doesn’t seem to work when the nodes belong to beam elements.
Someone suggest this is possible.

Example:

Thanksstrong textemphasized text

*EQUATION seems to be the only way. Maybe you could apply rigid body constraints to the end nodes and then use *EQUATION on their rot nodes.

probably the thread names need to be change from “stiffness” to “dof’s” to make it more clear.

Rotational Stiffness release. Internal steel connection

my previous example is related to end release in beam/frame based common structural analysis programs. When both end nodes of beam being released in all rotational DOF’s ti will lead to unstable structure. Some programs provide artificial stiffness in rotation around longitudinal axes of beam element, but the other is not.

rotation stiffness in beam weak and strong axis is advanced modeling, in branch of nonlinear semi-rigid connection.

That’s the point. When you link nodes that belong to two different beams it doesn’t work. Is it a bug , a limitation or wrong set up from my side?

Those kind of connections are very common. Any joint build with a pin does not allow rotations other than around the axis of the pin.

Doesn’t seem related with being end nodes. Example attached.(Doesn’t work because do not link both beam rotations on the head of the column).

``````*NODE
1,0,0,0
2,0.8125,0,0
3,0.8125,-0.51,-1.942890293094E-16
4,0.8125,-0.01,0
5,0.40625,0,0
6,0.8125,-0.26,-1.110223024625E-16
7,0.8125,-0.385,-1.665334536938E-16
8,0.8125,-0.135,-5.551115123126E-17
9,0.203125,0,0
10,0.609375,0,0
11,0.1015625,0,0
12,0.3046875,0,0
13,0.5078125,0,0
14,0.7109375,0,0
15,0.8125,-0.4475,-1.665334536938E-16
16,0.8125,-0.3225,-1.387778780781E-16
17,0.8125,-0.1975,-8.326672684689E-17
18,0.8125,-0.0725,-2.775557561563E-17
*ELEMENT,TYPE=B31
1,11,9
2,12,5
3,13,10
4,14,2
5,15,7
6,16,6
7,17,8
8,18,4
9,1,11
10,9,12
11,5,13
12,10,14
13,3,15
14,7,16
15,6,17
16,8,18
*ELSET,ELSET=Component
5
6
7
8
13
14
15
16
*ELSET,ELSET=Horizontal
1
2
3
4
9
10
11
12
*MATERIAL,NAME=Steel
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*DENSITY
7850
*BEAM SECTION,ELSET=Component,MATERIAL=Steel,SECTION=RECT
0.05,0.02
-1,0,0
*BEAM SECTION,ELSET=Horizontal,MATERIAL=Steel,SECTION=RECT
0.05,0.02
0,1,0
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
1,4,,0
1,5,,0
3,1,,0
3,2,,0
3,3,,0
3,4,,0
3,5,,0
*EQUATION
2
4,1,-1000,2,1,1000
*EQUATION
2
4,2,-1000,2,2,1000
*EQUATION
2
4,3,-1000,2,3,1000
*EQUATION
2
4,6,-57.29577951308,2,6,57.29577951308
*STEP,NLGEOM=YES,INC=100
*STATIC,SOLVER=PARDISO
1,1,0,0
5,2,-25000
*NODE FILE,GLOBAL=YES
U
*EL FILE,OUTPUT=2D,SECTION FORCES
S,NOE
*END STEP

``````

it’s a rotational dof’s not stiffness like figure below, if it’s a common thing, so i’m curious to know how.

(source: Alemdar et al, 2009)

maybe it needed to more some emphasize, physical member steel beam end is a different thing with beam element end node in mathematical model.

please provide sketch of problem and result expected by hand calculation, sometime too complex models and many nodes are not easy to understand quickly.

*edited

only quick review of input files attach, some questionable at this section

Abaqus has `*RELEASE` (and equivalent advanced MPC constraints) for that. Would be nice to have it in CalculiX too but it probably won’t be added due to all the issues with rotational DOFs.

2 Likes

regarding rotational stiffness, it needed to use additional rigid arm similar case i has been discussed before. Fortunately, semi-rigid connection of both linear and nonlinear spring can be modeled.

This approach works in Abaqus but fails in CalculiX (with no errors, just *INFO in cascade: linear MPCs and nonlinear MPCs depend on each other common node: 23 in direction 1):

``````*Node
1,           0.,           0.,           0.
2,           7.,           0.,           0.
3,          14.,           0.,           0.
4,          21.,           0.,           0.
5,          28.,           0.,           0.
6,          35.,           0.,           0.
7,          42.,           0.,           0.
8,          49.,           0.,           0.
9,          56.,           0.,           0.
10,          63.,           0.,           0.
11,          70.,           0.,           0.
*Element, type=B31, elset=beam1
1,  1,  2
2,  2,  3
3,  3,  4
4,  4,  5
5,  5,  6
6,  6,  7
7,  7,  8
8,  8,  9
9,  9, 10
10, 10, 11
*Beam Section, elset=beam1, material=Material-1, section=RECT
1,1
0.,0.,-1.
*Node
12,          70.,           0.,           0.
13,          77.,           0.,           0.
14,          84.,           0.,           0.
15,          91.,           0.,           0.
16,          98.,           0.,           0.
17,         105.,           0.,           0.
18,         112.,           0.,           0.
19,         119.,           0.,           0.
20,         126.,           0.,           0.
21,         133.,           0.,           0.
22,         140.,           0.,           0.
*Element, type=B31, elset=beam2
11, 12, 13
12, 13, 14
13, 14, 15
14, 15, 16
15, 16, 17
16, 17, 18
17, 18, 19
18, 19, 20
19, 20, 21
20, 21, 22
*Beam Section, elset=beam2, material=Material-1, section=RECT
1,1
0.,0.,-1.
*Node
23,          70.,           0.,           0.
24,          70.,           0.,           0.
25,          70.,           0.,           0.
26,          70.,           0.,           0.
*Nset, nset=end1
11,
*Nset, nset=end2
12,
*Rigid Body, ref node=23, rot node=25, nset=end1
*Rigid Body, ref node=24, rot node=26, nset=end2
*Equation
2
23, 1, 1.
24, 1, -1.
*Equation
2
23, 2, 1.
24, 2, -1.
*Equation
2
23, 3, 1.
24, 3, -1.
*Equation
2
25, 1, 1.
26, 1, -1.
*Equation
2
25, 2, 1.
26, 2, -1.
*Material, name=Material-1
*Density
8e-09,
*Elastic
210000., 0.3
*Boundary
1, 1, 6
*Step
*Dynamic
1.,1.,1e-05
22, 2, -200.
*Node file
U
*El file
S,E
*End Step
``````

ccx has *REMOVE parameter but I don’t think I can use that. I dare *EQUATION would work perfectly if Rx ry and rz could be stated between two nodes of different beams.

i have been discussed this feature in PrePoMax forums specifically for shell element since beam element is not already supported.

the purpose of release features are commonly used to remove rotational dof’s at beam end nodes. so, it may have a sense and usefulness.

many structural analysis program available have featured to control directly all dof’s released, but limited to 1D beam element.

Mecway internal solver can release rotational dofs of beams. It’s called flexible joint on beam.
Do you think this is an actual solver limitation? or maybe a bug or wrong set up from my side.
It doesn’t work with shells neighter.
¿What’s the point of those rx, rz and ry in *equation (dof’s 4,5,6) ?. Solids doesn’t have rotational degrees of freedom.

if i can remember properly, in my simple case at link above: some rotations can not directly equivalencies with another rotation at both. This mean rotation of some nodes only can be equivalencies to displacement of another node.

I think this is related to the “solid element nature” of CCX, ccx doesn’t have true structural elements (except those Calc_em brings to my memory usually) so nodes only have 3 dofs (not 6 in reality).

it looks like equation doesn’t account for the expansion, so probably a rigid body has to be created at the joint nodes so rotational dofs can be considered.

I have managed to define two rigid bodies , one per node and couple separately the REF and ROT but no luck.
Thanks all

Applying SPCs to rigid body ref nodes does work?

It does. I use that quite often.

also with ROT ref nodes?

ccx didn’t complain but I have never being able to make a rigid beam rotate using the rot node (*) .

EDITED : (*) Imposing a translation on ROT node to be more clear.

You can fix the translation of the REF NODE and the rotations around the ROT NODE using the *BOUNDARY card outside a STEP. And using *BOUNDARY inside a STEP (what the manual for *BOUNDARY calls “inhomogeneous conditions”) you can prescribe a translation on the REF NODE; that works. But I’ve not tried prescribing a rotation on a ROT NODE inside a STEP.

LISA is the predecessor, beam element using 1D classical Euler-Bernoulli formulation i.e ignoring shear deformation, but maybe Mecway has been updated later to Timoshenko formulations.

as i remember: end released, rigid end offset and elastic spring rotation/translation can be directly add or modify in elastic beam element stiffness matrix. This is may not possible for nonlinear beam element i.e composed (3D) or fiberized (1D), OpenSees also need the nodes to be separated and connecting them using MP Constraint (equalDOF)

however, it can be useful when CalculiX is capable to set up restrained DOF directly for all translation and rotation as OpenSees does. Maybe by user defined ‘knot’ at nodes of beam or shell element, so a behavior can be similar to rotational restrained of support or rotational load moment/torque as it has been implemented.