TIED contact and beam won't converge in CCX 2.17+

1

Any ideas? The contact isn’t on the beam element but just coexists on other elements in the same file.

contact and beam
contact and beam1350×552 13.9 KB

*NODE
1,1,-0.5,0
2,0,-0.5,2
3,1,0.5,0
4,1,-0.5,2
5,0,0.5,2
6,1,-0.5,4
7,1,-0.5,2
8,1,0.5,2
9,0,-0.5,0
10,0,0.5,0
11,1,0.5,4
12,0,0.5,2
13,1,0.5,2
14,0,0.5,4
15,0,-0.5,2
16,4,0,4
17,0,-0.5,4
18,4,0,0
*ELEMENT,TYPE=C3D8,ELSET=SOLID
1,9,1,3,10,15,7,13,5
3,2,4,8,12,17,6,11,14
*ELEMENT,TYPE=B31,ELSET=BEAM
2,18,16
*SURFACE,NAME=BONDED_CONTACT_FACES(2)
3,S1
*SURFACE,NAME=BONDED_CONTACT_FACES
1,S2
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*SOLID SECTION,ELSET=SOLID,MATERIAL=MATERIAL
*BEAM SECTION,ELSET=BEAM,MATERIAL=MATERIAL,SECTION=RECT
1,1
0,1,0
*BOUNDARY
1,1,3,0
3,1,3,0
9,1,3,0
10,1,3,0
18,1,6,0
*CONTACT PAIR,INTERACTION=SI_1,TYPE=SURFACE TO SURFACE,ADJUST=57.44562646538
BONDED_CONTACT_FACES(2),BONDED_CONTACT_FACES
*SURFACE INTERACTION,NAME=SI_1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
1000000000000,1
*FRICTION
1,1000000000000
*STEP
*STATIC
*CLOAD
17,2,125000
6,2,125000
11,2,125000
14,2,125000
16,2,500000
*NODE FILE
U
*END STEP
2

The only thing that catches my eye is this warning (generated with 2.21 in my case):

 *INFO in cascade: linear MPCs and
       nonlinear MPCs depend on each other
       common node: 30 in direction 1
3

True. I tend to be a bit blind to those messages since they’re everywhere. The same message appears without the contact and NLGEOM turned on which does solve OK so it’s not obviously a problem though.

4

Hi Victor,

I guess the problem is at the supporting node of the beam. Inducing a knot at the beam base then solves (but I understand that is not a general solution to the problem).

*NODE
1,2.5005,0,-2
2,2.5005,0,-2.106421593531
3,-0.4995,0.5005,0
4,2.5005,0,2
5,0.5005,0.5005,0
6,0.0005,0.0005,0
7,-0.4995,-0.5005,0
8,0.5005,-0.5005,0
9,0.5005,0.5005,0
10,-0.4995,0.5005,2
11,-0.4995,-0.5005,2
12,0.5005,-0.5005,2
13,0.5005,0.5005,2
14,-0.4995,0.5005,-2
15,0.5005,0.5005,-2
16,0.5005,-0.5005,-2
17,-0.4995,-0.5005,-2
18,-0.4995,0.5005,0
19,-0.4995,-0.5005,0
20,0.5005,-0.5005,0
*ELEMENT,TYPE=B31
1,2,1
4,1,4
*ELEMENT,TYPE=C3D8
2,18,19,20,5,10,11,12,13
3,3,9,8,7,14,15,16,17
*ELSET,ELSET=Solid_Master
3
*ELSET,ELSET=Beam
4
*ELSET,ELSET=Solid_Slave
2
*ELSET,ELSET=Knot
1
*SURFACE,NAME=BONDED_CONTACT_FACES
3,S1
*SURFACE,NAME=BONDED_CONTACT_FACES(2)
2,S1
*MATERIAL,NAME=Steel
*ELASTIC,TYPE=ISOTROPIC
200000000000,0.3
*DENSITY
7850
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
200000000000,0.3
*MATERIAL,NAME=Steel(2)
*ELASTIC,TYPE=ISOTROPIC
200000000000,0.3
*DENSITY
7850
*MATERIAL,NAME=Material(2)
*ELASTIC,TYPE=ISOTROPIC
200000000000,0.3
*SOLID SECTION,ELSET=Solid_Master,MATERIAL=Steel
*BEAM SECTION,ELSET=Beam,MATERIAL=Material,SECTION=RECT
1,1
0,1,0
*SOLID SECTION,ELSET=Solid_Slave,MATERIAL=Steel(2)
*BEAM SECTION,ELSET=Knot,MATERIAL=Material(2),SECTION=RECT
1,1.000001
0,1,0
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
1,4,,0
1,5,,0
1,6,,0
14,1,,0
14,2,,0
14,3,,0
15,1,,0
15,2,,0
15,3,,0
16,1,,0
16,2,,0
16,3,,0
17,1,,0
17,2,,0
17,3,,0
*CONTACT PAIR,INTERACTION=SI_1,TYPE=SURFACE TO SURFACE,ADJUST=57.44562646538
BONDED_CONTACT_FACES(2),BONDED_CONTACT_FACES
*SURFACE INTERACTION,NAME=SI_1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
1000000000000,1
*FRICTION
1,1000000000000
*STEP
*STATIC,SOLVER=PARDISO
*CLOAD
4,2,500000
10,2,125000
11,2,125000
12,2,125000
13,2,125000
*NODE FILE,GLOBAL=YES
U
*END STEP
1 Like
5

firstly i try to disable CLoad on beam element end nodes then it works, probably there is a problem. Below my approach as similar with previously discussed.

*NODE
1,1,-0.5,0
2,0,-0.5,2
3,1,0.5,0
4,1,-0.5,2
5,0,0.5,2
6,1,-0.5,4
7,1,-0.5,2
8,1,0.5,2
9,0,-0.5,0
10,0,0.5,0
11,1,0.5,4
12,0,0.5,2
13,1,0.5,2
14,0,0.5,4
15,0,-0.5,2
16,4,0,4
17,0,-0.5,4
18,4,0,0
*ELEMENT,TYPE=C3D8,ELSET=SOLID
1,9,1,3,10,15,7,13,5
3,2,4,8,12,17,6,11,14
*ELEMENT,TYPE=B31,ELSET=BEAM1
2,18,16
*ELEMENT,TYPE=B31,ELSET=BEAM2
4,18,16
*SURFACE,NAME=BONDED_CONTACT_FACES(2)
3,S1
*SURFACE,NAME=BONDED_CONTACT_FACES
1,S2
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*SOLID SECTION,ELSET=SOLID,MATERIAL=MATERIAL
*BEAM SECTION,ELSET=BEAM1,MATERIAL=MATERIAL,SECTION=RECT,OFFSET1=0.5
0.5,1
0,1,0
*BEAM SECTION,ELSET=BEAM2,MATERIAL=MATERIAL,SECTION=RECT,OFFSET1=-0.5
0.5,1
0,1,0
*BOUNDARY
1,1,3,0
3,1,3,0
9,1,3,0
10,1,3,0
18,1,6,0
*CONTACT PAIR,INTERACTION=SI_1,TYPE=SURFACE TO SURFACE,ADJUST=57.44562646538
BONDED_CONTACT_FACES(2),BONDED_CONTACT_FACES
*SURFACE INTERACTION,NAME=SI_1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
1000000000000,1
*FRICTION
1,1000000000000
*STEP
*STATIC
*CLOAD
17,2,125000
6,2,125000
11,2,125000
14,2,125000
16,2,500000
*NODE FILE
U
*END STEP

result of modified models with two elements along its spans length.

2024-04-29 12_33_18-CalculiX GraphiX
2024-04-29 12_33_18-CalculiX GraphiX802×715 19.8 KB

2024-04-29 12_35_44-CalculiX GraphiX
2024-04-29 12_35_44-CalculiX GraphiX802×715 18.8 KB

6

This seems like a separate bug since it was OK in 2.16 which is after the purge of knots. I notice a difference in the output that 2.16 says Decascading the MPC's at every (both) iteration, whereas 2.17+ only say it on the first iteration. I tried to look at the code for that but there are a lot of conditions that trigger cascade() and it’s not clear to me what determines them.

Then there’s the other problem of why TIED contact turns on NLGEOM at all. It solves fine with *FREQUENCY without any iterations.

7

indeed, knot in beam and tied contact of solid at another shall have no relations.