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

I’m not sure I understand you.
All my previous comments and attempts, they assume I have two separated nodes.

This is the aim of the post. ¿Have you try it ? It is not possible to link the rotations of two diferent nodes with *equation.

Standard Calculix test example files
beamrb.inp
beamrb2.inp

have a prescribed non-zero rotation for the ROT NODE through a *BOUNDARY card inside a step.

1 Like

It would have no sense.
You could impose a translation throug DOF 1,2 or 3 to the rot node.
That is supposed to induce a rotation on the rigid body.
It works on Solids but not for shells or beams. I’have been tryng for many years and only succed once in a really weird configuration.

yes, as i notified before it’s required rigid arm to transfer rotational.

*edited
using some distance in separation of nodes, it’s shown clear of pure displacement constraint in translation and rotation

Hi,

Could I look at you inp?. Looks like there is something strange.
I think your last three equation on the *EQUATION card are not taking any effect (rotational links).

I say that because you equation states : rx5 - rx10 = 0 —> rx5 = rx10.
Both ends must rotate clockwise, and your shape doesn’t look like they do.
By other hand, it is not a good point to test. Rx is zero at the midspam.

yes, just checked they work as expected with 3d elements. Now we need to check if same works with “1D beams” and then try to connect 2 beam spans using the ref nodes…

below result when rotational being released,

Why it doesn’t work for me?,

Could you please take a look at my input file.?

``````*NODE
1,0,0,0
2,0,0,3.025
3,0,0,2.775
4,0,0,0.25
5,0,0,0.5
6,0,0,0.75
7,0,0,1.025
8,0,0,1.275
9,0,0,1.525
10,0,0,1.775
11,0,0,2.025
12,0,0,2.275
13,0,0,2.525
14,0,0,1
15,0,0,2.65
16,0,0,2.9
17,0,0,0.125
18,0,0,0.375
19,0,0,0.625
20,0,0,0.875
21,0,0,1.15
22,0,0,1.4
23,0,0,1.65
24,0,0,1.9
25,0,0,2.15
26,0,0,2.4
*ELEMENT,TYPE=B32R
1,7,21,8
2,8,22,9
3,9,23,10
4,10,24,11
5,11,25,12
6,12,26,13
7,13,15,3
8,3,16,2
9,1,17,4
10,4,18,5
11,5,19,6
12,6,20,14
*ELSET,ELSET=Default
1
2
3
4
5
6
7
8
*ELSET,ELSET=Component
9
10
11
12
*MATERIAL,NAME=Steel
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7850
*BEAM SECTION,ELSET=Default,MATERIAL=Steel,SECTION=RECT
0.025,0.05
1,0,0
*BEAM SECTION,ELSET=Component,MATERIAL=Steel,SECTION=RECT
0.025,0.05
1,0,0
*BOUNDARY
2,1,,0
2,2,,0
2,3,,0
2,4,,0
2,5,,0
2,6,,0
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
1,6,,0
*AMPLITUDE,NAME=Ay_11_1
0,0
1,-100
*EQUATION
2
14,1,1,7,1,-1
2
14,2,1,7,2,-1
2
14,3,1,7,3,-1
2
14,5,1,7,5,-1
2
14,4,1,7,4,-1
2
14,6,1,7,6,-1
*STEP,NLGEOM=YES,INC=100,AMPLITUDE=STEP
*STATIC,SOLVER=PARDISO
0.1,1,0,0.1
11,2,1
*NODE FILE,GLOBAL=YES
U,RF
*EL FILE
S,NOE
*END STEP

``````

looking the attachment, i’m not seen an input section to defining rigid arm. Probably a general constraint also can be used to connecting beam ends to shell edge or solid face (mixed element) in a different way (i.e not tie constraint or tied contact). The advantage is capable to set as hinged or partial restraint by springs.

however, a lot of input is required to preset and only effective trough pre-processor such as CGX or PrePoMax.

I don’t understand a word .
Thanks anyway

i;m also post many screenshot of output, probably it can have more meaning than words.

Thanks too for bringing up the issue, it may lead me to another exploration.

it seems different with *RELEASE feature in Abaqus, one is assigned to node and the other is element. Remove options in CalculiX will induce all element connected sharing the same nodes, but release does not.

Trying to figure out what did you mean I came with an idea. I’m not sure if that’s what you wanted to transmit but anyway it lighted my bulb.
Now, I have no idea how I could validate this.

Thank you again.

attached an output of animation,

*edited

But the point is to be able to constrain 1 or 2 rotation and release the other.
¿Seems it works as a contact, right?.
¿Could you constrain bending but release torque? Would be ideal because stresses look really smooth in your proposal.

right, in case of no dof’s being released result displacement and stress continuity can be identical with tie constraint or tied contact type.

the advantages of general constraint using equation are possible to release specific dof’s and probably in partial restraint (semi-rigid) connection.

I can’t get this file running in ccx…however I noticed that ccx imposes the rot boundary condition using a mean rotation MPC (.12d file) so maybe that’s the path to follow: distributing coupling for translations and mean rotation mpc for rotations

1 Like

I modified Disla’s file in order to use rotations…I had to use 2 nodes per beam span but doesn’t work for torsion, bending is transmitted (more checks needed):

``````*NODE
1,0,0,0
2,0,0,3.025
3,0,0,2.775
4,0,0,0.25
5,0,0,0.5
6,0,0,0.75
7,0,0,1.025
8,0,0,1.275
9,0,0,1.525
10,0,0,1.775
11,0,0,2.025
12,0,0,2.275
13,0,0,2.525
14,0,0,1.025
15,0,0,2.65
16,0,0,2.9
17,0,0,0.125
18,0,0,0.375
19,0,0,0.625
20,0,0,0.875
21,0,0,1.15
22,0,0,1.4
23,0,0,1.65
24,0,0,1.9
25,0,0,2.15
26,0,0,2.4
262,1.,0.,0.
263,0.,1.,0.
264,0.,0.,1.
362,1.,0.,0.
363,0.,1.,0.
364,0.,0.,1.
*ELEMENT,TYPE=B32R
1,7,21,8
2,8,22,9
3,9,23,10
4,10,24,11
5,11,25,12
6,12,26,13
7,13,15,3
8,3,16,2
9,1,17,4
10,4,18,5
11,5,19,6
12,6,20,14
*ELSET,ELSET=Default
1
2
3
4
5
6
7
8
*ELSET,ELSET=Component
9
10
11
12
*MATERIAL,NAME=Steel
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7850
*BEAM SECTION,ELSET=Default,MATERIAL=Steel,SECTION=RECT
0.025,0.05
1,0,0
*BEAM SECTION,ELSET=Component,MATERIAL=Steel,SECTION=RECT
0.025,0.05
1,0,0
*BOUNDARY
2,1,,0
2,2,,0
2,3,,0
2,4,,0
2,5,,0
2,6,,0
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
1,6,,0
*AMPLITUDE,NAME=Ay_11_1
0,0
1,-100
*MPC
MEANROT,21,21,21,7,7,7,262
*MPC
MEANROT,21,21,21,7,7,7,263
*MPC
MEANROT,21,21,21,7,7,7,264
*MPC
MEANROT,20,20,20,14,14,14,362
*MPC
MEANROT,20,20,20,14,14,14,363
*MPC
MEANROT,20,20,20,14,14,14,364
*EQUATION
2
14,1,1,7,1,-1
2
14,2,1,7,2,-1
2
14,3,1,7,3,-1
** 2
** 14,5,1,7,5,-1
** 2
** 14,4,1,7,4,-1
** 2
** 14,6,1,7,6,-1
2
262,1,1.,362,1,-1.
2
263,1,1.,363,1,-1.
2
264,1,1.,364,1,-1.
*STEP,NLGEOM=YES,INC=100,AMPLITUDE=STEP
*STATIC,SOLVER=PARDISO
0.1,1,0,0.1
11,2,1
*NODE FILE,GLOBAL=YES
U,RF
*EL FILE
S,NOE
*END STEP
``````

Edited: mistake on nodes 20 21 in meanrotation definition

this modification allows for a flexible connection using springs:

``````*ELEMENT,TYPE=SPRING2,ELSET=rot-spring
1001,262,362
*SPRING,ELSET=rot-spring
1,1
1.e3
*EQUATION
2
14,1,1,7,1,-1
2
14,2,1,7,2,-1
2
14,3,1,7,3,-1
** 2
** 262,1,1.,362,1,-1.
2
263,1,1.,363,1,-1.
2
264,1,1.,364,1,-1.
``````

Thank you very much Juan for paying attention to this. I will carefully study your solution to see if I can extend to a more general case. My preliminary solution shown above is a mixture of Kinematic coupling and Equation.