Contact Issue

  • 156 Views
  • Last Post 3 weeks ago
  • Topic Is Solved
Autonewbie posted this 3 weeks ago

Hi,

I have a contact issue. I have created a contact in between two parts with an existing small gap. I increased the pinball radius to make sure it covers the gap but Part Red or Black still can move across each other. May I know what is the problem? Thank you!

 

Contact Issue

Order By: Standard | Newest | Votes
peteroznewman posted this 3 weeks ago

The best practice is to close all gaps in CAD before you bring the components into Mechanical for simulation. Try that first.

Did you insert a Contact Tool under the Connections folder and then Generate Initial Contact Status?  Please show the table of the status.  This will show if the contact is open or closed or near open.

Autonewbie posted this 3 weeks ago

Hi Peter,

Thank you for your reply. I did check the status and know there is a gap. Do you mean the gap should be closed in the simulation even it is physically exist in real time?

For example the picture below that there are two gaps pointed by red arrow, are you suggesting to close both the gaps?

Thanks!

peteroznewman posted this 3 weeks ago

No, those gaps don't need to be closed. Any gap between the bottom edge of the rectangle and the two ledges it is sitting on would best be closed.

Please show the table of the status.  This will show if the contact is open or closed or near open. There is a big difference between a gap that is open and one that is near open and you use a Pinball radius to change an open gap to a near open gap.

Near open means the contact algorithm is monitoring that gap from the beginning of the simulation.  Open gaps don't get this special treatment, which means if there is a large motion in the first increment, the surfaces can go past each other. That doesn't happen so much with near open gaps.

Autonewbie posted this 3 weeks ago

Hi Peter,

I did run the contact status check and no Open contact but some Near Open contacts. I tried to use frictionless with Pure Penalty but the part is still passing through each other although there is contact defined.

Sorry for not able to upload the model. I made a simple description below. The contact defined at Up-Down direction is closed status. All other contacts defined for Front-Back and Left to Right are Near Open.

Some gaps are pretty big but contact was defined to prevent the mating part deflecting too large (observed from previous analysis). However, it is Near Open status.

From the latest run result, the top part is still passing through the bottom from left to right. Note that the bottom was fixed at the bottom area. Thank you so much for your time!

 

peteroznewman posted this 3 weeks ago

Autonewbie, 

Under Analysis Setting,  set the Auto Time Step to On.

Set the Initial Substeps to 100 and the Maximum Substeps to 200.

Set Large Deflection to On.

Does that help.

Autonewbie posted this 3 weeks ago

Hi Peter,

It works when I increase the time steps. However, I still got some warning and error messages below:

 

 *** ERROR ***                           CP =     417.859   TIME= 20:12:11

 Element 35092 (type = 6, SOLID187) (and maybe other elements) has       

 become highly distorted.  Excessive distortion of elements is usually   

 a symptom indicating the need for corrective action elsewhere.  Try     

 incrementing the load more slowly (increase the number of substeps or   

 decrease the time step size).  You may need to improve your mesh to     

 obtain elements with better aspect ratios.  Also consider the behavior  

 of materials, contact pairs, and/or constraint equations.  Please rule  

 out other root causes of this failure before attempting rezoning or     

 nonlinear adaptive solutions.  If this message appears in the first     

 iteration of first substep, be sure to perform element shape checking.  

 

 *** WARNING ***                         CP =     740.297   TIME= 20:17:55

 Contact element 309083 (real ID 26) status changes abruptly from        

 no-contact -> contact (with target element 308969). 

 

The deformation looks as what I expected but the result scale is deactivated. 

 

Also, I do not know why at true scale, the deformed part still overlapped with the fixed part? I expect the deformed part (with color contour) pushing against each other.

 

peteroznewman posted this 3 weeks ago

When a solution does not complete incrementing the load, it extrapolates to the full load for diagnostic purposes. Look at the tabular data for a result. If the full load was applied at 1 second, and the last converged time step was 0.34 seconds, for example, select the row with 0.34 seconds and Retrieve This Result.  You may find the contact looks better at a converged substep, and not at the extrapolated end time that is unconverged.

You can adjust the time step and change the Minimum Substeps to 100 to see if this helps.  Otherwise, you may need a more refined mesh to avoid the excessive distortion error.

If there is still too much penetration on a converged substep, you can edit the details of the contact and specify an allowable penetration.

Autonewbie posted this 3 weeks ago

Hi Peter,

All problems solved after reducing the time steps.

However, there is one large penetration contact is not able to be detected and highly distorted elements found at contact area after adjusting the pinball radius.

I have refined the contact area either using sphere or surface (try to cut down number of elements) up to 2X but still see the error. Note that the contact is a very tiny contact flat surface to large target flat surface.

peteroznewman posted this 3 weeks ago

For the one contact that still has too much penetration, adjust the Normal Stiffness and set a factor of 10 or even 100 to increase the normal stiffness and reduce the penetration.

Autonewbie posted this 3 weeks ago

Hi Peter,

I tried to adjust the FKN up to 100 and it did not work at all. Residual force found. I tried to reduce FKN to 0.01, it started with very high convergence force and cannot converge.

Do you have any advice?

Besides, does it affect the contact stress by changing the contact stiffness as the large interference fit is designed in such way? Thank you!

 The error messages below obtained when I changed the FKN to 0.01

 

 *** WARNING ***                         CP =     231.000   TIME= 00:16:26

 Contact element 507271 (real ID 31) has too much penetration 1.23279129 

 related to target element 507720.  Please verify the pinball radius.    

 

 *** ERROR ***                           CP =     302.266   TIME= 00:179

 Element 61484 (type = 8, SOLID187) (and maybe other elements) has       

 become highly distorted.  Excessive distortion of elements is usually   

 a symptom indicating the need for corrective action elsewhere.  Try     

 incrementing the load more slowly (increase the number of substeps or   

 decrease the time step size).  You may need to improve your mesh to     

 obtain elements with better aspect ratios.  Also consider the behavior  

 of materials, contact pairs, and/or constraint equations.  Please rule  

 out other root causes of this failure before attempting rezoning or     

 nonlinear adaptive solutions.  If this message appears in the first     

 iteration of first substep, be sure to perform element shape checking.  

peteroznewman posted this 3 weeks ago

Do you have a large interference designed into the geometry that you want the contact algorithm to resolve? 

If penetration is there at the beginning, that was not clear before and requires a different approach.

Please show the geometry at the start of the simulation.

 

Autonewbie posted this 3 weeks ago

Hi Peter,

Yes. The large interference was designed into the geometry. Sorry for the vague question.

I could not reveal the geometry due to the company policy but I draw a simple geometry below. 

 

 

Please note that there is a tiny flat surface of the rounded end at the large interference fit location.

 

Thank you for your time!

peteroznewman posted this 3 weeks ago

A simple solution is to move the blue part down in CAD to make it tangent to the tip of the finger as an initial position. Then in step 1 of the solution, a displacement is applied to the blue part to move it up to the correct position. In this way, there is no large penetration at the beginning of the simulation and at the end of the simulation, the proper deformation is created.

  • Liked by
  • Autonewbie
Autonewbie posted this 3 weeks ago

I like this idea. There is another risk that if you look at another side of the blue part, there is a catcher which is touching the blue part. If the blue part is moving down, the catcher will experience large interference fit also.

peteroznewman posted this 3 weeks ago

If you can't do the simplest solution, here is another solution, use element birth and death to kill the contact in step 1, and have a displacement load move the tip of the finger up to be level with the surface of the blue part. Then in step 2, make the contact come alive, then in step 3, deactivate the displacement load.

A similar method is to use a force to move the tip of the finger up, then in step 3, set the value of the force to be zero.

One thing to try first is to change the Contact Definition and let the solver try to resolve the contact with no other steps.  Under the Contact Details, in the Advanced category, change the Detection Method to Nodal-Normal To Target.  That assumes the blue surface is the Target and the finger is the Contact.  This might cause the algorithm to create forces to push the interference upward. The default might have been creating forces that pushed the finger inward, which is not useful.

  • Liked by
  • Autonewbie
Autonewbie posted this 3 weeks ago

Hi Peter,

 

That sounds complicated but I am trying to run it in different way. I move the fingers up and touching the blue body surface. And all the fingers are chopped with tips only. Apply displacement on the fingers and define contact with no interference fit between finger and blue body.

It still take pretty long to run ... and I guess another issue is also due to the very small contact area between finger and blue body. If it is still cannot converge, will change the detection method to projection.

Close