Element Membrane M3D6

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

Re: ERROR : too many cutbacks

Postby Groguigui » Fri Apr 21, 2017 8:34 am

Thanks, that is very interesting! You're right, membrane element must be better in my case.

Actually, if I write M3D6 in "*element type", instead of S6, FreeCAD say :
*ERROR reading *SHELL SECTION: *SHELL SECTION can only be used for shell elements.
Element 11 is not a shell element.

Obviously, element 11 is the first of element of the list.

Do you know how can I resolve this error?

I use ccx2.9 but here http://www.dhondt.de/ccx_2.9.pdf, M3D6 already exist.
ulrich1a
Posts: 1406
Joined: Sun Jul 07, 2013 12:08 pm

Re: Element Membrane M3D6

Postby ulrich1a » Fri Apr 21, 2017 12:47 pm

Groguigui wrote:Do you know how can I resolve this error?
I could not find a hint in the manual, but for example for axisymmetric elements, you have to use a *SOLID SECTION but not a *SHELL SECTION.
So I would try to just replace the *SHELL with *SOLID.

Edit: Another try would be to replace *SHELL with *MEMBRANE
Calculix is partially compatible to Abaqus. So I sometimes look up information on Abaqus. See for example here: http://abaqusdoc.ucalgary.ca/v6.9/books ... 33sfsq.inp

Ulrich
User avatar
Groguigui
Posts: 18
Joined: Thu Mar 09, 2017 2:13 pm
Location: Lille

Re: Element Membrane M3D6

Postby Groguigui » Fri Apr 21, 2017 1:18 pm

It is exactly what I did, but this message appear :
*ERROR reading *SHELL SECTION: *SHELL SECTION can only be used for shell elements.
Elemenrt 11 is not a shell element.

But I don't understand totally if I must use *Shell Section or *Solid Section.
http://www.dhondt.de/ccx_2.12.pdf p445 :
*SHELL SECTION
Keyword type: model definition
This option is used to assign material properties to shell element sets. The parameter ELSET is required, one of the mutually exclusive parameters MATERIAL and COMPOSITE is required too, whereas the parameters ORIENTATION, NODAL THICKNESS, OFFSET are optional. The parameter ELSET
defines the shell element set to which the material specified by the parameterMATERIAL applies. The parameter ORIENTATION allows to assign local axes to the element set. If activated, the material properties are applied to the local axis. This is only relevant for non isotropic material behavior. The parameter NODAL THICKNESS indicates that the thickness for ALL nodes in the element set are defined with an extra *NODAL THICKNESS card and
that any thicknesses defined on the *SHELL SECTION card are irrelevant.
*SHELL SECTION
•Enter any needed parameters.
Second line if the parameter COMPOSITE is not used (only read if the first line does not contain NODAL THICKNESS):
•thickness
Second line if the parameter COMPOSITE is used (NODAL THICKNESS is not allowed):

If I understand, it is possible to simulate with shell elements in both cases :
This option is used to assign material properties to 3D, plane stress, plane strain, axisymmetric and truss element sets. The parameters ELSET and MATERIAL are required, the parameter ORIENTATION is optional
. The parameter ELSET defines the element set to which the material specified by the parameter MATERIAL applies. The parameter ORIENTATION allows to assign local axes to the element set. If activated, the material properties are applied to the local axis. This is only relevant for non isotropic material behavior. For plane stress and plane strain elements the thickness can be specified on the second line. Default is 1.
First line:
•*SOLID SECTION
•Enter any needed parameters.
Second line (only relevant for plane stress, plane strain and truss elements; can be omitted for axisymmetric and 3D elements):
• thickness for plane stress and plane strain elements, cross-sectional area for truss elements.


But my question is, the Error File provided is by Calculix or FreeCAD?

EDIT :
Currently, Calculix run because I wrote "planestress" in *Solid Section line.
*ERROR : increment size smaller than minimum best solution and residuals are in the frd file.
So, that is interesting.
ulrich1a
Posts: 1406
Joined: Sun Jul 07, 2013 12:08 pm

Re: Element Membrane M3D6

Postby ulrich1a » Sat Apr 22, 2017 2:25 pm

After a little experimenting, I got a working calculix-file from an Abaqus-example. It has only M3D3 elements, but will give a start. I had to define the membrane thickness with *NODAL THICKNESS.

Ulrich

Code: Select all

*HEADING
: MEMBRANE LOADING  [M3D3]
*NODE, NSET=Nall
 1, 0.0, 0.0
 2, 2.0, 0.0
 3, 2.0, 1.0
 4, 0.0, 1.0
*NODAL THICKNESS
Nall, 1.0
*ELEMENT,TYPE=M3D3, ELSET=EALL
 1, 1,2,3
 2, 1,3,4
*SOLID SECTION,MATERIAL=A1, ELSET=EALL
 1.0,
*MATERIAL,NAME=A1
*ELASTIC,TYPE=ISOTROPIC
 30.0E6,0.3
*BOUNDARY
 1,1,3
 2,2,3
 3,3
 4,3
*STEP
*STATIC
*CLOAD
 2,1,  500.0
 3,1, -1500.0
 3,2, -1500.0
 4,1, -500.0
 4,2, -500.0
*ELEMENT OUTPUT
S,
E,
*OUTPUT,FREQUENCY=1
*NODE OUTPUT
U
*NODE PRINT, NSET=Nall
U
*EL PRINT, ELSET=EALL
 S,
 E,
*END STEP