Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2006-09-28 19:11:30

Jm B
Guest
Registered: 2007-11-20
Posts: 0

Understanding the FORCE_FACE command

Hello all,

I am using the following boundary conditions in a 3D hexahedron meshed model that is in millimeters.  The cross sectional area of the face "Load" that is being loaded by the FORCE_FACE command is 3500 sq. mm.  Ignore the FACE_IMPO command, since it is fixing (encastering) the faces belonging to a group named "Fixed".

BCnd=AFFE_CHAR_MECA(MODELE=FEMLin,
                    FACE_IMPO=_F(GROUP_MA='Fixed',
                                 DX=0.0,
                                 DY=0.0,
                                 DZ=0.0,),
                    FORCE_FACE=_F(GROUP_MA='Load',
                                  FY=10,),);

Will the total force applied to the model be 10N x 3500 = 35,000N?  I am asking a very basic question, but I have come to this point because I am questioning my understanding (or my sanity) after running an analysis that is not giving the right results &  I want to figure out why.

Thanks for any help
JMB

Offline

#2 2006-09-28 19:24:57

Pagé MICHAËL
Guest
Registered: 2007-11-20
Posts: 0

Re: Understanding the FORCE_FACE command

Hi JMB,

Yes, you're right, the force applied to a face with the command FORCE_FACE is not really a force, but a pressure. So, when you say :

FORCE_FACE=_F(GROUP_MA='Load',
FY=10,),);

In reality FY = 10 MPa (in your case because you work in mm and N).

I already asked for a manner to put a force in N, but there is no way at this moment.

Also, FORCE_ARRETE is a force by lenght unit (N/mm for example).

MP

Offline

#3 2011-11-10 17:10:06

vic
Member
Registered: 2011-07-20
Posts: 28

Re: Understanding the FORCE_FACE command

Hello,

It looks like very simple question but I'm not sure and don't know how to check it quickly.

Does it mean that the

 BCnd=AFFE_CHAR_MECA(MODELE=...,
                   ... 
                   FORCE_FACE=_F(GROUP_MA='Load',
                                  FY=10,),);

sets stresses SigmaYY=10 on face 'Load' ?

or it depends on location of the face relative to the axis ?

thanks,
Vic.


Pimeca C_A 10.3 for Windows, Salome-Meca 2010

Offline

#4 2011-11-11 02:05:10

JMB365
Member
Registered: 2008-01-19
Posts: 781

Re: Understanding the FORCE_FACE command

Hello vic,

The FY=10.0 is with respect to the global co-ordinate system.

Regards, JMB


SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

#5 2011-11-11 09:28:15

kamil
Member
Registered: 2010-07-05
Posts: 60

Re: Understanding the FORCE_FACE command

Hi JMB,

I use that as Force applied/area of surface. I divide the force by area and I get the pressure. If that was a pressure there wouldn't be a command of applying pressure on a Group_Ma= 2D facial...... Now I am confused.

I think code aster- salome meca needs a module to visualise the previews of such operations as ansys or abaqus does. Not to apply just to preview the effects for the start.

Furthermore, I have a different question for you JMB

When I looked to the code fragment, I have seen you used FACE_IMPO in order to encaster a face of  a 3D solid (lower face I presume).

There is also DDL IMPO- Encastre option, I generally use that option. Is there any significant difference between them ? you can look to my mess file uplodaded there
http://www.code-aster.org/forum2/attach … ?item=4966.  ( you can also see that I use sometimes Force_Face for an indentation experiment )

Thanks in advance ,

regards,

Kamil

Offline

#6 2011-11-11 10:11:31

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,829

Re: Understanding the FORCE_FACE command

hello

FORCE_FACE will apply a force per unit area in the global axis direction
PRES_REP will apply a pressure, normal to the surface, beware of the normal direction!
have a look at U4.44.01

kamil wrote:

I think code aster- salome meca needs a module to visualise the previews of such operations as ansys or abaqus does. Not to apply just to preview the effects for the start. l

humm, yes!!


kamil wrote:

When I looked to the code fragment, I have seen you used FACE_IMPO in order to encaster a face of  a 3D solid (lower face I presume).
There is also DDL IMPO- Encastre option, I generally use that option. Is there any significant difference between them ?

you should do a bit of experiment with that
remember that 3D elements do not know rotational DOF!

jean pierre aubry


consider reading my book
freely available here https://framabook.org/beginning-with-code_aster/

Offline

#7 2011-11-11 11:03:09

vic
Member
Registered: 2011-07-20
Posts: 28

Re: Understanding the FORCE_FACE command

Hello

I don't understand the following

usually FX (or FY) has dimension [N] (like a force)

but in this case it has [N * m * m] = [Pa] . So it might be analog of pressure or stress, not a force.

I made some test calculations. Plate fixed at 'bottom' and FORCE_FACE applied to 'med' section or to 'top' face.
'med' section divides plate at angle 45 degrees. (img attached)

CH_M1 = AFFE_CHAR_MECA(MODELE = MODEL_M,
                 FORCE_FACE=(_F(GROUP_MA='top',
                              FY=100.E6,),),);


CH_M2 = AFFE_CHAR_MECA(MODELE = MODEL_M,
                 FORCE_FACE=(_F(GROUP_MA='med',
                              FY=100.E6,),),);

DISPL1 =MECA_STATIQUE(MODELE=MODEL_M,
                      CHAM_MATER=MATER_M,
                      EXCIT=(_F(CHARGE=CLIM_M,),
                             _F(CHARGE=CH_M1,),)
                    );

DISPL2 =MECA_STATIQUE(MODELE=MODEL_M,
                      CHAM_MATER=MATER_M,
                      EXCIT=(_F(CHARGE=CLIM_M,),
                             _F(CHARGE=CH_M2,),)
                    );

in the first case I have received that in the body we have Syy=100 MPa . So Fy corresponds to Syy
in the second case we see that Syy=Fy / cos(45).

But I need to apply stresses as boundary condition. Is it possible to find easy way to calculate angles between face and global coordinate system?

Vic

Last edited by vic (2011-11-11 11:38:08)


Attachments:
syy-test.png, Size: 40.79 KiB, Downloads: 358

Pimeca C_A 10.3 for Windows, Salome-Meca 2010

Offline

#8 2011-11-11 11:17:03

Johannes_ACKVA
Member
From: Ingenieurbüro für Mechanik, DE
Registered: 2009-11-04
Posts: 753
Website

Re: Understanding the FORCE_FACE command

Hi all together,

I think there is some 'logic' in the naming of the types of loads (even
sometimes it remains unlogic). Let me try:

The dimension of a load follows from its name:

FORCE_NODAL -> force per node -> N/-  (a node has no dimension)
FORCE_FACE    -> force per face  -> N/m2
FORCE_ARETE    -> force per edge  -> N/m
FORCE_CONTOUR    -> force per contour-length  -> N/m
FORCE_POUTRE    -> force per beam-length -> N/m

The first part of the name (FORCE_) indicates that You will have to specify
components (at least one from DX, DY, DZ, DRX, DRY, DRZ). Since there is no
other, this is done in the global CS. Components are needed because a FORCE_* is
a vector.

In some of the FORCE_* loads  (those which are applied to elements having a
local coordinate system) You have the choice to specify the components
in the gobal CS (at least one from FX, FY, FZ) or in the
local CS of the element (at least one from N, VY, VZ). This is possible for

FORCE_POUTRE    -> force per beam-length -> N/m in global or local CS
FORCE_COQUE    -> force per area-of-shell -> N/m2 in global or local CS


The "non_FORCE_loads" take there dimensionality often from their 'nature',
for example

PRES_REP distributed pressure. Pressure -> N/m2

and take their direction from the orientation of the elements (PRES_REP acts
normal to a face and not inclined as You can do with FORCE_FACE)


Well, what I am telling seems is not true for FORCE_TUYAU, where a pressure has
to be specified. I would like to rename it to PRES_TUYAU

Regards,
Johannes Ackva
______________________________________________________________________
Ingenieurbüro für Mechanik
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen

______________________________________________________________________
next CODE-ASTER-courses organized by Ingenieurbüro für Mechanik

*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, 30th Nov - Sat 3rd Dec 2011

*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Thursday 26th to Friday 27th January 2012

Registration forms are here:
http://www.code-aster.de/index.php?opti … Itemid=110

*** PYTHON with CODE-ASTER course in preparation


Ingenieurbüro für Mechanik
D 91717 Wassertrüdingen / Germany

www.code-aster.de                                                Training & Support for NASTRAN and CODE-ASTER

Offline

#9 2011-11-11 15:43:29

vic
Member
Registered: 2011-07-20
Posts: 28

Re: Understanding the FORCE_FACE command

Hi all again,

Is it possible to set stresses as boundary conditions in following steps:

to create a copy of initial mesh (M2)
to set pressure as boundary condition on mesh M2
to extract x-component of pressure using PROJ_CHAMP (or similar) from mesh M2 to initial mesh M1

sorry if my questions are incorrect or stupid.


Vic


Pimeca C_A 10.3 for Windows, Salome-Meca 2010

Offline

#10 2011-11-11 16:10:12

Johannes_ACKVA
Member
From: Ingenieurbüro für Mechanik, DE
Registered: 2009-11-04
Posts: 753
Website

Re: Understanding the FORCE_FACE command

Vic, In Your steps:

a) to create a copy of initial mesh (M2)
b) to set pressure as boundary condition on mesh M2
c) to extract x-component of pressure using PROJ_CHAMP (or similar) from mesh M2 to initial mesh M1

In step b) the pressure is a Code-Aster concept of type 'load'

But in step c), command PROJ_CHAMP needs a concept of type 'resultat' or of type 'champ' (field) to take a field from and project it.  Such concept  ('resultat' or  'champ') is normally obtained by doing an analysis (MECA_STATIQUE, STAT_NON_LINE etc, followed eventually by CALC_ELEM, CALC_NO etc). So this analysis must be done between b) and c). After the analysis You can PROJ_CHAMP only those fields which are contained in Your concept of type 'resultat'. These are displacements (DEPL), Gauss-point-stresses (SIEF_ELGA), etc. All fields are referred to the nodes (nodal fields like DEPL) or to the elements (SIGM_ELNO for example) of the model. The pressure onto some faces of You model is not such a field in a concept of type 'resultat'.

Maybe there is another way for You to do what You want, but You should explain it better.

Regards,
Johannes Ackva
______________________________________________________________________
Ingenieurbüro für Mechanik
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen

______________________________________________________________________
next CODE-ASTER-courses organized by Ingenieurbüro für Mechanik

*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, 30th Nov - Sat 3rd Dec 2011

*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Thursday 26th to Friday 27th January 2012

Registration forms are here:
http://www.code-aster.de/index.php?opti … Itemid=110

*** PYTHON with CODE-ASTER course in preparation


Ingenieurbüro für Mechanik
D 91717 Wassertrüdingen / Germany

www.code-aster.de                                                Training & Support for NASTRAN and CODE-ASTER

Offline

#11 2011-11-14 11:28:30

vic
Member
Registered: 2011-07-20
Posts: 28

Re: Understanding the FORCE_FACE command

Dear Johannes,

thank you for explanation. I felt that I'm wrong but didn't know where.

I'd like to determine displacements and stress intensity factors at the defined points in prestressed material after removing some part of the object tested.
(picture a)

To model stressed state I want to replace removing of material by applying of stresses at new appeared surfaces (after cutting the material). Residual stresses (black arrows) after making a notch induces displacements the same as stresses applied to the free surface (blue arrows)
(pictures b, c )

So I need to set initial stresses on the surfaces A.

I can use PRES_REP or FORCE_FACE if form of notches is simple. But above mention functions are not possible to use directly in more complex situation when notches are created by drill tool with a conical form or others.

So I'm looking for way to set stresses SigmaXX as boundary conditions on chosen surfaces.

Maybe it is possible to find angles between axis OX and face on which required to apply stresses SigmaXX. After this use cos(angle) and FORCE_FACE to set stresses.


Attachments:
notch1.jpg, Size: 87.16 KiB, Downloads: 469

Pimeca C_A 10.3 for Windows, Salome-Meca 2010

Offline