Code_Aster forums
Welcome on the forums. Please post in English or French.
You are not logged in. You won't be able to post until you register and log in using the top-right bar.
#1 2012-06-11 11:46:16
- rlopezcancelos
- Member
- Registered: 2011-07-19
- Posts: 17
Discreet contact Doubt
Hi all.
I'm trying to simulate a simple contact problem, a block on top of another block. I would like to solve a discrete method for comparison with the continuous method.
I have read that can be used DIS_T element to simulate the behavior of springs in the area of contact. Defining characteristics of the elements by DIS_CONTACT in DEFI_MATERIAU but this is used for DIS_CHOC constitutive law.
In my case I want to solve the problem with STAT_NON_LINE and the two pieces are based on initial contact.
Someone can tell if there is any way to solve it in CODE_ASTER.
thanks
Offline
#2 2012-06-11 19:44:03
- Thomas DE SOZA
- Guru
- From: EDF
- Registered: 2007-11-23
- Posts: 2117
Re: Discreet contact Doubt
You should have a look at test case SSNP121 which does exactly that. There are several models some 2d some 3d.
Note that discret element are not advised unless you require point contact or have a need for contact in explicit dynamics or modal analysis.
TdS
Offline
#3 2012-06-20 13:25:19
- rlopezcancelos
- Member
- Registered: 2011-07-19
- Posts: 17
Re: Discreet contact Doubt
Thomas DE SOZA wrote:
You should have a look at test case SSNP121 which does exactly that. There are several models some 2d some 3d.
Note that discrete element are not advised unless you require point contact or have a need for contact in explicit dynamics or modal analysis.
TdS
Thanks for the help. The test cases SSNP121 were very clarifying for me. But in any case an element DIS_T was used.
My boundary conditions is not a displacement mode, it is a surface force. Therefore I need a POI1 element to simulate a spring if I want to solve the problem with discrete contact.
I was looking up the testing cases SSNA122, corresponding to the second case included in the following publication: Advanced Finite Element Contact Benchmarks (NAFEMS). In this case are two examples solved by the continuous method and two with the continuous method. In these last two cases POI1 elements are used.
Code-Aster solves different cases with a axisymetric model. And I have a simple question, in both cases (SSNA122b and SSNA122d) imposes a zero displacement in the x direction in the symmetry axis, why is this done? (Question 1) I thought that the axis of symmetry already had imposed this condition by definition. But in SSNA122D is removed the condition of zero displacement to the edge corresponding to the element of the punch is in contact, why is the reason? (Question 2)
And other simple question, why it is used to impose the condition AFFE_CHAR_CINE and not the usual AFFE_CHAR_MECA? (Question 3)
Now I am trying to solve the SSNA122 problem with a 3D model, with the two formulations: discrete and continuous. I show the different results in the file PUNCH.pdf. In the graph we could see four solutions:
- Blue line belong to discrete case in 3D.
- Red line belong to continuous case in 3D.
- Green line belong to discrete case in 2D (SSNA122c).
- Violet line belong to discrete case in 2D whit the axis condition DX=0 (SSNA122d).
In the 3D cases I have different solution to the 2D cases.
In the discrete case 3D (called P3D_1) I have to use a POI1 stiffness in z direction of 1e+3. But i think that is a big value than the SSNA122 discrete case. But I can not solve the problem whit a lower value (the result does not converge). How could I improve the quality of my results in this case? (Question 4)
In the continuous case 3D (called P3D_3) I have to use the penalization method for both algorithms, and I think that the COEF_PENA_FROT is somewhat low, 1e+6. But I can not solve the problem whit a higher value (the result does not converge). How could I improve the quality of my results in this case? (Question 5)
I had to use different types of finite elements between 2D and 3D cases. Because I was not able to mesh with Q1 finite elements in SALOME 2012.1.
And I use to calculate the 11.1.0 CODE_ASTER version.
I attached in the compressed file: PUNCH.pdf, P3D_1 (P3D_1.comm and the meshes) and P3D_3 (P3D_3.comm and the meshes)
Could somebody help me to solve my doubts?
Thanks in advance.
Offline
#4 2012-06-20 13:40:24
- rlopezcancelos
- Member
- Registered: 2011-07-19
- Posts: 17
Re: Discreet contact Doubt
Sorry i had a problem with the file attachment.
I will try putting it back o within two hours.
Offline
#5 2012-06-20 16:29:14
- rlopezcancelos
- Member
- Registered: 2011-07-19
- Posts: 17
Re: Discreet contact Doubt
rlopezcancelos wrote:
Sorry i had a problem with the file attachment.
I will try putting it back o within two hours.
finally here is the file
Offline
#6 2012-06-25 14:26:14
- Thomas DE SOZA
- Guru
- From: EDF
- Registered: 2007-11-23
- Posts: 2117
Re: Discreet contact Doubt
rlopezcancelos wrote:
But in any case an element DIS_T was used.
My boundary conditions is not a displacement mode, it is a surface force. Therefore I need a POI1 element to simulate a spring if I want to solve the problem with discrete contact.
Sorry but I don't understand your statement. DEFI_CONTACT based algorithms should be able to solve any contact problem and resorting to DIS_CONTACT elements should be exceptional.
rlopezcancelos wrote:
Code-Aster solves different cases with a axisymetric model. And I have a simple question, in both cases (SSNA122b and SSNA122d) imposes a zero displacement in the x direction in the symmetry axis, why is this done? (Question 1) I thought that the axis of symmetry already had imposed this condition by definition.
As already explained many times in the forum, the DX (e.g. radius displacement) boundary condition is implicit in AXIS modelization. It is usually applied nonetheless for 2 reasons :
- teaching purpose and sake of clarity (the structural engineer must remember this condition)
- to alleviate meshing issues : sometimes points located on the axis of symmetry, will have an x-coordinate of 1.0E-12 instead of 0.0 and therefore will be allowed to move alongside DX.
rlopezcancelos wrote:
But in SSNA122D is removed the condition of zero displacement to the edge corresponding to the element of the punch is in contact, why is the reason? (Question 2)
This documented (albeit in french) in the .comm file of the test case : for test case B and D where friction is involved, the DX blocking will be in conflict with the Coulomb stick-slip condition on the one slave point located on the axis of symmetry. In order to workaround this problem (which will cause a singular matrix if we do nothing) :
- the CONTINUE formulation has a special feature to exclude points from friction solving only (SANS_GROUP_NO_FR)
- the DISCRETE formulation has nothing. Therefore we apply the b.c. using a very stiff spring (k=1.0E+14) which will prevent singularity and in the meantime block DX displacement.
rlopezcancelos wrote:
And other simple question, why it is used to impose the condition AFFE_CHAR_CINE and not the usual AFFE_CHAR_MECA? (Question 3)
Because it saves dofs. But you may safely replace it with AFFE_CHAR_MECA
rlopezcancelos wrote:
Now I am trying to solve the SSNA122 problem with a 3D model, with the two formulations: discrete and continuous.
I did not look at the files but in 3D, have you meshed only one quarter of the structure ? This is far better since it will negate most of the rigid body motions. The remaining one being eliminated by using the CONTINUE formulation (CONTACT_INIT='INTERPENETRE'). The singularity is avoided by the same mean as in 2D.
Regarding DISCRETE formulation springs will have to be used in the same manner as in 2D.
TdS
Offline
