buckling 1

[gwena]

buckling

I'm doing a non-linear analysis in order to perform buckling of a strip. One extremity is clamped. The second one is free and a load is applied.
The linear buckling analysis was ok.
For the non-linear one, using S4R5 elements,
*STEP,NLGEOM,INC=500
*static,riks
...
adding an imperfection or not, the problem is that only the last row of elements at the end of the strip is folded and not all the shape is deformed. (with a picture it would be easier to understand!)
Is anyone has an explanation? I can't find what is wrong.
Thanks a lot !

 

[gwolf]

Try taking riks off, if it's fully constrained at one end it will work. The analysis will bomb out near the bucking load with successively smaller increments.

Also check that your initial load fraction on the *static does not already exceed the buckling load. Apply about 10-20% of buckling load to start with e.g.

*STATIC
0.1,1.0

If this doesn't fix it, who knows, I'd have to take a look at the model.

regards,

gwolf.

 

[gwena]

First, thank you for your response !
Unfortunately, I didn't solve my model. As you said, I tried it with 10% of the buckling load and I put the RIKS method off but it doesn't work.
I tried it with the stabilize option too and with a displacement control but the problem is the same.
I don't understand.
How can I join you the model in order to have a look?
Thanks a lot for your experience !
Regards,
Gwen

 

[corus]

I would guess that the end which is clamped will buckle as here you have bending as well as direct compressive stresses. At the free end you only have direct compressive stresses and hnece the deflection will first show at the clapmed end.

corus

 

[gwena]

Only the last row of elements at the free end is deforming but I know that the deflection has to be global in a bending mode.
I didn't specific that is a curved thin strip.

Gwen

 

[xerf]

Did you try using S9R5 ?

 

[gwena]

I tried it with S4, S4R5, S8R5 and also STRI3.
But not with S9R5.
It should work with a simply S4R5 !
...
Gwen

 

[jcmbl]

try pasting the code in here to peruse it. Maybe you just use some other axes for load function, if you haven't used CAE. I know there is in the manual an example like yours..try fiddle it, although there's nothing clever in it.

 

[gwena]

Here it is ! Thanks a lot for any help!

*HEADING
TORSIONAL BUCKLING
*RESTART,WRITE
*parameter
R1=0.0359
L=0.6
p=0.060
PI=3.141592654
THETA=(p/R1*180/PI)/2
thickness = 0.0002
BETA=-90-THETA
BETA1=-90+THETA
node_circum=71
node_length=71
node_tot = node_circum*node_length
node_int = node_length-1
node_circum1 = node_circum+1
node_circum2 = node_circum+2
node_tmp = node_tot-node_circum+1
node_circum0 = node_circum-1
chn = node_circum*node_length-node_circum
*NODE,SYSTEM=C
10000,0,0,0
20000,0,0,<L>
1,<R1>,<BETA>,0
<node_circum>,<R1>,<BETA1>,0
<node_tmp>,<R1>,<BETA1>,<L>
<node_tot>,<R1>,<BETA>,<L>
*NGEN,LINE=C,NSET=bottom,SYSTEM=C
1,<node_circum>,1,10000,,,,0,0,1
*ncopy,new set=top,old set=bottom,shift,change number=<chn>
0,0,<L>
0,0,0,0,0,1,0
*NFILL
bottom,top,<node_int>,<node_circum>
*ELEMENT,TYPE=S4R5
1,1,2,<node_circum2>,<node_circum1>
*ELGEN,ELSET=LAME
1,<node_circum0>,1,1,<node_int>,<node_circum>,<node_circum>
*SHELL SECTION,ELSET=LAME,MATERIAL=MAT
<thickness>,
*MATERIAL,NAME=MAT
*ELASTIC
2.03E11,.3
**
*STEP,NLGEOM,INC=500
postbuckling analysis
*static,STABILIZE,FACTOR=0.0001
0.0001,1,1.E-30
*monitor,node=5006,dof=3
*BOUNDARY
5006,3,,-1
*BOUNDARY
bottom,1,6
*CONTROLS,ANALYSIS=DISCONTINUOUS
*OUTPUT,FIELD,FREQUENCY=2
*NODE OUTPUT,NSET=TOP
U,RF
*NODE OUTPUT,NSET=BOTTOM
RF,
*ELEMENT OUTPUT
S,
*OUTPUT,HISTORY,FREQUENCY=2
*NODE FILE,NSET=TOP
U,
RF,
*END STEP

 

[corus]

I see no meaningful results for this model as it says that deformed variables for one or more nodes are not available. From the displaced plot it appears that all of the model has been fixed by Abaqus except for the top line of nodes. The model can't be loaded into CAE as it's parametized so it can't be checked so easily. Go through the model again and check how you have defined the elements.

corus

 

[corus]

I went through the data and renmoved the spaces from the beginning of each line and got results. Here's part of the data:

*ELEMENT,TYPE=S4R5
1,1,2,<node_circum2>,<node_circum1>
*ELGEN,ELSET=LAME
1,<node_circum0>,1,1,<node_int>,<node_circum>,<node_circum>
*SHELL SECTION,ELSET=LAME,MATERIAL=MAT
<thickness>,
*MATERIAL,NAME=MAT
*ELASTIC
2.03E11,.3
**
*STEP,NLGEOM,INC=500
postbuckling analysis
*static,STABILIZE,FACTOR=0.0001
0.0001,1,1.E-30
*monitor,node=5006,dof=3
*BOUNDARY
5006,3,,-1
*BOUNDARY
bottom,1,6
*CONTROLS,ANALYSIS=DISCONTINUOUS
*OUTPUT,FIELD,var=preselect
*OUTPUT,HISTORY,var=preselect
*END STEP

corus

 

[corus]

When you look at the final results you'll see that the C section deforms as a cantilever beam. This is because you have applied the displacement to the centre of the arc on the shell which is offset from the centroid of the arc. This imposes a bending moment on the overall shell.

The shell deforms but the base of the shell is fully restrained and hence the shell buckles some distance above the fixed base.

corus

 

[gwena]

Great !
Conclusion is that spaces from the beginning of lines are dangerous !?
It's exactly what I want to verify : Buckling in a bending mode because of the bending moment.
Thanks a lot !