Sheet Metal Bending-Contact/BC set up
- Alibay
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 14
- Thank you received: 0
8 years 4 months ago - 8 years 4 months ago #8457
by Alibay
Sheet Metal Bending-Contact/BC set up was created by Alibay
Hi everyone.
I am working on simulation of 3D sheet metal bending simulation of aluminum Code_Aster (CAELinux 11.3). I would appreciate if some one can give advice on the questions that I have. For reference, I attached my mess file and model pics in a zip file.
Model---My model has 4 parts, punch, die, blank holder and sheet.
Material--- sheet is aluminum, others are rigid bodies, so I set them to steel. I am interested in plastic deformation of the sheet, so sheet has nonlinear material properties.
Boundary condtion--- die is fixed at bottom. A pressure load is applied on top surface of blank holder. Punch moves downward to deform aluminum sheet.
Contact---I thought there should be 5 zones which are in contact. They are sheet top---blank holer bottom, sheet top --- punch bottom, punch back----sheet top, die top---sheet bottom, die front---sheet bottom.
I can not set all of these 5 contact in simulation because the same slave surface can not be in multiple contact zone or because there is singular matrix error if I set a slave surface in one zone as master surface in another zone.
solution--- I followed test case ssnp155, so I used DYNA_NON_LINE with deformation behavior 'SIMO_MIEHE'.
result--- now i get result for first few steps. but the result shows that there penetration between sheet and die, which is not expected.
Questions:
1. Is there a way that I can set all five contacts in simulation correctly?
2. The continue method in contact definition uses Lagrangian method by default. So I expected no penetration. But why am I getting the penetration? How can I avoid penetration with continue method?
3. Is there a better way that apply the blank holder force instead of applying pressure on top of blank holder?
4. solution seems to take very long time because of small time step required by DYNA_NON_LINE. Is there any way that the computation time can be reduced to reasonable amount?
Thanks.
I am working on simulation of 3D sheet metal bending simulation of aluminum Code_Aster (CAELinux 11.3). I would appreciate if some one can give advice on the questions that I have. For reference, I attached my mess file and model pics in a zip file.
Model---My model has 4 parts, punch, die, blank holder and sheet.
Material--- sheet is aluminum, others are rigid bodies, so I set them to steel. I am interested in plastic deformation of the sheet, so sheet has nonlinear material properties.
Boundary condtion--- die is fixed at bottom. A pressure load is applied on top surface of blank holder. Punch moves downward to deform aluminum sheet.
Contact---I thought there should be 5 zones which are in contact. They are sheet top---blank holer bottom, sheet top --- punch bottom, punch back----sheet top, die top---sheet bottom, die front---sheet bottom.
I can not set all of these 5 contact in simulation because the same slave surface can not be in multiple contact zone or because there is singular matrix error if I set a slave surface in one zone as master surface in another zone.
solution--- I followed test case ssnp155, so I used DYNA_NON_LINE with deformation behavior 'SIMO_MIEHE'.
result--- now i get result for first few steps. but the result shows that there penetration between sheet and die, which is not expected.
Questions:
1. Is there a way that I can set all five contacts in simulation correctly?
2. The continue method in contact definition uses Lagrangian method by default. So I expected no penetration. But why am I getting the penetration? How can I avoid penetration with continue method?
3. Is there a better way that apply the blank holder force instead of applying pressure on top of blank holder?
4. solution seems to take very long time because of small time step required by DYNA_NON_LINE. Is there any way that the computation time can be reduced to reasonable amount?
Thanks.
Last edit: 8 years 4 months ago by Alibay. Reason: why is there no attachment
Please Log in or Create an account to join the conversation.
- RichardS
- Offline
- Elite Member
-
8 years 4 months ago - 8 years 4 months ago #8458
by RichardS
SimScale - Engineering Simulation in your browser!
Replied by RichardS on topic Re: Sheet Metal Bending-Contact/BC set up
Hi Alibay,
- use parallelization techniques: MPI or OpenMP
- reduce the slave surfaces of your contacts to a minimum
- try DISCRETE contact method with GCP (if you don't require friction)
- use an iterative solver if possible (convergence might be hard)
- use AFFE_CHAR_CINE instead of AFFE_CHAR_MECA whenever possible to reduce the total number of DOFs
- Do you use fixed point method for the contact resolution? Try using NEWTON for all nonlinearities.
- ...........
Good luck.
Richard
Sure, there is no limitation in how many times a surface can be as MASTER in a contact.Alibay wrote: 1. Is there a way that I can set all five contacts in simulation correctly?
The best way would be to refine your mesh.Alibay wrote: 2. The continue method in contact definition uses Lagrangian method by default. So I expected no penetration. But why am I getting the penetration? How can I avoid penetration with continue method?
I don't understand this. What means better here? You can use a surface tension, which can apply distributed forces in arbitrary directions if you need non-normal forces.Alibay wrote: 3. Is there a better way that apply the blank holder force instead of applying pressure on top of blank holder?
There are a lot. The problem is too unspecified to give meaningful suggestions. Pick one of those:Alibay wrote: 4. solution seems to take very long time because of small time step required by DYNA_NON_LINE. Is there any way that the computation time can be reduced to reasonable amount?
- use parallelization techniques: MPI or OpenMP
- reduce the slave surfaces of your contacts to a minimum
- try DISCRETE contact method with GCP (if you don't require friction)
- use an iterative solver if possible (convergence might be hard)
- use AFFE_CHAR_CINE instead of AFFE_CHAR_MECA whenever possible to reduce the total number of DOFs
- Do you use fixed point method for the contact resolution? Try using NEWTON for all nonlinearities.
- ...........
Good luck.
Richard
SimScale - Engineering Simulation in your browser!
Last edit: 8 years 4 months ago by RichardS.
Please Log in or Create an account to join the conversation.
- Alibay
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 14
- Thank you received: 0
8 years 4 months ago #8459
by Alibay
Replied by Alibay on topic Re: Sheet Metal Bending-Contact/BC set up
Thank you for your detailed answers.
I will try them and come back.
ps: I wnated to attach model, the mess . but I am not able to do that. is it problem of my account or the forum?
I will try them and come back.
ps: I wnated to attach model, the mess . but I am not able to do that. is it problem of my account or the forum?
Please Log in or Create an account to join the conversation.
- Alibay
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 14
- Thank you received: 0
8 years 4 months ago #8460
by Alibay
Replied by Alibay on topic Re: Sheet Metal Bending-Contact/BC set up
Another question: is there any anisotropic yield criteria for sheet metal bending? I mean has yield criteria like Hill 1948,Hill1990, Barlot, BBC etc. implemented in code-aster?
thanks.
thanks.
Please Log in or Create an account to join the conversation.
- Alibay
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 14
- Thank you received: 0
8 years 4 months ago - 8 years 4 months ago #8462
by Alibay
Replied by Alibay on topic Re: Sheet Metal Bending-Contact/BC set up
Hi RechardS,
I tried what your suggested. I made my mesh finer, especially on the contact surface in order to avoid penetration.
But again problem still exists when I try to define contact zones that have the same surface as MASTER or Slave. As you advised, I set the same surface as MASTER in two (or more) contact zone and got the same error saying nodes are shared in different contact zone or simulation stopped due to singular matrix. I tried with discrete method, seems this method is not that strict to master-slave surface definition, but there is friction involed in this simulation, so I can not go with it.
Unfortunately, I am not able to attach my files. The following is my model. The punch goes down and deform the sheet into a L form. Here is the link to how my model looks like.
L-Bending
The main problem is how to define contact zone. there are five contact zone:
(1) Sheet Top---Blank Holder Bottom
(2) Sheet Top---Punch Bottom
(3) Sheet Top---Punch Right side surface (these two surface come in contact after punch goes down certain distance.)
(4) Sheet Bottom---Die Top
(5) Sheet Bottom---Die Left side surface (these two surface come in contact after sheet is bent 90 degrees).
How am I supposed to select master-slave surface for each contact zone?
Here is my current set up.
In order to reduce computation time I activated NEWTON_KYRLOV and iterative solver PETSC. But it just fails or hangs after a few iteration saying that maximum number of iteration reached. Below is my solution set up. Where I went wrong?
I tried what your suggested. I made my mesh finer, especially on the contact surface in order to avoid penetration.
But again problem still exists when I try to define contact zones that have the same surface as MASTER or Slave. As you advised, I set the same surface as MASTER in two (or more) contact zone and got the same error saying nodes are shared in different contact zone or simulation stopped due to singular matrix. I tried with discrete method, seems this method is not that strict to master-slave surface definition, but there is friction involed in this simulation, so I can not go with it.
Unfortunately, I am not able to attach my files. The following is my model. The punch goes down and deform the sheet into a L form. Here is the link to how my model looks like.
L-Bending
The main problem is how to define contact zone. there are five contact zone:
(1) Sheet Top---Blank Holder Bottom
(2) Sheet Top---Punch Bottom
(3) Sheet Top---Punch Right side surface (these two surface come in contact after punch goes down certain distance.)
(4) Sheet Bottom---Die Top
(5) Sheet Bottom---Die Left side surface (these two surface come in contact after sheet is bent 90 degrees).
How am I supposed to select master-slave surface for each contact zone?
Here is my current set up.
COND= DEFI_CONTACT(MODELE= MO,
FORMULATION='CONTINUE',
FROTTEMENT='COULOMB',
#ALGO_RESO_GEOM = 'NEWTON',
#ALGO_RESO_CONT='NEWTON',
#ALGO_RESO_FROT='NEWTON',
LISSAGE='OUI',
ZONE =(
_F(GROUP_MA_MAIT = 'Sh_Top_R',
GROUP_MA_ESCL = 'BH_Bott',
# SANS_GROUP_NO='Sh_Top_L',
COULOMB=0.05,
# CONTACT_INIT='INTERPENETRE',
# INTEGRATION='AUTO',
),
_F(GROUP_MA_MAIT='Die_Comp',
GROUP_MA_ESCL='Sh_Bot_R',
# SANS_GROUP_NO='DieFront',
COULOMB=0.05,
# CONTACT_INIT='INTERPENETRE',
# INTEGRATION='AUTO',
),
_F(GROUP_MA_MAIT='P_Comp',
GROUP_MA_ESCL='Sh_Top_L',
SANS_GROUP_NO='Sh_Top_R',
COULOMB=0.05,
# CONTACT_INIT='INTERPENETRE',
# INTEGRATION='AUTO',
),
#_F(GROUP_MA_MAIT='Sh_Top',
# GROUP_MA_ESCL='P_Surf',
# COULOMB=0.05,
# ),
#_F(GROUP_MA_MAIT='Sh_Bott',
# GROUP_MA_ESCL='Die_Surf',
# COULOMB=0.05,
# ),
_F(GROUP_MA_MAIT='Sh_Top_L',
GROUP_MA_ESCL='P_Back',
SANS_GROUP_NO='P_Comp',
COULOMB=0.05,
),
_F(GROUP_MA_MAIT='Sh_Bot_L',
GROUP_MA_ESCL='DieFront',
SANS_GROUP_NO='Die_Comp',
COULOMB=0.05,
),
),
);In order to reduce computation time I activated NEWTON_KYRLOV and iterative solver PETSC. But it just fails or hangs after a few iteration saying that maximum number of iteration reached. Below is my solution set up. Where I went wrong?
RESU=DYNA_NON_LINE(MODELE=MO,
CHAM_MATER=MAT,
EXCIT=(_F(CHARGE=CL,),
_F(CHARGE=CH,
FONC_MULT=FONC,),),
CONTACT=COND,
COMP_INCR=(_F(RELATION='VMIS_ISOT_TRAC',
#DEFORMATION='PETIT_REAC',
DEFORMATION='SIMO_MIEHE',
GROUP_MA='Sheet',),
_F(RELATION='ELAS',
DEFORMATION='GROT_GDEP',
GROUP_MA='Punch',),
_F(RELATION='ELAS',
DEFORMATION='PETIT',
GROUP_MA=('BH','Die',),),
),
INCREMENT=_F(LIST_INST=LINST,),
SCHEMA_TEMPS=_F(SCHEMA='HHT',
FORMULATION='DEPLACEMENT',),
NEWTON=_F(PREDICTION='TANGENTE',
MATRICE='TANGENTE',
REAC_ITER=1,),
METHODE='NEWTON_KYRLOV',
SOLVEUR=_F(
#SYME='OUI',
MATHODE=' PETSC',
RENU='SANS',
PRE_COND='LDLT_SP',
REAC_PRECOND=30;
),
ARCHIVAGE=_F(LIST_INST=L_INST,),
CONVERGENCE=_F(ITER_GLOB_MAXI=20,
),
);
Last edit: 8 years 4 months ago by Alibay.
Please Log in or Create an account to join the conversation.
- Claus
-
- Offline
- Moderator
-
Less
More
- Posts: 670
- Thank you received: 34
8 years 4 months ago #8470
by Claus
Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version
Replied by Claus on topic Re: Sheet Metal Bending-Contact/BC set up
I tried this a while back:
web-code-aster.org/forum2/viewtopic.php?id=14558
Also, try searching for 'deep draw' and 'springback'
/C
web-code-aster.org/forum2/viewtopic.php?id=14558
Also, try searching for 'deep draw' and 'springback'
/C
Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version
Please Log in or Create an account to join the conversation.
Moderators: catux
Time to create page: 0.156 seconds