#1 2020-06-18 07:47:10

KevinTse

Member

From: Winnipeg, MB, Canada

Registered: 2020-05-13

Posts: 11

How to do these options in ParaVis

Hi every one, I just see an example about the analysis in my topic, but how I can do the options like it shows in the picture(e.g. LOADED, DISPLACEMENT) I find a lot of time reading ParaViewTutorial 56.pdf but cannot find what exactly it is.

Here is the code in Aster study:
DEBUT(LANG='EN')

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

model = AFFE_MODELE(AFFE=_F(GROUP_MA=('ElmCL', 'ElmBeam'),
                            MODELISATION=('POU_D_E', ),
                            PHENOMENE='MECANIQUE'),
                    MAILLAGE=mesh)

elemprop = AFFE_CARA_ELEM(MODELE=model,
                          POUTRE=_F(CARA=('HY', 'HZ'),
                                    GROUP_MA=('ElmCL', 'ElmBeam'),
                                    SECTION='RECTANGLE',
                                    VALE=(140.0, 50.0)))

TimbISO = DEFI_MATERIAU(ELAS=_F(E=11000.0,
                                NU=0.35))

fieldmat = AFFE_MATERIAU(AFFE=_F(MATER=(TimbISO, ),
                                 TOUT='OUI'),
                         MODELE=model)

BC = AFFE_CHAR_MECA(DDL_IMPO=_F(DRX=0.0,
                                DRY=0.0,
                                DRZ=0.0,
                                DX=0.0,
                                DY=0.0,
                                DZ=0.0,
                                GROUP_NO=('Support', )),
                    MODELE=model)

Load = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=290.0,
                                  GROUP_NO=('NdForce', 'NdTOP')),
                      MODELE=model)

reslin = MECA_STATIQUE(CARA_ELEM=elemprop,
                       CHAM_MATER=fieldmat,
                       EXCIT=(_F(CHARGE=BC),
                              _F(CHARGE=Load)),
                       MODELE=model)

reslin = CALC_CHAMP(reuse=reslin,
                    FORCE=('REAC_NODA', 'FORC_NODA'),
                    RESULTAT=reslin)

NdSPfrc = POST_RELEVE_T(ACTION=_F(GROUP_NO=('SupA', ),
                                  INTITULE='Node_Supp',
                                  MOMENT=('DRX', 'DRY', 'DRZ'),
                                  NOM_CHAM='REAC_NODA',
                                  OPERATION=('EXTRACTION', ),
                                  POINT=(0.0, 0.0, 0.0),
                                  RESULTANTE=('DX', 'DY', 'DZ'),
                                  RESULTAT=reslin))

IMPR_RESU(RESU=_F(CARA_ELEM=elemprop,
                  RESULTAT=reslin),
          UNITE=80)

IMPR_TABLE(TABLE=NdSPfrc,
           UNITE=8)

FIN()

---

Attachments:
7.png, Size: 148.24 KiB, Downloads: 225

sb1966

Member

From: INDIA

Registered: 2015-03-16

Posts: 262

Re: How to do these options in ParaVis

Hi,
If I have understood your problem correctly:

1. First save your results in a med file (.rmed)
2. Open it in Paravis.
3. Apply the filter 'Warp by Vector'
4. Now you would be able to see the deformed shape.

5. It will be easier to understand how to do it, if you see some video tutorial. Plenty of good ones are there in youtube.

Hope this helps.

Regards.

Sukumar

KevinTse

Member

From: Winnipeg, MB, Canada

Registered: 2020-05-13

Posts: 11

Re: How to do these options in ParaVis

Hi,
If I have understood your problem correctly:

1. First save your results in a med file (.rmed)
2. Open it in Paravis.
3. Apply the filter 'Warp by Vector'
4. Now you would be able to see the deformed shape.

5. It will be easier to understand how to do it, if you see some video tutorial. Plenty of good ones are there in youtube.

Hope this helps.

Regards.

Sukumar

sorry I found that 'Warp by Vector' doesn't suitable on 1d elements

---

Attachments:
9.png, Size: 129.63 KiB, Downloads: 213

dezsit

Member

Registered: 2012-06-27

Posts: 69

Website

Re: How to do these options in ParaVis

Hi,

Warp by Vector can do that, but you need a real vector with 3 elements!
In case of beams you have 6 in the DEPL filed: 3 translation 3 rotation, so you should produce a real vector from that.
You have two options to do that
1) the easy way: when you open your med file and select your filed (e.g. depl of course) , you have to tick the checkbox "Generate vectors"  (just below the field selection window). This will generate a new DEPL field (DEPL_Vector or something) what will contain the 3 necessary directional displacements, and can be used by Warp filter

2) the manual way: use the calculator filter, then apply the following expression: ihat*DX + jhat*DY + khat*DZ (DX,DY,DZ is the scalars of your DEPL filed),
this will produce a new vector field with 3 components under the name you provides in the Calculator filter (by default it is Result).

Note: you should use one of the option in any case where the DEPL field contains more than 3 directional displacement, so e.g. in case of shells, or if you use contacts.

Best regards,
dezsit

sb1966

Member

From: INDIA

Registered: 2015-03-16

Posts: 262

Re: How to do these options in ParaVis

Hi KevinTse,

Dezsit wrote:

1) the easy way: when you open your med file and select your filed (e.g. depl of course) , you have to tick the checkbox "Generate vectors"  (just below the field selection window). This will generate a new DEPL field (DEPL_Vector or something) what will contain the 3 necessary directional displacements, and can be used by Warp filter

This is what I tried to point you out through point no 5 in my earlier reply. Dezsit has given already a beautiful reply. If it has solved your issue, kindly mark it as solved by adding "[SOLVED]" at the beginning of topic heading. such marking is helpful for the community.

Sukumar