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

You are not logged in.

#1 2020-02-21 03:36:53

xupeiwust
Member
Registered: 2020-02-21
Posts: 14

Error when using force_face

when I use force_face to load a force to a Group_MA(3d element),I get the following error:
FIN()
# ------------------------------------------------------------------------------------------
JDC.py : ERREUR WITH THE EXECUTION - INTERRUPTION
>> JDC.py: DEBUT CR of execution of JDC in MIXTE
   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
   ! <S> Exception user raised but not interceptee.                      !
   ! The bases are fermees.                                              !
   ! Type of the exception: error                                        !
   !                                                                     !
   !  les 25 mailles imprim??es ci-dessus n'appartiennent pas au mod??le !
   !  et pourtant elles ont ??t?? affect??es dans le mot-cl?? facteur :  !
   ! FORCE_FACE                                                          !
   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
fine CR of execution of JDC in MIXTE

REPORT
>> JDC.py: FIN REPORT


What is the reason?  thank you

Offline

#2 2020-02-22 03:20:57

xupeiwust
Member
Registered: 2020-02-21
Posts: 14

Re: Error when using force_face

help  help

Offline

#3 2020-02-22 15:52:46

mf
Member
Registered: 2019-06-18
Posts: 117

Re: Error when using force_face

Hello,

the error says, that you tried to address a group in your FORCE_FACE command that is not present in your model. Maybe you forgot a group? If you created your groups in the geometry module, did you import them to your mesh also ('create groups from geometry'-command in Salome)? Did you enter the group names in Aster by hand (typo)?

Bye,

Mario.

Offline

#4 2020-02-23 03:17:31

xupeiwust
Member
Registered: 2020-02-21
Posts: 14

Re: Error when using force_face

Thank you for your answer. I'm analyzing in salomemeca. There is only one component. When I use everything when setting the unit and material, the calculation is no problem, but when I use the group to set the material and unit, this problem occurs. I actually have a face group in my part

Offline

#5 2020-02-23 10:24:07

AsterO'dactyle
Administrator
Registered: 2007-11-29
Posts: 342

Re: Error when using force_face

Hello,


When computing surfacic forces, you need skin elements in you model (integral … )

In your AFFE_MODELE, use TOUT='OUI' or GROUP_MA = ('Volumic', 'SkinForce') where 'SkinForce' is the group you used in AFFE_CHAR_MECA/FORCE_FACE


Code_Asterの開発者

Offline

#6 2020-07-29 11:17:18

zhuge000
Member
Registered: 2020-07-01
Posts: 3

Re: Error when using force_face

AsterO'dactyle wrote:

Hello,


When computing surfacic forces, you need skin elements in you model (integral … )

In your AFFE_MODELE, use TOUT='OUI' or GROUP_MA = ('Volumic', 'SkinForce') where 'SkinForce' is the group you used in AFFE_CHAR_MECA/FORCE_FACE

I have tried, but still can't run the model, some error about Force_Face. Could you help me to check the code below? Thank you!

=============================================
mesh = LIRE_MAILLAGE(FORMAT='MED',
                     UNITE=20)

model = AFFE_MODELE(AFFE=_F(MODELISATION=('3D', ),
                            PHENOMENE='MECANIQUE',
                            TOUT='OUI'),
                    MAILLAGE=mesh)

mater = DEFI_MATERIAU(ELAS=_F(E=210000000000.0,
                              NU=0.3))

materfl = AFFE_MATERIAU(AFFE=_F(MATER=(mater, ),
                                TOUT='OUI'),
                        MODELE=model)

mecabc = AFFE_CHAR_MECA(DDL_IMPO=_F(GROUP_MA=('fix', ),
                                    LIAISON='ENCASTRE'),
                        MODELE=model)

mecach = AFFE_CHAR_MECA(FORCE_FACE=_F(FZ=-10000.0,
                                      GROUP_MA=('load', )),
                        MODELE=model)

result = MECA_STATIQUE(CHAM_MATER=materfl,
                       EXCIT=(_F(CHARGE=mecabc),
                              _F(CHARGE=mecach)),
                       MODELE=model)

IMPR_RESU(FORMAT='MED',
          RESU=_F(RESULTAT=result),
          UNITE=2)
===========================================

Offline

#7 2020-08-12 00:05:48

AsterO'dactyle
Administrator
Registered: 2007-11-29
Posts: 342

Re: Error when using force_face

Check if skin elements  of GROUP_MA='load' have been affected by AFFE_MODELE


Code_Asterの開発者

Offline

#8 2020-08-12 20:28:43

sb1966
Member
Registered: 2015-03-16
Posts: 178

Re: Error when using force_face

Hi,

1. Did you export the groups from Geometry to the mesh?
2. Or did you create the group (of FACE as you mentioned) in the mesh?
3. You may check whether your Groups exist in the mesh or not by looking at the object viewer in the mesh module.
4. Alternatively you may check your message file. It should record all the groups you created after the LIRE_MAILLAGE command.
5. It is best to upload your files, including the .mess file to get appropriate help from the forum.

Hope this helps.

Regards.

Sukumar

Offline

#9 2020-08-24 11:20:49

Kidbooo
Member
Registered: 2019-03-28
Posts: 5

Re: Error when using force_face

the error says, that you tried to address a group in your FORCE_FACE command that is not present in your model. Maybe you forgot a group? If you created your groups in the geometry module, did you import them to your mesh also ('create groups from geometry'-command in Salome)? Did you enter the group names in Aster by hand (typo)?

Offline

#10 2020-08-30 06:04:06

zhuge000
Member
Registered: 2020-07-01
Posts: 3

Re: Error when using force_face

I have uploaded my model file(hdf file), it is a very simple model, just a 3D beam model, and I'm sure there are "fix" and "load" mesh face groups(not geometry face groups). I have try it in Salome Meca 2018 and 2019 both in windows(7 and 10) and linux(ubuntu 18.04).  It always show me the FORCE_FACE error.


Attachments:
beam2018_3D.hdf, Size: 224.35 KiB, Downloads: 32

Offline

#11 2020-08-30 14:03:48

mf
Member
Registered: 2019-06-18
Posts: 117

Re: Error when using force_face

Hi,

you are adressing a group 'Volumic' in your FORCE_FACE command. This group is not present in your mesh, I assume it is an old group from a previous calculation? In this case you have to remove it 'by hand' (remove text at the bottom in FORCE_FACE under 'Manual Selection') in AsterStudy.

Another error: CALC_CHAMP shall have the same name as MECA_STATIQUE (click on 'reuse input object' or type the same name in by hand).

I had to remesh, apparently we are using different versions of SM?

After these corrections, your example should work.

Mario.


Attachments:
corrected.zip, Size: 199.39 KiB, Downloads: 32

Offline

#12 2020-08-30 17:46:32

zhuge000
Member
Registered: 2020-07-01
Posts: 3

Re: Error when using force_face

mf wrote:

Hi,

you are adressing a group 'Volumic' in your FORCE_FACE command. This group is not present in your mesh, I assume it is an old group from a previous calculation? In this case you have to remove it 'by hand' (remove text at the bottom in FORCE_FACE under 'Manual Selection') in AsterStudy.

Another error: CALC_CHAMP shall have the same name as MECA_STATIQUE (click on 'reuse input object' or type the same name in by hand).

I had to remesh, apparently we are using different versions of SM?

After these corrections, your example should work.

Mario.

Thanks for your answer! I can run the model now!

But I can't change the CALC-CHAMP name to the same as MECA_STATIQUE, the Analysis command will turn red. And I still can run the model without change its name.

And I find that if I set Model Definition by "Group of element" and select a 3D element mesh group, the FORCE_FACE error will happen. If I set it by "Everywhere", the model will run without errors.

Offline