Contact interaction on surface not working

General Questions
1

Hello Community,

I am new in PrePoMax but I have some experience with Inventor Nastran. I have big issue with static analysis of assembly with contact. I have been working on this for whole week and now I just don’t have more power to face this.

In general the contact interaction (hard) between surface is not acting in my model.

I have also add frequency step to analyse to check how the model is behave and it shows that components are not interacting with each other.

Please see attached model file and help me solve this issue.

2

In frequency (linear) analyses, contact doesn’t work like in nonlinear analyses - it can’t change its state. You should use tie constraints for frequency studies and then you can replace them with contact for static simulations. Gradually build up the complexity: tie constraint → tied contact → hard contact.

3

Is hard contact in frequency (linear) analysis act like tie constraint / tied contact or just not act att all?

4

Its status should be frozen in those analyses. It may prevent penetration but not separation and sliding.

Slave surface adjustment is quite important in contact. You can set its tolerance to make sure that the slave surface nodes are moved to lie exactly on the master surface, ensuring proper contact initialization.

1 Like
5

With some minor corrections to the input parameters and approximately 15 min. of the calculation time.

Capture
Capture1982×1321 425 KB

6

It is looks like what I am looking for. Can you share the input parameters for the analysis? I am still fighting with this…

7

I have made some adjustment but still can’t catch the convergence. The solution now looks like this. Seems like the contact still not behaving wright.

Please see image below and initial input for this.

image
image1920×973 117 KB

** Physical constants ++++++++++++++++++++++++++++++++++++++
**
**
** Materials +++++++++++++++++++++++++++++++++++++++++++++++
**
*Material, Name=Alu
*Elastic
70000, 0.33
*Density
2.7E-09
*Material, Name=Steel
*Elastic
210000, 0.3
*Density
7.8E-09
**
** Sections ++++++++++++++++++++++++++++++++++++++++++++++++
**
*Solid section, Elset=Internal_Selection-1_Solid_Section-1, Material=Alu
*Solid section, Elset=Internal_Selection-1_Solid_Section-2, Material=Steel
**
** Pre-tension sections ++++++++++++++++++++++++++++++++++++
**
**
** Constraints +++++++++++++++++++++++++++++++++++++++++++++
**
*Rigid body, Nset=Internal-1_Load, Ref node=164587, Rot node=164588
*Tie, Name=Tie-1, Position tolerance=1
Bolt1, Ground2
**
** Surface interactions ++++++++++++++++++++++++++++++++++++
**
*Surface interaction, Name=Surface_Interaction-1
*Surface behavior, Pressure-overclosure=Hard
*Surface interaction, Name=Surface_Interaction-2
*Surface behavior, Pressure-overclosure=Tied
10000000
*Friction
1
**
** Contact pairs +++++++++++++++++++++++++++++++++++++++++++
**
*Contact pair, Interaction=Surface_Interaction-1, Type=Surface to surface, Adjust=0.1
Internal_Selection-1_Ground1_Slave, Internal_Selection-1_Ground1_Master
*Contact pair, Interaction=Surface_Interaction-2, Type=Surface to surface, Adjust=0.5
Internal_Selection-1_Washer_Slave, Internal_Selection-1_Washer_Master
*Contact pair, Interaction=Surface_Interaction-2, Type=Surface to surface, Adjust=0.5
Internal_Selection-1_Bolt1_Slave, Internal_Selection-1_Bolt1_Master
**
** Amplitudes ++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Initial conditions ++++++++++++++++++++++++++++++++++++++
**
**
** Steps +++++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Step-1 ++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Step, Inc=50
*Static
0.01, 1, 1E-05, 1E+30
**
** Output frequency ++++++++++++++++++++++++++++++++++++++++
**
*Output, Frequency=1
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
**
*Boundary, op=New
** Name: Displacement_Rotation-1
*Boundary
164587, 1, 1, 0
** Name: Fixed-1
*Boundary
Internal_Selection-1_Fixed-1, 1, 6, 0
** Name: Displacement_Rotation-2
*Boundary
Internal_Selection-1_Displacement_Rotation-2, 1, 1, 0
** Name: Displacement_Rotation-3
*Boundary
Internal_Selection-1_Displacement_Rotation-3, 1, 1, 0
Internal_Selection-1_Displacement_Rotation-3, 3, 3, 0
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Cload, op=New
*Dload, op=New
** Name: Concentrated_Force-1
*Cload
164587, 2, -9000
164587, 3, -5000
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
*Node file
RF, U
*El file
S, E, PEEQ, NOE
*Contact file
CDIS, CSTR
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
**
** Step-2 ++++++++++++++++++++++++++++++++++++++++++++++++++
**
** Name: Step-2: Deactivated
** Name: CaeModel.FrequencyStep: Deactivated
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
**
** Name: Displacement_Rotation-1: Deactivated
** Name: Displacement_Rotation-2: Deactivated
** Name: Displacement_Rotation-3: Deactivated
** Name: Displacement_Rotation-4: Deactivated
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
** Name: NF-Output-1: Deactivated
** Name: EF-Output-1: Deactivated
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
** Name: Step-2: Deactivated
8

Increased scale factor distorts the bolt, making it hard to see what actually happens there. The T plate is just separating from the base (are those GAP elements visualized between them ?) - regular contact won’t prevent this. As I said, you should start with tie constraints or tied contact and replace them with hard contact one by one to locate the problematic interactions.

9

I just hide the bolt to show how the nodes in area of slotted hole behave.

Now I run the simulation with first order mesh elements and result looks fine. I will try one more time with the second order.

image
image1920×971 99.4 KB

10

Sorry for the late response. How can I upload *.pmx (), when I try I get the message -Sorry, new users can not upload attachments- .

11

Please try with the google drive or wetransfer as I did.

You can also send only exported INP file to reduce the size.

image

12

We transfer link: WeTransfer - Send Large Files & Share Photos Online - Up to 2GB Free
I hope it can be a starting point.

13

Exporting the .inp file is not so helpful in such cases since you often can’t import it back properly due to the current limitations of the .inp importer. Instead, it usually helps to close the results and then save. In the new dev versions you can even compress the .pmx files.

1 Like
14

Thank you for sharing this!

It perfectly shows how small changes and different approach for the same problem can help with the convergence of simulation.

It will help me a lot in the future problems!