Is contact of beam and shell allowed in CCX?

[xyont]

hi,

i’m modeling contact analysis of beam and shell faces, try a simple model but did not succeed. anyone has experiences, are the solver CCX allowed this analysis type? or something i miss at input decks.

bellows are input files, thank you.

** Objective : Beam to Shell Contact
*NODE
1,0,0,0
2,100,0,0
3,100,100,0
4,0,100,0
5,50,25,10
6,125,50,10
*ELEMENT,TYPE=S4
1,1,2,3,4
*ELEMENT,TYPE=B31
2,5,6
*ELSET,ELSET=eplate
1
*ELSET,ELSET=ebeam
2
*SURFACE,NAME=splate
1,SPOS
*SURFACE,NAME=sbeam
2,S1
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
210000,0.3
*SHELL SECTION,ELSET=eplate,MATERIAL=Material
10
*BEAM SECTION,ELSET=ebeam,MATERIAL=Material,SECTION=RECT
10,10
*BOUNDARY
1,1,6
4,1,6
*SURFACE INTERACTION,NAME=SInt
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
10000000
*FRICTION
1,1000000
*CONTACT PAIR,INTERACTION=SInt,TYPE=SURFACE TO SURFACE,ADJUST=1
sbeam,splate
*STEP,NLGEOM
*STATIC
*CLOAD
6,3,1000
*NODE FILE,GLOBAL=YES
U,RF
*EL FILE
S,E,ENER
*END STEP

[jbr]

Hi @xyont, I haven’t tried contact with beams and shells in ccx. If I remember correctly, these elements are expanded in ccx which could be part of the issue if the nodes are penetrating surfaces. Also, I recall having issues with the friction card for initial contact.
Try removing the friction card and expand the elements to fully solid elements and see what happens- that way you would be able to pin-point the issue with the simplified model (I hope).

Good luck,
J

[xyont]

thanks @jbr , yes right… beam element B31 are expanded to C3D8I in CCX as documented. so i moved the beam coordinate by 10mm upward to match face of shell element with 10mm thickness (center) and set tolerance to 1mm.

previously i was succeed to models shell to shell contact analysis, except solid to shell element. had some problems if i places solid at the edges of shell. it’s been long time, i did not remember exactly for each of contact type i used. need to check again later.

for now i want to study in contact of beam and shell element possibility in CalculiX (CCX), try to remove friction keywords as suggested and refine my mesh models still not succeed, it divergences.

[vicmw]

It looks like you don’t have any constraints on the beam so it will be free to rotate about the contact point or translate through the shell before the contact closes. I would constrain all 6 DOF at the far end of the beam and put the force at the contact end so it’s a cantilever.

I’ve had success with beams like this as well as shell edges but the beam or shell edge should be the slave surface.

Get it to solve without contact first, otherwise you might be chasing non-contact problems.

[xyont]

hi @vicmw thank you for looking up into my problems, as i know tied contact does not required any additional restraint (e.g rotation). but still i try as you suggested, seems rotational restrain in the edge of beam leads to MPC conflict. even i removed concentrated load and apply another loads due to self weight.

here’s the same problem as the first, i solved by using shell to shell tied contact.

[vicmw]

Oh right, I didn’t notice the TIED in there. What do you mean shell to shell tied contact? It’s working OK now though?

[xyont]

it’s ok. i mean using shell element for both plate and beam models, it’s shell face contact using simple one (tied) before another complexity in contact features of CalculiX CCX.

yes. seems it work as expected, i’ll validate later using continuous mesh models with solid element.

again, for now i’m seeking the possibility using contact between shell and beam element faces. especially for tied contact type.

thank you,

[vicmw]

I recreated a similar model and it works fine. Not sure what the difference is from yours. Maybe ADJUST is too small?

Inp file:

*NODE
1,0,0,0
2,1,0,0
3,1,1,0
4,0,1,0
5,0.5,0,0
6,1,0.5,0
7,0.5,1,0
8,0,0.5,0
9,0.5,0.5,0
10,0.7578885555267,0.2700786888599,0.1
11,0.9867775440216,0.4209091067314,0.493542432785
*ELEMENT,TYPE=S4,ELSET=Shell
1,8,9,7,4
2,1,5,9,8
3,5,2,6,9
4,9,6,3,7
*ELEMENT,TYPE=B31,ELSET=Beam
5,10,11
*SURFACE,NAME=bonded_contact_faces(2)
5,S6
*SURFACE,NAME=bonded_contact_faces(3)
4,SPOS
3,SPOS
1,SPOS
2,SPOS
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*BEAM SECTION,ELSET=Beam,MATERIAL=Material,SECTION=RECT
0.1,0.1
-0.5502415540974,0.8350055282119,0
*SHELL SECTION,ELSET=Shell,MATERIAL=Material
0.1
*BOUNDARY
1,1,6,0
4,1,6,0
8,1,6,0
*CONTACT PAIR,INTERACTION=SI_1,TYPE=SURFACE TO SURFACE,ADJUST=14.97859850907
bonded_contact_faces(2),bonded_contact_faces(3)
*SURFACE INTERACTION,NAME=SI_1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
1E+14
*FRICTION
1,1E+14
*STEP,NLGEOM=YES
*STATIC
1,1
*CLOAD
11,1,1
11,2,2
11,3,3
*NODE FILE
U
*END STEP

[vicmw]

Oh, nevermind that last post. The problem in your original model is that it should use the S2 face of the beam, not the S1 face.

S2 is the beam’s face that’s adjacent to the shell. Its normal is in the +1 direction, which is -Z as described in the manual section 6.2.33 Three-node 3D beam element (B32 and B32R) with “implicitly through the default of (0,0,-1).”

[xyont]

thanks again @vicmw to looking back into my problems, it’s work as expected for now. i wrongly/missed to redefine face of beam element due to default setting assignment by the solver. previously i removed user local axis definition since it lead to error in umpc_mean_rot

next i will study the same cases with all of element type, also in mesh sensitivity and validation with continuous mesh of solid element.

[xyont]

regarding to your output pictures: it’s quite strange, the solver finished to runs and gave an output results. beam faces S6 is not available in documentation (p.444), only 1,2,3,5 there’s no face for 4 & 6?

looking up to your model, seems it detected as face at bottom end of beam element.

[vicmw]

Yea, beam faces 4 and 6 are at the two ends. Not sure why they’re not listed with the others.