[SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

DarrenY · 2012-05-02 20:17:46

Hi,

I followed Jean Pierre Aubry's tutorial and attempted to create the model and analysis
(http://www.caelinux.org/wiki/images/6/6 … -aster.pdf).

Attached are the COMM, MED, HDF, MESS files.

When I ran the analysis I encountered EXIT CODE=139 and the code exited after trying to write the mesh. I've divided the topbeam into smaller groups but otherwise stayed true to the tutorial. I've tried multiple ways to represent the geometry from following the GMSH method described in the tutorial to drawing the geometry in Salome (GEOM) but I can't find a cure. The MESS file doesn't provide further information and I can't seem to figure out the problem.

In looking through the Forum regarding Exit Code 139 I see that this can relate to the installation and segmentation. There's also reference to a particular problem with 0D and 1D elements.

I'm using Codes Aster STA11.0, Salome Meca 6.4.0, 64-bit, Oracle VM Virtual Box 4.1.8, Ubuntu 10.04.03, CAELinux 2011.

Any help in getting this to run would be appreciated.

Regards,
- Darren

Last edited by DarrenY (2013-01-30 04:56:00)

Attachments:
port1_120502_1311_DY.zip, Size: 48.96 KiB, Downloads: 452

jeanpierreaubry · 2012-05-03 07:18:26

hello

when i run your files in 10.6 i get this error somewhat later in the .comm file

    #  COMMANDE NO :  0006            CONCEPT DE TYPE : cham_mater
    #  -------------                  ----------------- 
   material=AFFE_MATERIAU(INFO=1,
                         MAILLAGE=mesh,
                         AFFE=_F(MATER=steel,
                                 GROUP_MA=('mast','topbeam',)),
                         );

   
   !-----------------------------------------------------------!
   ! <EXCEPTION> <MODELISA7_77>                                !
   !                                                           !
   ! le GROUP_MA  mast  ne fait pas partie du maillage :  mesh !
   !-----------------------------------------------------------!

this means you try to assign a material to non existing groups
it looks like you did not finish adapting the .comm to your meshing

for the main problem it looks like being a window$ separator or end of line problem
may be you downloaded or edited some files under window$ and try to run them directly
try running dos2unix on the files
even the med file seems to be corrupted,
i cannot open it in Gmsh but i can in Salome
running xmdump3 detect a corrupted file
how did you create this file ?

jean pierre aubry

Thomas DE SOZA · 2012-05-03 10:15:35

DarrenY wrote:

When I ran the analysis I encountered EXIT CODE=139 and the code exited after trying to write the mesh. I've divided the topbeam into smaller groups but otherwise stayed true to the tutorial. I've tried multiple ways to represent the geometry from following the GMSH method described in the tutorial to drawing the geometry in Salome (GEOM) but I can't find a cure. The MESS file doesn't provide further information and I can't seem to figure out the problem.

There's a bug in 10.5 version when reading 1D meshes. Update to 10.6 version to fix it.

TdS

DarrenY · 2012-05-04 20:27:30

Hi,

Thanks for your responses.

Jean Pierre, the MED file is exported from Salome-Meca. The geometry is drawn in the geometry module in this manner:
- drew vertices (numbered 1 to 7)
- drew lines between the vertices (Line 1 to 7)
- used the BUILD command to create a wire with the lines (this became 'gswing')
- used the EXPLODE command to create the subgroups of geometry for nodes and edges.

In the mesh module I created the mesh as follows:
- created the mesh with 1D elements using a local length of 100 (this created 40 elements)
- created groups based on the exploded geometry (from the geometry module)

Afterward, I exported the mesh to a MED file.

The COMMAND file I created in Efficas. (I'm still not comfortable enough with the code and options to work in a text editor alone.)

I started with GMSH as described in the tutorial but ran into difficulties so I turned to Salome-Meca because to this point I've learned more about the Salome-Mecas based modules through the tutorials. I'll return to GMSH in the future to learn more. It sounds like you prefer using GMSH and there is merit in using this meshing software. Is GMSH a better choice?

As Thomas indicates CAELinux 2011 is running Code Aster STA10.5. Due to constraints IT-wise in my office, I'll probably have to wait until a STA10.6 or higher stable version is available in CAELinux. I'm running a Linux virtual machine in Windows which is not entirely allowed under our IT confines.

From Jean Pierre's description, there may have been some unusual characters in the COMMAND file. I believe I made a mistake by copying the remarks in the tutorial PDF into the EFFICAS command file and may have added some hidden characters in copying between Windows and Linux. I've re-created the COMMAND file purely in EFFICAS without remarks and cross-copying. The revised files are attached.

As Jean Pierre indicated, the 'topbeam' and 'mast' groups don't exist since I discretized the top beam into smaller lengths. I'm embarrassed that I missed that one. It was obvious once you pointed it out.

From the ASTK GUI (still from CAELinux 2011), I attempted to use Code Aster NEW11.0 but had the same result (Exit Code = 139 plus Abnormal Abort = 1) so I suspect that the bug that doesn't allow 1D elements might have been in both versions STA10.5 and NEW11.0 in CAELinux 2011.

Though I haven't been able to successfully run the model, I found the tutorial descriptions alongside the code to be helpful.

If and when I do get this tutorial running I'll re-post. I've attached current HDF, COMM, MED, MESS, EXPORT files for the attempted runs through Salome Meca (Sta10.5) and the ASTK GUI (NEW11.0) labelled with 'v11' in the names. Meantime, I'll wait for a bug-free stable version in CAELinux.

Regards,
- Darren

Attachments:
port1_120503_1606_DY.zip, Size: 40 KiB, Downloads: 431

jeanpierreaubry · 2012-05-05 09:08:03

hello

first point
it is not a good practice to blame the software or the versions about such or such a point before fully understanding what is happening!

second point
what was happening is that the discret element 'nmass_5' was not given properties in AFFE_CARA_ELEM
in addition it looks like that Salome meshing (or rather, your Salome meshing) produced only a node at this location and not an element
so we have to create one
all this, with some other errors is corrected in the attached file
there are some comments in it

jean pierre aubry

Attachments:
COMM_port1_120503_1606_DY.comm, Size: 7.75 KiB, Downloads: 577

DarrenY · 2012-05-07 18:40:15

Hi Jean Pierre,

Thank you.

I can see where I'm a prime candidate for your quote in the tutorial (Section 13, page 31):

"...our ingeniousness in raising errors does not seem to have any limit."

I think that's a good one.

I readily admit that there are items that I don't fully understand. That's the main reason why I'm trying to complete this tutorial so that I can understand. It all seems rather basic so I can't see why it's not working. I'm just a bit distressed that if I can't make these simple examples work that I won't be able to succeed with more intricate work.

I've used the corrected COMM file (I appreciate your added comments to help me understand). The last IMPR_RESU command for the output MED file I've changed as recommended. I've attached data from two different versions that I ran. For the _0941_ version, I changed the commented lines relating to IMPR_RESU and the output MED file using the text editor called 'medit' (part of the CAELinux package). For the _1016_ version, I used EFFICAS and entered the new IMPR_RESU command (that was to be uncommented) and deleted the original command (that was to be commented). I tried to run these in Salome Meca (Aster Module) STA10.5 and in ASTK NEW11.0 but without success. I didn't change anything else in the COMM or MED files.

The lack of a 0D element makes sense for 'nmass_5'. When I meshed in Salome I only set mesh parameters for 1D elements and I didn't set any 0D elements. (Since no loads are applied to the other nodes we don't have to define a mesh at these nodes. Correct?)

If these run for you, I'm at a loss and there's something wrong at my end. The only other thing I can think of is that I need to follow Thomas' recommendation and move to STA10.6.

Thanks again for your help.

Regards,
- Darren

Attachments:
port1_v11_120507_0941_and_1016_DY.zip, Size: 89.77 KiB, Downloads: 439

jeanpierreaubry · 2012-05-08 08:20:36

hello

first
i can run your two sets med and comm either with 10.06.05 or 11.1.15
second
when i try to open the med files with Gmsh nothing seems to be loaded
however when i run xmdump on your med files all seems ok
maybe TdS is having an idea about what is going on!

try installing 10.6 and see what happens

comments about IMPR_RESU were just about details
about 'nmass_5' you must grasp the difference between nodes and point elements

last thought, with 10.5
try commenting all the IMPR_TABLE, see what happens,
then try using only one,
then only two

jean pierre aubry

Last edited by jeanpierreaubry (2012-05-08 08:37:36)

DarrenY · 2012-05-08 17:26:02

Hi,

Thanks, Jean Pierre. That's good news on several fronts.

I'll find a way to install STA10.6. I need to modernize to this next stable version.

Yes, the facets of meshing you've cleared up for me now. From the user guide I see where:

- 'Node' is a 0D object of a mesh presented by a point with coordinates

and

- '0D Element' is an element of a mesh defined by one node.

I'll try your suggestion of commenting IMPR_TABLE in 10.5

Regards,
- Darren

Johannes_ACKVA · 2012-12-04 12:39:44

Hi Darren,
I have just some remarks for You:

(1) it is quite typic for the way of CodeAster thinking to do things with Aster-commands if possible instead of using a Pre-/Postprocessor. So creating 0D-elements is easier done in .comm with this 1-line-command
- mesh=CREA_MAILLAGE(MAILLAGE=mesh1, CREA_POI1=_F(GROUP_NO='nmass_5',NOM_GROUP_MA='nmass_5',),);
More of such examples:
- changing from linear to quadratic elements: CREA_MAILLAGE(...LINE_QUAD=...
- check and revert face-element-normals: MODI_MAILLAGE(... ORIE_PEAU_3D=...
- creating tables with sorting, averaging, envelopping features
- many more..
This "philosophy" distinguishes Code-Aster from the many other FE-Codes and makes it so smart.

(2) On Your OS CAELinux2011 You can easily install the newest SalomeMeca2012.2 from here:
http://www.code-aster.org/V2/spip.php?article303

Best regards,

Johannes_ACKVA

next CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany

*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, Monday 28th Jan - Thursday 31 Jan 2013

*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Monday 08 to Tuesday 09 April 2013

DarrenY · 2012-12-10 18:19:55

Hi Johannes,

Thanks for your help.

I was successful in installing the latest version of Salome Meca (2012.2) onto the CAELinux 2011 operating system.

Attached are my notes on how I did it, in case it may help someone else.

Just one more question regarding the downloads: Under Downloads on the website, what are the Sources listed as Aster Module of Salome-Meca 2012.2? Is this the Aster Module as a standalone that is included in the Salome-Meca complete package?

Regards,
- Darren

Last edited by DarrenY (2012-12-10 18:36:29)

Attachments:
01_Install_Salome_Meca_on_CAELinux_OS_121210_1050_DY.zip, Size: 533.68 KiB, Downloads: 610

DarrenY · 2012-12-23 03:48:27

Hi,

I've managed to complete Jean Pierre's example to the point that I have Exit Code=0 (no longer =139). It ran properly with Code Aster 10.7 from Salome Meca 2012.2 (installed in CAElinux 2011 OS).

I tried to modify the command file listed in the text (Salome 5.1.4) to be compatible with this newer version and was not entirely successful. There were quite a few alarms (many repeated) and I can't seem to clear them. I suspect it is has to do with setting up AFFE_CARA_ELEM and the stress fields (SIEF_ELGA) but haven't been able to figure it out. I think these alarms make a difference since the maximum deflection that I get is 1.59 but the text indicates it should be 2.63.

I'd appreciate your help to clear the alarms. I've attached all the files including the GMSH files. Thanks.

Regards,
- Darren

Attachments:
port1_121222_2045_DY.zip, Size: 1.44 MiB, Downloads: 407

jeanpierreaubry · 2012-12-23 16:31:27

hello

i am happy to know you are putting things together

DEPL should be 0 at INST 2, 0.379 at INST3 , 1.95 at INST 4, 23.9 at INST 5,
i do know where the 2.63 value comes from in my text, it is a false value !!

regarding the warning

!------------------------------------------------------------------------------------------------------!
   ! <A> <DISCRETS_27>                                                                                    !
   !                                                                                                      !
   ! Vous utilisez des discrets MECA_DIS_T_N pour affecter des RAIDEURS alors que vous n'avez pas affecté !
   ! les caractéristiques de raideurs. Par défaut la raideur est nulle.                                   !
   ! Il faut vérifier les affectations sous AFFE_CARA_ELEM/DISCRET.                                       !
   ! Informations :                                                                                       !
   !    Maille de nom M3, de 1 noeud(s).                                                                  !
   !    Nom et coordonnées des noeuds :                                                                   !
   !       N6    0.00000E+00    5.00000E+02    1.00000E+03                                                !
   !                                                                                                      !
   !                                                                                                      !
   ! Ceci est une alarme. Si vous ne comprenez pas le sens de cette                                       !
   ! alarme, vous pouvez obtenir des résultats inattendus !                                               !
   !------------------------------------------------------------------------------------------------------!

means there was no stiffness given for the discrete elements that bears a mass Code_Aster will put a null stiffness on them
all the good we do not want any stiffness here!

   !------------------------------------------------------------------------------------------------------!
   ! <A> <CALCULEL_26>                                                                                    !
   !                                                                                                      !
   ! Les commandes CALC_ELEM et CALC_NO ne doivent pas etre utilisées en "reuse" lorsque                  !
   ! l'on utilise l'un des mots clés suivants :                                                           !
   !   * MODELE                                                                                           !
   !   * CHAM_MATER                                                                                       !
   !   * CARA_ELEM                                                                                        !
   !   * EXCIT                                                                                            !
   !   * GROUP_MA / MAILLE                                                 !
   !------------------------------------------------------------------------------------------------------!

this is to tell that the named keyword are unnecessary in this operator

it is better to drop them out

all the very verbose warning set is harmless in this example

jean pierre aubry

DarrenY · 2012-12-24 01:21:28

Hi Jean Pierre,

Thanks for your help that's good to hear that the alarms are not serious.

I get slightly different displacement (DEPL) results as follows:

INSTANT DEPL
2 0
3 0.309
4 1.594
5 19.542

I commented (#) the MODELE, CHAM_MATER, and CARA_ELEM keywords in the CALC_ELEM command. The alarm was eliminated. The results weren't affected by the alarm.

I added an IMPR_RESU command for the DEPL results.

Now I can continue the exercise with more confidence. Thanks again.

Regards,
- Darren

Last edited by DarrenY (2012-12-28 20:30:48)

Attachments:
port1_121223_1723.zip, Size: 1.45 MiB, Downloads: 417

DarrenY · 2012-12-28 16:44:37

Hi,

I've gotten to Chapter 14 (page 32) of the tutorial regarding a hinge at the ends of the top beam. I was hoping to figure this out on my own but need a bit of help. I've attached the files.

The concept is simple: allow a more free rotation where the top beam meets the mast by introducing an element with low resistance (stiffness) to rotation about the x-axis.

The text didn't go into detail since this should be simple and also pointed to a port2.* from WORKED EXAMPLES. I couldn't find these.

Do the WORKED EXAMPLES files exist somewhere?

In GMSH, I did the following:

- Created a point on topbeam 10mm from the ends
- Made the mesh length (changed cl1 to cl2) 10 to be consistent with the actual length
- Made lines with these new points
- Changed the Physical Line for "topbeam" to include these new lines
- Made a new Physical line called "hinge"
- Meshed as 1D

I did all the edits using a text editor, it seemed more convenient, and reloaded in GMSH then exported to MED for use in SALOME-MECA. The mesh looked fine when imported into Salome-Meca. The "hinge" submesh was present. No other errors from either GMSH or Salome were encountered.

I modified the keyword DISCRET as follows:

DISCRET=(_F(CARA='M_T_D_N',
GROUP_MA='massN',
VALE=0.01,),
_F(REPERE='GLOBAL',
CARA='K_TR_D_L',
GROUP_MA='hinge',
VALE=(1e6,1e6,1e6,1e1,1e9,1e9,),),),);

When tried to run, received 1 error:

-----------------------------------
<EXCEPTION> <UTILITAI_2>
il ne faut pas demander 'TR' derrière cara si le type d'élément discret ne prend pas en compte la rotation

Destruction du concept 'elemcar'.
-----------------------------------

This translated as follows (excuse my poor skills in the French language):

-----------------------------------
< EXCEPTION > < UTILITAI_2 >
so do not ask 'TR' behind cara if discreet item type does not take into account the rotation

Destruction of the 'elemcar' concept.
-----------------------------------

Along the way, I have tripped myself. Please help. Thank-you.

Regards,
- Darren

Last edited by DarrenY (2012-12-28 16:48:58)

Attachments:
port1_Chapter_14_Release_Top_Ends_121227_1129_DY.zip, Size: 52.49 KiB, Downloads: 328

jeanpierreaubry · 2012-12-28 17:08:29

hello

some lines are missing in the AFFE_MODELE to tell Code Aster that the hinge group contains
a discrete element
as you did they do exist in the mesh but not in the model

model=AFFE_MODELE(
    MAILLAGE=mesh,
    AFFE=(
		............................
        _F(
          GROUP_MA=('hinge',),PHENOMENE='MECANIQUE',
          MODELISATION='DIS_TR',
        ),
		................
     ),
);

regarding the WORKED EXAMPLES i did not include any purposefully
considering that it is better learning to type by hand the examples at the beginning

jean pierre aubry

Last edited by jeanpierreaubry (2012-12-28 17:16:08)

DarrenY · 2012-12-28 18:32:38

Hi Jean Pierre,

Assigning the discrete model to the "hinge" removed the one error.

Now there is an error at M14.

------------------------
<EXCEPTION> <MODELISA_8>
Vous affectez des caractéristiques de type POUTRE à la maille M14 qui est pas de ce type.

Conseil :
Vérifier le résultat de la commande AFFE_MODELE pour la maille M14.
------------------------

------------------------
Destruction du concept 'elemcar'.
------------------------

If I interpret this correctly, M14 is a mesh element numbered 14. It appears that the the numbering is different between the GMESH and MED files. In the GMSH file element 14 is in the mast but in the MED file element 14 (turning on element numbering in window) is in the top beam but away from the hinge. If I go to MESH INFORMATION in Salome-Meca MESH Module and click on the hinge, this is numbered EDGE #14.This makes the most sense (though I don't understand the numbering systems) since it's the hinge that's been revised in this case.

The error message seems to refer to an assignment of a beam to maille M14 (which is likely the hinge) but it's not of this type. Then the message points back to the assign model command. (It's good that these messages are so descriptive.)

Have I mixed two types of model assignment to one element?

It makes sense not to include the WORKED EXAMPLES. I think I'm learning far more to this point than if I had the files.

Regards,
- Darren

Attachments:
port1_Chapter_14_DIS_TR_Release_Top_Ends_121228_1116_DY.zip, Size: 12.87 KiB, Downloads: 327

jeanpierreaubry · 2012-12-28 18:46:59

there is a mistake in the group making in .geo file
the hinges belong to 'topbeam' group and 'hinge' group

having elements belonging to different groups in Gmsh should be avoided
except if the .comm file is built for that
and this not a beginner,s job

DarrenY · 2012-12-28 20:25:06

Hi Jean Pierre,

It worked! I had consciously made "hinge" as part of "topbeam" thinking that it needed to be that way to share properties. (It looks like there was another error with how I'd ordered the beams as well.) Now I see that doesn't make much sense since the stiffness is given by the discrete element variables for "hinge". I separated the elements in the GEO file and the results look logical with no lateral displacement of the masts and only vertical deflection of "topbeam".

Thank-you very much.

On to Chapter 15....

Regards,
- Darren

Last edited by DarrenY (2012-12-28 20:30:09)

Attachments:
port1_Chapter_14_DIS_TR_Free_End_Rotation_SUCCESS_121228_1311.zip, Size: 115.68 KiB, Downloads: 408

DarrenY · 2013-01-09 17:29:34

Hi,

I've completed Chapter 15 to 17 which involves adding a plate (COQUE) between the masts and below the topbeam. I think everything went well in GMSH (Chapter 15). From the image in Figure 19, it appeared that the vertical edges of the sign are located 10mm horizontally from the masts due to the hinges. I made sure that the two new lower hinge elements are now part of the original upper two hinges (total of 4 hinges). I checked the normals and reversed two of them as described in the tutorial.

I completed the additions to the command file in Chapter 16 and preparations in ASTK in Chapter 17. I had some uncertainties along the way as follows:
____________________________________________________________________

For the INCLUDE command to create a GMSH file I created the comm2 file (I called it "port1_include_GMSH.comm2"). Not being absolutely sure what this code should look like, I used EFICAS to try to ensure that the correct keywords are present. This was after reading the documentation U4.13.01 INCLUDE and U4.81.31 STANLEY.
____________________________________________________________________

The example in Section 4 (bottom of page 3) of document U4.13.01 INCLUDE PROCEDURE does not show semicolons (";") at the end of each command line but the semicolons are present in what appears to be the MESS file on the last page.

In the tutorial, (Chapter 16, page 37) the semicolons are also not present for the INCLUDE and STANLEY commands.

EFICAS includes the semicolons so I included semicolons.

Are the semicolons (";") at the end of command lines optional?
Is this possibly true only for INCLUDE and STANLEY commands?
____________________________________________________________________

On page 38 near the top of the page (Chapter 17) there is reference to first lines in the command file that are used for mesh verification. I'm not sure what these commands look like and how it writes to a mmed file (LU 71). I thought perhaps it is the VERI_MAIL keyword in the U4.21.01 LIRE_MAILLAGE command or perhaps the U7.03.02 MACRO_INFO_MAIL. I included the post1verif.med file in the ASTK file but am not sure if there is an automatic writing to this file or if I require another keyword.
____________________________________________________________________

The first run had an error that appeared to relate to assigning a material (AFFE_MATERIAU) for element M183 which appears to be part of the "panel". So I included the "panel" along with "topbeam" and "mast" in the AFFE_MATERIAU command. That seemed to repair the error for CHAM_MATER though several alarms remain and in the end and there is an error (the attached files have "panel" added to AFFE_MATERIAU which wasn't indicated in the tutorial so I'm not sure if I'm correct in adding this. If this is correct do I have to add "panel" to other commands as well?). Some results are obtained (RESU, RMED files) but they seem to only represent the topbeam and masts, not the panel. STANLEY doesn't open from the run as well which is probably due to the error (EXIT CODE=1).

The files are attached.

I'd appreciate your help. Thank-you.

Regards,
- Darren

Attachments:
port1_CHAPTER_15_to_17_SIGN_ADDED_130109_1020_DY.zip, Size: 332.34 KiB, Downloads: 356

jeanpierreaubry · 2013-01-10 09:07:14

hello

i have modified a bit your .comm file regarding the results

INCLUDE(UNITE=91, INFO=2,); will include a file with this LU
this include file should be written like this
yours was a bit to short to properly print the Gmsh .pos file
of course you need to have the relevant entries in ASTK

IMPR_RESU(
	MODELE=model,
	FORMAT='GMSH',
	UNITE=37, #LU different of 91 already used
	RESU=_F(
		RESULTAT=stat,
		NOM_CHAM=('DEPL','SIPO_ELNO','SIEF_ELNO','REAC_NODA',),
		GROUP_MA=('topbeam','mast',),
	),
);

you

this line
IMPR_RESU(FORMAT='MED', UNITE=71, RESU=_F(MAILLAGE=mesh,),);
does just print a copy of the mesh that will be actually used in the calculation
you can just open it with Salome or Gmsh

regarding semicolons at the end of lines i must admit that i do not exactly in which conditions they can be omitted!
anyhow if the syntax is not correct they will a error explained in the .mess file

jean pierre aubry

Attachments:
port1.comm, Size: 7.63 KiB, Downloads: 408

DarrenY · 2013-01-11 23:58:36

Thank-you, Jean Pierre.

It works. I was able to follow through the STANLEY and GMSH post processing in Chapter 18 and 19.

The following are some things that I'm not very sure about:

- Comparing the results with Figures 27 and 28 seem to be a bit different. The scale bar for statsup_SIEQ_NOEU_VMIS ranges from 0.478 to 176 (Load Step 4) in this case and the tutorial shows a range from 0.786 to 19.4 (Load Step 5).

- Load Step 5 doesn't appear as an option in Stanley for drawing (it does appear as an option in Salome when importing the rmed file into Post Pro).

- There appears to be high stress concentrations in the upper corners in this calculation (where the topbeam and masts meet) but not as significant in Figures 27 and 28. At midspan, the tutorial shows equally high values for the top and bottom but this calculation doesn't show high values at the top only higher values toward the bottom edge of the panel.

- If I import the rmed file into Salome the panel doesn't show up (only topbeam and mast groups are shown). The panel shows up fine in GMSH post processing.

Perhaps the differences are due to how I prepared the mesh. Maybe weight should be given to the plate as well? Now that I have a working example I can alter variables to better understand the meaning.

Files are attached.

On to Chapter 20 and stiffening rods....

Regards,
- Darren

Attachments:
port1_Chapter_17_to_19_SUCCESS_130111_1530_DY.zip, Size: 795.05 KiB, Downloads: 414

jeanpierreaubry · 2013-01-12 16:16:54

hello

the high stresses shown at the top corners should warn you that something is wrong somewhere,
may be some members drawn in the .geo file have not been translated into the mesh as you believe they have been and thus are not used in the structural model,
in fact quite a few of them!
i let you find by yourself at first
looking at port1verif.med may help

jean pierre aubry

Last edited by jeanpierreaubry (2013-01-12 16:20:02)

DarrenY · 2013-01-12 19:34:53

Hi,

I suspect I know where there are missing members with some logic as follows.

- When drawing the panels a new bottom beam and five new vertical members joining the 'topbeam' and bottom are added.

- Then four panels were created within these vertical and horizontal members to create the 'panel' group.

- The hinges created for the previous exercise at the junction between the mast and topbeam are located at the top corners of the panel. Two new hinges were created to support the lower corners and these were added to the 'hinge' group.

- The new members from the first step (bottom beam and verticals) were not added to a mesh group as was done for the 'hinge' group.

- It seems that at present the current example effectively represents one continuous panel (not four individually supported panels) and the panel is supported only from the topbeam (hinged at the top corners) and exclusively at the bottom corners. It's presently one big sheet blowing in the wind and needs to be divided and supported.

- If I add the new bottom and vertical members to 'topbeam' I should reduce the stress concentration at the top corners and redistribute the stress to the lower corners and bottom edge. This should produce more symmetrical stress distribution along the top and bottom edge of the panel.

Now to prove suspicions...

Thanks for not pointing to this directly.
The discovery process is the best teacher.

Regards,
- Darren

DarrenY · 2013-01-13 04:11:44

Hi,

I modified the mesh to include the missing members. Now the panels are framed by 'topbeam' members. In turn I made another correction to the masts by making the mast two members that meet at the lower hinge intersection.

Now the stress pattern for statsup_SIEQ_NOEU_VMIS looks similar to those shown in Figure 27 and 28 along with some stress concentration in the lower corners. The magnitudes still differ. In the tutorial the scale bar range is 0.786 to 19.4 but this calculation ranges from 3.83 to 79.7. I changed the orientation of the topbeam section from laying on the long side to laying on the short side as indicated on page 27 (didn't do this previously) with

ORIENTATION=_F(GROUP_MA=(topbeam,),CARA=ANGL_VRIL, VALE=90.0,),

When laid on the short end the scale bar becomes 3.7 to 78.9, not a significant change.

In the STANLEY window the steps shown are from 1 to 4. There isn't a 5th step as shown in Figure 26. Opening *.rmed in Post Pro there are four steps as well and they're numbered from 2 to 5. Files are attached.

I think this is correct now as far as I can tell.

Regards,
- Darren

Attachments:
port1_Chapter_17_to_19_SUCCESS_4_PANELS_130112_2101_DY.zip, Size: 1.16 MiB, Downloads: 406

jeanpierreaubry · 2013-01-13 12:09:36

well
it is not in full agrrement with the example yet
the vertical members in between the 'topbeam' should be in a separate group with
_F(GROUP_MA=('vertb'),
SECTION='RECTANGLE',CARA=('HY','HZ','EP',),
VALE=(20, 20, 1.5,),
),
i admit is not clearly written in the tutorial

regarding the fifth load case you have to create it with load 'cv' adding itself to the previous one!

#1 2012-05-02 20:17:46

[SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#2 2012-05-03 07:18:26

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#3 2012-05-03 10:15:35

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#4 2012-05-04 20:27:30

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#5 2012-05-05 09:08:03

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#6 2012-05-07 18:40:15

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#7 2012-05-08 08:20:36

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#8 2012-05-08 17:26:02

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#9 2012-12-04 12:39:44

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#10 2012-12-10 18:19:55

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#11 2012-12-23 03:48:27

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#12 2012-12-23 16:31:27

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#13 2012-12-24 01:21:28

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#14 2012-12-28 16:44:37

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#15 2012-12-28 17:08:29

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#16 2012-12-28 18:32:38

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#17 2012-12-28 18:46:59

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#18 2012-12-28 20:25:06

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#19 2013-01-09 17:29:34

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#20 2013-01-10 09:07:14

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#21 2013-01-11 23:58:36

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#22 2013-01-12 16:16:54

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#23 2013-01-12 19:34:53

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#24 2013-01-13 04:11:44

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

#25 2013-01-13 12:09:36

Re: [SOLVED] Exit Code = 139 for Tutorial Beam-cable-gmsh-aster

Board footer