## Element Membrane M3D6

About the development of the FEM module/workbench.
Groguigui
Posts: 18
Joined: Thu Mar 09, 2017 2:13 pm
Location: Lille

### Element Membrane M3D6

Hi,

I would like to simulate a spherical shell with internal pressure, like a ball, with hyperelastic material (Neo Hooke and Yeoh), to compare with analytical solution.

But the model never converges, always for same reason :
"*ERROR : too many cutbacks
best solution and residuals are in the frd file"

I test some solver and different increment (direct, iteratif, cholesky, explicit, in INP writing).

1) Do you know if calculix can solve spherical shell problem?
2) How can I change cutbacks?
3) Which solver is it better?

May be it will be better to ask this question at Guido Dhondt, because it is a calculix problem...
Last edited by Groguigui on Fri Apr 21, 2017 8:35 am, edited 1 time in total.
sodelo
Posts: 73
Joined: Tue Jan 24, 2017 9:20 am

### Re: ERROR : too many cutbacks

Hi,

I suspect you face a problem of material instability (well known for elasto-plasticmaterials).
- Please try first with an elastic material --> it should cpnvergence with the static solver
- then for a elasto-plastic material (for example sigma=KEps^n). I do not exactly remember the formula but if n=0.18, you should get the instability when EpsBar (equivalent plastic strain) is around 0.12.

To solve this, best solver is dynamic, implicit. You need inertia to stabilize the solution.
Try something like,
*Dynamic
0.01,1.,1e-7,0.01

BR
Last edited by sodelo on Fri Apr 07, 2017 7:52 am, edited 1 time in total.
makkemal
Posts: 325
Joined: Wed Apr 29, 2015 12:41 pm

### Re: ERROR : too many cutbacks

Activate user defined incrementation , the defaults tend to not be sufficient when dealing with non-linear problems.
Then set the control parameters manually

user_incrementations.PNG (11.45 KiB) Viewed 248 times
Groguigui
Posts: 18
Joined: Thu Mar 09, 2017 2:13 pm
Location: Lille

### Re: ERROR : too many cutbacks

Thanks,

Finally, I found how solve my problem : I used *Controls fonction to set increments and cutbacks.
http://web.mit.edu/calculix_v2.7/Calcul ... de179.html
bernd
Posts: 3924
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: ERROR : too many cutbacks

Groguigui wrote:I used *Controls fonction to set increments and cutbacks.
you can set them in FreeCAD CalculiX solver object too. Means no need to edit the input file.
Groguigui
Posts: 18
Joined: Thu Mar 09, 2017 2:13 pm
Location: Lille

### Re: ERROR : too many cutbacks

Yes Bernd, I saw, but I think isn't possible to set cutback in FreeCAD. Anyway, actually I have another problem.

Do you know why FreeCAD solve a stress in third dimension when we use a shell element? Usually, it must be zero with plane stress hypothesis.

Actually I would like to solve a hyperelastic spherical problem under pressure. But I don't understand why results are different to analytic solution.
fandaL
Posts: 226
Joined: Thu Jul 24, 2014 8:29 am

### Re: ERROR : too many cutbacks

Results in local coordinate system are new for shell elements in ccx 2.12 * ccx 2.12 creates automatically local coordinate system for shell elements, but projecting of global x-axis could be strange for elements with normal direction close to x-direction.

For shells a local coordinate system is automatically established by projecting the global or local (if defined by the user) x-axis on the shell surface.
from http://www.dhondt.de/new_calc.htm

Older versions print stresses in a global c.s.! * results are by default in the global c.s. The local coordinate system must be triggered in the .inp file by

Code: Select all

`*EL FILE, global=noS, E`

Plane stress (or plane strain) needs special element types which can be used only on 2D model in xy plane in Calculix. So I would expect nonzero normal stresses on your shell elements.

*EDITED
Last edited by fandaL on Wed Apr 19, 2017 2:40 pm, edited 1 time in total.
Groguigui
Posts: 18
Joined: Thu Mar 09, 2017 2:13 pm
Location: Lille

### Re: ERROR : too many cutbacks

So I would expect non zero normal stresses on your shell elements.
And you're right!

Plane stress (or plane strain) needs special element types which can be used only on 2D model in xy plane in Calculix.
I understand, that is why I have non zero normal stresses, because applied pressure is normal on my shell elements. In fact I didn't work with plane stress hypothesis.

1) How can I find this elements types? Does it exist actually in FreeCAD? In calculix?

2) What calculix version is in FreeCAD 0.17? I don't know where is this information.

3) Sorry I have already ask this question, but I forgot the answer, it is possible to solve a problem with shell AND volumic mesh with calculix and/or freeCAD? Like a volumic cube with different materials on each faces and inside.
fandaL
Posts: 226
Joined: Thu Jul 24, 2014 8:29 am

### Re: ERROR : too many cutbacks

1) How can I find this elements types? Does it exist actually in FreeCAD? In calculix?

You can look to the manual http://www.feacluster.com/CalculiX/ccx_2.11/doc/ccx/ under Theory/Element Types there are several plane stress elements. After writing .inp file in FreeCAD you can search in the file line like

Code: Select all

`*Element, TYPE=S6, ELSET=Eall`

and change from S6 (shell) to CPS6 (plane stress) element type
However, it will most probably fail on spherical model. You can define plane stress elements only in xy plane.

2) What calculix version is in FreeCAD 0.17? I don't know where is this information.

2.8p or 2.11 You can find it, when you click “Run Calculix”, in the beginning of the printed log

3) Sorry I have already ask this question, but I forgot the answer, it is possible to solve a problem with shell AND volumic mesh with calculix and/or freeCAD? Like a volumic cube with different materials on each faces and inside.

It should be possible in CalculiX. FreeCAD does not yet support meshes combining 2D and 3D elements.
UR_
Posts: 44
Joined: Tue Jan 03, 2017 8:42 pm

### Re: ERROR : too many cutbacks

Hello,
If you have a 3d-shape like a balloon, and you have to avoid bending stress. then membrane elements are first choose.

See http://www.dhondt.de/ccx_2.12.pdf
Page 92 cit:
6.2.14 Three-node membrane element (M3D3)
This element is similar to the S3 shell element except that it cannot sustain
bending. This is obtained by modelling hinges in each of the nodes of the
element. Apart from that, all what is said about the S3 element also applies
here.

Membrane elements could not bend. They stay plain in space.
External forces (and pressure loads) are applied normal to membrane's face
Internal forces are aligned tangentialy to membrane's face and leads to plain deformation.
Curvature is only done on element's edges.