stress output values
- Ron Lilley
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 3
- Thank you received: 0
17 years 3 months ago #1692
by Ron Lilley
stress output values was created by Ron Lilley
Hello,
I have a question on the stress output from Code_Aster. I am running a non-linear (plastic deformation) axi-symmetric problem. This consists of a solid bar (mandrel) passing through a tube causing and plastic stretching of the tube wall. The problem runs fine, the problem I’m have is interpreting the results. I am trying to get numbers for the axial, radial, and hoop stress at the node points. As I only need a characteristic sample I selected a row of nodes along a radius to place in a group. I then put out the components for each stress (SIXX, SIYY, SIZZ) in the .RESU file. This also works fine. The problems is there are 2 to 4 values for each stress component at a given node. There are 2 values for nodes on the ID and OD and 4 values for each component for internal nodes. For the 10 nodes in the group I end up with 36 sets of stress values. The output looks like this
CHAMP PAR ELEMENT AUX NOEUDS DE NOM SYMBOLIQUE SIEF_ELNO_ELGA
NUMERO D'ORDRE: 157 INST: 1.00000E+00
MAY X Y SIXX SIYY SIZZ
N47 1.84000E+00 3.33333E+00 -4.30982E+03 1.72332E+04 4.63076E+04
N7N 1.66000E+00 3.33333E+00 -1.31805E+03 1.90692E+04 5.47880E+04
MAZ X Y SIXX SIYY SIZZ
N7N 1.66000E+00 3.33333E+00 -1.15475E+04 1.48758E+04 5.05572E+04
N7O 1.48000E+00 3.33333E+00 -7.09154E+03 1.82319E+04 6.25665E+04
MB0 X Y SIXX SIYY SIZZ
N7O 1.48000E+00 3.33333E+00 -2.18918E+04 1.21595E+04 5.64273E+04
N4B 1.30000E+00 3.33333E+00 -1.52354E+04 1.76121E+04 7.39280E+04
MB1 X Y SIXX SIYY SIZZ
N47 1.84000E+00 3.33333E+00 -3.79219E+03 1.85005E+04 4.68252E+04
N7N 1.66000E+00 3.33333E+00 -9.67433E+02 1.99276E+04 5.51386E+04
MB2 X Y SIXX SIYY SIZZ
N7N 1.66000E+00 3.33333E+00 -1.11969E+04 1.57342E+04 5.09078E+04
N7O 1.48000E+00 3.33333E+00 -6.69495E+03 1.92029E+04 6.29631E+04
And so on for the 36 sets. In other FEA programs I am used to seeing one value for each stress component at a node. Does anyone know how to resolve the 2 to 4 values to a single value? Where this output is explained in the documentation? What value does Salome use when you plot out the stress component in the postprocessor?
Is there a way to have Code_ Aster calculate a single value? To obtain these values the following commands are in my .comm file.
CALC_ELEM: SolNonL
RESULTAT: SolNonL
b_noli
b_toutes
OPTION: (SIEF_ELNO_ELGA, EQUI_ELNO_SIGM)
IMPR_RESU:
FORMAT: RESULTAT
RESU:
b_extrac
NOM_CHAM: SIEF_ELNO_ELGA
b_cmp
NOM_CMP: (SIXX,SIYY,SIZZ)
b_topologie
GROUP_NO: output (output is the group of nodes)
b_valeurs
IMPR_COOR: OUI
I would greatly appreciate any help in this matter.
Thank You,
Ron
I have a question on the stress output from Code_Aster. I am running a non-linear (plastic deformation) axi-symmetric problem. This consists of a solid bar (mandrel) passing through a tube causing and plastic stretching of the tube wall. The problem runs fine, the problem I’m have is interpreting the results. I am trying to get numbers for the axial, radial, and hoop stress at the node points. As I only need a characteristic sample I selected a row of nodes along a radius to place in a group. I then put out the components for each stress (SIXX, SIYY, SIZZ) in the .RESU file. This also works fine. The problems is there are 2 to 4 values for each stress component at a given node. There are 2 values for nodes on the ID and OD and 4 values for each component for internal nodes. For the 10 nodes in the group I end up with 36 sets of stress values. The output looks like this
CHAMP PAR ELEMENT AUX NOEUDS DE NOM SYMBOLIQUE SIEF_ELNO_ELGA
NUMERO D'ORDRE: 157 INST: 1.00000E+00
MAY X Y SIXX SIYY SIZZ
N47 1.84000E+00 3.33333E+00 -4.30982E+03 1.72332E+04 4.63076E+04
N7N 1.66000E+00 3.33333E+00 -1.31805E+03 1.90692E+04 5.47880E+04
MAZ X Y SIXX SIYY SIZZ
N7N 1.66000E+00 3.33333E+00 -1.15475E+04 1.48758E+04 5.05572E+04
N7O 1.48000E+00 3.33333E+00 -7.09154E+03 1.82319E+04 6.25665E+04
MB0 X Y SIXX SIYY SIZZ
N7O 1.48000E+00 3.33333E+00 -2.18918E+04 1.21595E+04 5.64273E+04
N4B 1.30000E+00 3.33333E+00 -1.52354E+04 1.76121E+04 7.39280E+04
MB1 X Y SIXX SIYY SIZZ
N47 1.84000E+00 3.33333E+00 -3.79219E+03 1.85005E+04 4.68252E+04
N7N 1.66000E+00 3.33333E+00 -9.67433E+02 1.99276E+04 5.51386E+04
MB2 X Y SIXX SIYY SIZZ
N7N 1.66000E+00 3.33333E+00 -1.11969E+04 1.57342E+04 5.09078E+04
N7O 1.48000E+00 3.33333E+00 -6.69495E+03 1.92029E+04 6.29631E+04
And so on for the 36 sets. In other FEA programs I am used to seeing one value for each stress component at a node. Does anyone know how to resolve the 2 to 4 values to a single value? Where this output is explained in the documentation? What value does Salome use when you plot out the stress component in the postprocessor?
Is there a way to have Code_ Aster calculate a single value? To obtain these values the following commands are in my .comm file.
CALC_ELEM: SolNonL
RESULTAT: SolNonL
b_noli
b_toutes
OPTION: (SIEF_ELNO_ELGA, EQUI_ELNO_SIGM)
IMPR_RESU:
FORMAT: RESULTAT
RESU:
b_extrac
NOM_CHAM: SIEF_ELNO_ELGA
b_cmp
NOM_CMP: (SIXX,SIYY,SIZZ)
b_topologie
GROUP_NO: output (output is the group of nodes)
b_valeurs
IMPR_COOR: OUI
I would greatly appreciate any help in this matter.
Thank You,
Ron
- Joël Cugnoni
-
- Offline
- Moderator
-
17 years 3 months ago #1695
by Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Replied by Joël Cugnoni on topic Re:stress output values
Dear Ron,
Code-Aster distinguish between several "localization" of filed outputs (stress tensor, strains...): As any other non-linear solver, Code-Aster calculates the stress tensor at the integration points (Gauss points) of each element. In Aster, these fields are named Something_ELGA (GAuss points of the ELements). Some other fields like displacement (DEPL) are directly calculated at the nodes (because these are the primary variables of the FE problem).
Then by using CALC_ELEM, you can compute other fields in the ELMENTS: for example, when writing SIGM_ELNO_ELGA, you ask for the effective stress (SIEF) at the nodes of each elements (ELNO) calculated from the field at the integration points of the element (ELGA).
So you will get on one node as many different values as the number of elements that share this node.
In Salome, you will see only a constant value in each element (centroid) for this kind of fields. But in the future, you should be able to see the discontinuous stress field at nodes as calculated by Aster.
Then if you want an "averaged" stress at nodes, you can ask for it via the command CALC_NO whicha calculates unique nodal values:
for example, if you request SIEF_NOEU_ELGA or EQUI_NOEU_ELGA, you will get the values that you are looking for.
Note that you always need to calculate the field at elements (CALC_ELEM) before requesting it at nodes (CALC_NO).
You can have a look at the .comm file generated in the piston tutorial to see an example.
By the way, this problem would be an excellent example to show how to use the non-linear capabilities of Aster. It would be great if you could publish it on the Wiki to help other users in this field.
Congratulation for the work done, it is not simple at all.
Joël Cugnoni
www.caelinux.com
Code-Aster distinguish between several "localization" of filed outputs (stress tensor, strains...): As any other non-linear solver, Code-Aster calculates the stress tensor at the integration points (Gauss points) of each element. In Aster, these fields are named Something_ELGA (GAuss points of the ELements). Some other fields like displacement (DEPL) are directly calculated at the nodes (because these are the primary variables of the FE problem).
Then by using CALC_ELEM, you can compute other fields in the ELMENTS: for example, when writing SIGM_ELNO_ELGA, you ask for the effective stress (SIEF) at the nodes of each elements (ELNO) calculated from the field at the integration points of the element (ELGA).
So you will get on one node as many different values as the number of elements that share this node.
In Salome, you will see only a constant value in each element (centroid) for this kind of fields. But in the future, you should be able to see the discontinuous stress field at nodes as calculated by Aster.
Then if you want an "averaged" stress at nodes, you can ask for it via the command CALC_NO whicha calculates unique nodal values:
for example, if you request SIEF_NOEU_ELGA or EQUI_NOEU_ELGA, you will get the values that you are looking for.
Note that you always need to calculate the field at elements (CALC_ELEM) before requesting it at nodes (CALC_NO).
You can have a look at the .comm file generated in the piston tutorial to see an example.
By the way, this problem would be an excellent example to show how to use the non-linear capabilities of Aster. It would be great if you could publish it on the Wiki to help other users in this field.
Congratulation for the work done, it is not simple at all.
Joël Cugnoni
www.caelinux.com
Joël Cugnoni - a.k.a admin
www.caelinux.com
- Ron Lilley
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 3
- Thank you received: 0
17 years 3 months ago #1697
by Ron Lilley
Replied by Ron Lilley on topic Re:stress output values
Joel,
Thank You so much for your prompt and very informative reply. I had thought the values were probably the tensors but wanted to be sure. I had also tried outputting the SIEF_NOEU_ELGA but had missed the CALC_NO step. All is working now.
By the way general explanations like you provided are extremely helpful. They provide direction in a way that tutorials do not. It would be really nice if there was a general overview document that provided general overview(s). Maybe this could be added to the users community "To DO" list.
I will try to put an example on WIKI when I get a chance. However I can not just put the current problem I am doing onto WIKI as it contains proprietary geometry.
Thank You again.
Ron
Thank You so much for your prompt and very informative reply. I had thought the values were probably the tensors but wanted to be sure. I had also tried outputting the SIEF_NOEU_ELGA but had missed the CALC_NO step. All is working now.
By the way general explanations like you provided are extremely helpful. They provide direction in a way that tutorials do not. It would be really nice if there was a general overview document that provided general overview(s). Maybe this could be added to the users community "To DO" list.
I will try to put an example on WIKI when I get a chance. However I can not just put the current problem I am doing onto WIKI as it contains proprietary geometry.
Thank You again.
Ron
Moderators: catux
Time to create page: 0.152 seconds