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

You are not logged in.

#1 2020-08-14 14:23:54

SamuelTwain
Member
Registered: 2020-08-14
Posts: 18

Geostatic operation in Code Aster?

Dear all:
    I'm a novice to Code Aster. Having watched some videos about Code Aster in Youtude and read some introductory books about Code Aster, I can do some simple simulations right now smile. But when I turn to some complex geomechanical problems, I find I don't know how to realize geostatic step (namely, balance the stress produced by gravity without any/small deformation). Actually, I have searched the documentation, and found that in the command file of V6.03.104 (SSNP104 for test ), it mentioned geostatic step. However, it adpoted the analytical form of stress and created a field (CREA_CHAM).
    But refers to my condition, I don't know the analytical form of geostatic stress, so it seems impossible to create the geostatic stress field analytically. Maybe I can do a prior simulation to calculate the stress produced by gravity solely. Then project the stress result/field  to the desired simulation. The inspiration comes from the projection of temperature in themo-mechanical simulation. But I'm not sure whether it's feasible, because I can't find the keywords to assign the projected stress field in material. So I'm confused.
    First, in prior simulation, what kind of stress should be output? SIGM_ELNO, SIGM_ELGA or SIGM_NOEU?
    Second, when I assign the projected filed through order AFFE_VARC, it seems that stress is not included in the keywords.
    Would you kindly please tell me how to do geostatic setup? Or give some hints of relevant training materials?
Best regards
Samuel

Offline

#2 2020-08-16 09:52:19

mf
Member
Registered: 2019-06-18
Posts: 118

Re: Geostatic operation in Code Aster?

Hi,

I try to answer as best as I can. Please bear in mind, many CA-users wouldn't know what you want to do from your brief description, I assume the number of users that do geomechanics is not very large compared to mechanical engineers.

From what you describe, I would do the following:
-) in a first calculation step (is it nonlinear? I wouldn't know from your description) I would calculate the stress field you mention.
-) in a second calculation I would take the result from the first as ETAT_INIT in the second (probably nonlinear) calculation. At this step there is no worrying necessary about which stresses etc. to output. You take the whole result as ETAT_INIT (same mesh!).

Please let us know more if you need help, if possible post .med and .comm.

Mario.

Offline

#3 2020-08-16 17:21:19

SamuelTwain
Member
Registered: 2020-08-14
Posts: 18

Re: Geostatic operation in Code Aster?

mf wrote:

Hi,

I try to answer as best as I can. Please bear in mind, many CA-users wouldn't know what you want to do from your brief description, I assume the number of users that do geomechanics is not very large compared to mechanical engineers.

From what you describe, I would do the following:
-) in a first calculation step (is it nonlinear? I wouldn't know from your description) I would calculate the stress field you mention.
-) in a second calculation I would take the result from the first as ETAT_INIT in the second (probably nonlinear) calculation. At this step there is no worrying necessary about which stresses etc. to output. You take the whole result as ETAT_INIT (same mesh!).

Please let us know more if you need help, if possible post .med and .comm.

Mario.

Thank you, Mario! That's spot on what I'm looking for. First, I will do a preliminary calculation to get a stress result, and then introduce this stress result to another model by "ETAT_INIT".  And I succeed under your instruction. smile
I also find that  "ETAT_INIT" can only be adopted in the same mesh. Then I happend to get the idea to assign intial stress field between different mesh (namely, diffent grid size). So "ETAT_INIT" cannot be used directly. To bridge the gap, I firstly project the stress field from original mesh to the newer mesh. And then use the projected field of the newer mesh as an intial field by "ETAT_INIT". This method really works. smile
Next, I'm going to investigate different influence of different project method (ECLA_PG and so on). From some training materials, I have known that these methods will transfer/project data between nodes or gauss points. But I'm nor sure for my condition, if I want to project stress field between different mesh and then use this stress field as a initial field , which method would be preferable. Maybe, ECLA_PG is better? From what I gather, field of gauss point are more precious.
Could you please give me some suggestions?
Thanks again
samuel

Offline

#4 2020-08-17 00:02:09

sb1966
Member
Registered: 2015-03-16
Posts: 180

Re: Geostatic operation in Code Aster?

Dear Samuel,

After a search in the forum, I found the following two topics which should be of relevance to a geotechnical engineer:

HTT PS/www.code-aster.org/forum2/viewtopic.php?id=8682

and

 ..... viewtopic.php?id=20240 

However, I am not sure how to equate the DEPL field to zero, while retaining the stress field from the geostatic stage of analysis, and project the same in the next calculation with excavation/filling etc.

I would like to hear from you or other users working in geotechnical field.

Best regards

Sukumar

Offline

#5 2020-08-17 04:08:43

SamuelTwain
Member
Registered: 2020-08-14
Posts: 18

Re: Geostatic operation in Code Aster?

sb1966 wrote:

Dear Samuel,

After a search in the forum, I found the following two topics which should be of relevance to a geotechnical engineer:

HTT PS/www.code-aster.org/forum2/viewtopic.php?id=8682

and

 ..... viewtopic.php?id=20240 

However, I am not sure how to equate the DEPL field to zero, while retaining the stress field from the geostatic stage of analysis, and project the same in the next calculation with excavation/filling etc.

I would like to hear from you or other users working in geotechnical field.

Best regards

Sukumar

Hi Sukumar:
   Nice to meet you! The two posts you listed are very helpful. And I find that my approach is substaintially as same as  their. We both make a preliminary calculation to get a initial field (stress, strain, displacement and so on). Then apply this initial field to a new model through the order "ETAT_INIT". smile The difference is I only apply stress field.
    As for what you mentioned
   

sb1966 wrote:

However, I am not sure how to equate the DEPL field to zero, while retaining the stress field from the geostatic stage of analysis

     This is spot on what I am concerning and what I'm currently doing ( all my above threads focus only on it, so I have no excavation/filling step).
     My approach is :
     1. For a  soil model, apply the normal material and boundary conditions. Meantime, gravity is loaded. And do a calculation under these steups. So as you see, in this step, displacement is allowed and wouldn't be zero. Thus, I have to figure out how to deminish this displacement in the next step.
     2. For the second step, I will use the same initial mesh, material, boundary conditions and gravity. If I do calculation, the result would not be different from what I get from the first step (so displacement will not be zero). But if I introduce the stress field (only stress field) of first step as the initial stress field of second step, the model wouldn't deform under gravity. So that's tricky and interesting.
    Actually, a geostatic step comprises above two steps. smile

P.S.:  Another problem which has nothing to do with the above question, do you know how to project all field between two different meshes (different grid size) in an easy way?
        When I use PROJ_CHAM to project temperature, strain, stress, displacement and so on, I have to give the type and name of each field one by one. That's a bit tedious and arduous... So I'm wondering whether I can project all field in just one keyword. For example: PROJ_CHAM (_F(TOUT=‘OUI’,),).
        Any suggestion?
Best regards
Samuel

Offline

#6 2020-08-18 15:43:27

sb1966
Member
Registered: 2015-03-16
Posts: 180

Re: Geostatic operation in Code Aster?

Dear Samuel,

Actually, a geostatic step comprises above two steps. smile

1. Thank you very much for the steps you have discussed above. I think it correctly models the physics of the process involved, provided not reloaded with gravity in the 2nd step you described above.

1(A). It would be great if you could share your comm file here, showing these steps.

2. Regarding the point you mentioned:

So I'm wondering whether I can project all field in just one keyword. For example: PROJ_CHAM (_F(TOUT=‘OUI’,),).

I think, it is possible to select all the fields for projection, nodewise. Element wise projection needs explicit name of the projected field, if I have understood correctly.  The doc u4.72.05 in section 3.12 says

Keywords TOUT_CHAMP = ‘OUI’ or NOM_CHAM = l_noch allow to choose which are the fields of SD RESULT that one wants to project (by default all fields with the nodes). One can also project the fields by elements “ELNO“and”ELEM“, for that it is explicitly necessary to give their names via the keyword NOM_CHAM.

Hope this replies your question.

Best regards.

Sukumar

Offline

#7 2020-08-18 16:20:44

SamuelTwain
Member
Registered: 2020-08-14
Posts: 18

Re: Geostatic operation in Code Aster?

sb1966 wrote:

1. Thank you very much for the steps you have discussed above. I think it correctly models the physics of the process involved, provided not reloaded with gravity in the 2nd step you described above.

Hi, Sukumar. From what I gather, reload the gravity is necessary. Because, geostatic step is to find the stress field under gravity without deformation. If in the second step, we  don't  apply gravity, the stress on every element would not  balance, then they will deform.

sb1966 wrote:

1(A). It would be great if you could share your comm file here, showing these steps.

Actually, I haven't saved these files, so I am not able to post it right now. Currently, I'm  diving in the assignments from my tutors.....But I will recreate my command file about two day later ( I hope so ). In this command file,results reloading and not reloading gravity will be compared.

Finally, thanks for your share of Keywords TOUT_CHAMP = ‘OUI’. It's useful for me.

Samuel

Offline

#8 2020-08-20 16:05:47

SamuelTwain
Member
Registered: 2020-08-14
Posts: 18

Re: Geostatic operation in Code Aster?

Hi,
    As I have promised, the attachment includes my geostatic step command file and mesh file.
    GEOSTATIC1 is the first step to apply gravity and stress field will be extracted at the end of GEOSTATIC1. The final displacement of GEOSTATIC1 is ~0.58.
    GEOSTATIC2 is the second step. Stress field from GEOSTATIC1 is introduced into GEOSTATIC2 as the initial field. Moreover, gravity is also applied. After calculation of GEOSTATIC2, the displacement decreased from  0.58 to 5.5e-16.
    One thing confuses me. In GEOSTATIC2, I have to replace ELAS_VIMS_LINE with Elastic for comportmente. Otherwise, the calculation will break down and tell me the ELAS_VIMS_LINE comportmente is incompatible. Could anyone please give me some suggestions?

Samuel

Last edited by SamuelTwain (2020-08-20 16:12:14)


Attachments:
GEOSTATIC.rar, Size: 76.79 KiB, Downloads: 30

Offline

#9 2020-08-20 17:16:12

sb1966
Member
Registered: 2015-03-16
Posts: 180

Re: Geostatic operation in Code Aster?

Dear Samuel,

Thanks a lot for your files. I will study them and will come back here, if and when necessary.

Best regards

Sukumar

Offline