Contact of two sets

I manage to write inp file not really understanding what I do. There are two sets to be contacted with each other but

*ERROR: too many cutbacks
best solution and residuals are in the frd file

What mistakes do I make in the inp file?

*HEADING
Model: CalculiX Beam Input File for welding experiment
*INCLUDE,INPUT=shelf.msh
*INCLUDE,INPUT=wall.msh
*BOUNDARY
*INCLUDE,INPUT=fix_123456.bou
*MATERIAL,NAME=steel
*ELASTIC
2e11,0.3
*SOLID SECTION,ELSET=Eshelf,MATERIAL=steel
*SURFACE,NAME=shelfsur
97, S6
99, S6
101, S6
103, S6
105, S4
107, S4
109, S4
111, S4
98, S6
100, S6
102, S6
104, S6
106, S4
108, S4
110, S4
112, S4
*SOLID SECTION,ELSET=Ewall,MATERIAL=steel
*SURFACE,NAME=wallsur
209, S3
225, S3
213, S3
229, S3
273, S1
289, S1
217, S3
233, S3
221, S3
237, S3
241, S3
245, S3
305, S1
249, S3
253, S3
257, S3
261, S3
321, S1
265, S3
269, S3
275, S1
291, S1
276, S6
280, S6
337, S1
353, S1
337, S6
307, S1
369, S1
323, S1
385, S1
*CONTACT PAIR,INTERACTION=SI1,TYPE=SURFACE TO SURFACE
shelfsur,wallsur
*SURFACE INTERACTION,NAME=SI1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=HARD
0,0
*STEP
*STATIC
*CLOAD
*INCLUDE,INPUT=loadn1.frc
*NODE FILE
U
*EL FILE
S
*END STEP
*STEP
*STATIC
*CLOAD
*INCLUDE,INPUT=loadn2.frc
*NODE FILE
U
*EL FILE
S
*END STEP
*STEP
*STATIC
*CLOAD
*INCLUDE,INPUT=loadn3.frc
*NODE FILE
U
*EL FILE
S
*END STEP
*STEP
*STATIC
*CLOAD
*INCLUDE,INPUT=loadn4.frc
*NODE FILE
U
*EL FILE
S
*END STEP

That’s a typical non-convergence problem. But it’s hard (if not impossible) to say what’s causing it since the majority of the input file is not included here. Maybe you could try using displacement control instead of force control. There can be some rigid body motions resulting from insufficient constraints too.

1 Like

What bases do you manage to come to this conclusion on?

Check it out here DropMeFiles – free one-click file sharing service

Since it’s a T-joint, contact doesn’t seem to be necessary here. Tie constraint should be sufficient and will eliminate this convergence issue.

HI,

¿Did you know ccx delivers results even when the model does not converge?

Look at the deformed view. There is valuable information there to understand what is going on.

¿How is your model constrained?. Keep in mind solids do not have rotational degrees of freedom.

¿What is your units system for dimensions, Load and Young Modulus?.

¿Have you consider using PREPOMAX or other tool to set up your models?

I mean, if you are learning, use it to set up the model and look what keywords are generated.

-You have defined 4 STEPS. ¿Which one is failing? ¿Don’t you think it is more convenient to be sure you can manage to make one to work?

1 Like

Hi Disla,

I constrained one node 123456 dof. But having some recent experience on BOUNDARY conditions, I am not sure if one constrained node is OK for simulation

Respectively mm, grams, gram / mm^2

I have no idea if there is such a tool to set up my models on Linux.

After a while I recall: “Divide and conquer.”. I took shelf with its forces but I did not go further then that as I managed to stumble into some party.

Not enought

Respectively mm, grams, gram / mm^2

grams is not a Load unit. Do you mean gramforce or somethig similar. Same for Young Modulus

You can give a try to MECWAY free version. You will see the inp for small models <1000 nodes until you gain some experience. Plenty of examples on the forum.

Right.

Run a frequency analysis (once you apply tie constraint to connect the parts) and you will see which degrees of freedom are left.

This table will help you with unit consistency:

IMG_0246

On Linux you could use GraphiX or FEM workbench in FreeCAD (it also utilizes CalculiX).

1 Like

I managed to omit force, my bad.

Thank you very much for comments.

Thank you very much for comments.

No it is not.

No it is not hard to say, of cause if you understand how *CONTACT PAIR card must be written.
Read the following example very carefully and when you reach *CONTACT PAIR card open ccx manual on the *CONTACT PAIR page, read my code and manual simultaneously

tiecontact.inp

*HEADING
Contact
*include, input=all.msh
*include, input=b-contact.nam
*include, input=s-contact.nam
*MATERIAL,NAME=EL
*ELASTIC
2e5,0.3
*SOLID SECTION,ELSET=Eall,MATERIAL=EL
*SURFACE,NAME=BIGSURF1
18, S1
19, S1
*SURFACE,NAME=SMALLSURF2,TYPE=NODE
Ns-contact
*CONTACT PAIR,INTERACTION=BIGSURF1,TYPE=NODE TO SURFACE
SMALLSURF2,BIGSURF1
*SURFACE INTERACTION,NAME=BIGSURF1
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
*CONTACT PAIR,INTERACTION=SMALLSURF2,TYPE=NODE TO SURFACE
SMALLSURF2,BIGSURF1
*SURFACE INTERACTION,NAME=SMALLSURF2
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=TIED
*BOUNDARY
*include, input=fix_123456.bou
*STEP
*STATIC
*DLOAD
*INCLUDE,INPUT=load.dlo
*NODE FILE ** It adds to Datasets → 1 DISP
U
*EL FILE ** It adds to Datasets → 2 STRESS
S
*END STEP
*END OF INP*********************************

And if you like to see how all of it works together I provide you with fbd file

tiecontact.fbd

valu Etyp he8

seto big
pnt p1 0 0 0
pnt p2 0 0 80

line l1 p1 p2
seta se1 l l1

swep se1 sesb1 tra 80 0 0 3

seta sesb2 A001
swep sesb2 sesb3 tra 0 80 0

seta fix A005
seta b-contact A006
setc big

seto small

pnt p3 30 30 80
pnt p4 30 50 80

line l2 p3 p4
seta se2 l l2

swep se2 sess1 tra 20 0 0 4

seta sess2 A007
swep sess2 sess3 tra 0 0 20
seta s-contact A007
seta load A008
setc small

elty all
elty all Etyp
mesh all
send all abq

#elty big Etyp
#mesh big
#send big abq

#elty small Etyp
#mesh small
#send small abq

send b-contact abq nam
send s-contact abq nam
send load abq pres 1000
send fix abq spc 123456

#contact big A006
#contact small A007
#plot se big r
#plus se small b
plot se all
/END OF FBD*******************

HAVE FUN!

I was talking about the error message “too many cutbacks”, it is commonly shown when convergence can’t be obtained.

Again, I was referring to the error message and the fact that in 99% of cases when it occurs, a complete input file is needed to see the boundary conditions, run the analysis and carry out some additional tests. I know the ccx syntax (and use its documentation for reference) but I was waiting for you to upload the rest of the input deck to take a look at it. Then, after seeing it, I told you that contact is likely unnecessary here.

Did you have a fun after all?