Discussion Groups

Simulation Mechanical and Multiphysics

Reply
Active Contributor
isaacc
Posts: 30
Registered: ‎01-11-2013

Surfaces will not contact...

792 Views, 10 Replies
01-29-2013 10:23 AM

Surfaces.JPG

 

The surfaces in my model will not contact. I have tried selecting just the two faces, the whole parts, etc. I have done linear, nonlinear, and MES... I have no idea why they keeps passing through each other.

Please use plain text.
Employee
zhuangs
Posts: 246
Registered: ‎10-04-2010

Re: Surfaces will not contact...

01-29-2013 11:36 AM in reply to: isaacc

You might upload the model for us to easilly investige it.

 

-Shoubing

Please use plain text.
Active Contributor
isaacc
Posts: 30
Registered: ‎01-11-2013

Re: Surfaces will not contact...

01-29-2013 11:50 AM in reply to: zhuangs

Ok I will as soon as I get a chance! Could it be because the part is not actually touching, just exaggerated to touch?

Please use plain text.
Employee
zhuangs
Posts: 246
Registered: ‎10-04-2010

Re: Surfaces will not contact...

02-05-2013 12:15 PM in reply to: isaacc

It seems that the contact is not detected.  I am wondering whether the contact is well set up between the surface really in contact.

 

-Shoubing

Please use plain text.
Member
charsguo
Posts: 4
Registered: ‎01-26-2013

Re: Surfaces will not contact...

02-16-2013 09:30 AM in reply to: isaacc

I have the same problem.

 

I'm working on a FEA of a climbing carabiner (oval-shaped; one side of the oval is a gate which opens and closes allowing a rope into the carabiner).

 

The gate of the 'biner has a hook which attaches to the "nose" of mainbody/biner.  However, this hook does not engage until the biner slightly deforms.

 

I've attempted to use the separation/no sliding contact option, but the solver behaves as if there is no contact occuring.  The nose simply passes right through the gate hook.

 

The initial gap of the system is about 0.040".  That means the nose must deflect 0.040" before the contact surface comes into play.

 

Any help would be greatly appreciated!

Please use plain text.
*Expert Elite*
AstroJohnPE
Posts: 521
Registered: ‎08-30-2012

Re: Surfaces will not contact...

02-16-2013 12:47 PM in reply to: charsguo

Hi charsguo and isaacc,

 

I suggest that both of you create an archive of the models and attach them to the reply. It would make it much easier to find the probem.

 

See this thread for instructions on archiving.

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
*Expert Elite*
AstroJohnPE
Posts: 521
Registered: ‎08-30-2012

Re: Surfaces will not contact...

02-17-2013 03:34 PM in reply to: AstroJohnPE

In Charlie's case, the analysis type was set to linear static stress. Contact only works in this analysis type when the gap/interference is 0. If the initial gaps are not critical to the design, I suggest that you remove them from the CAD model and start the process again. If the gap is critical to the design, then you must use an analysis type of "Nonlinear > MES". MES is the only analysis type that can handle surface contact between two surface with a gap.

 

For more information, see the page "Types of Contact" in the wikihelp. I will try to submit an update to the page to help make it clearer that contact requires a 0 gap in most situations.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
Member
charsguo
Posts: 4
Registered: ‎01-26-2013

Re: Surfaces will not contact...

02-21-2013 05:34 AM in reply to: AstroJohnPE

John,

 

This fixed my problem.  Many thanks!

Please use plain text.
New Member
Junior_Brown
Posts: 2
Registered: ‎06-04-2013

Re: Surfaces will not contact...

06-04-2013 12:18 PM in reply to: AstroJohnPE

Hello Guys,

 

Could you please help? I am trying to analyse stresses in a spur gear during a complete rotation (i.e. 360 degrees). The pinion is rotating at a rate of 300 rpm and the main gear has a resisting torque of 225 in-lbs.  The pinion and gear teeth pass through each other without making surface to surface contact. Even though I am running the analysis within a Mechanical Event Simulation environment.

I have tried various ways to create surface contact pairs by assigning them manually as well as automatically (i.e. all surfaces on part 1 to all surfaces on part 2) but they still fail to make contact. I have even extended the analysis time but that did not work.  

 

I have spent many hours trying to diagnose what the problem is and I am beginning to think that the simulation cannot be done with this software.  Is it possible? Can someone please help. I Cannot upload the ach file because of file size limitation on the forum. Please see attached  jpeg file showing the gear teeth passing through each other. Thanks. 

Please use plain text.
*Expert Elite*
AstroJohnPE
Posts: 521
Registered: ‎08-30-2012

Re: Surfaces will not contact...

06-05-2013 08:36 AM in reply to: Junior_Brown

Hi Junior Brown,

 

It will be challenging to diagnose the model without having it. Did you read the thread "Create, Post, or Provide an Archive of your model" for tips on reducing the size of the archive?

Otherwise, here are some things to check:

  1. Read the log file from the Report environment. Just before the section that shows the time steps and iterations, the log file lists how many elements are in each part. Does the number of contact elements seem reasonable? (Be aware that the number reported is the initial number of elements. It can go up or down depending on the contact situation at each time step.)
  2. Do the reaction force results show any contact occurring between the teeth? If so, the contact stiffness can be increased to help prevent the teeth from passing through each other.
  3. What is causing the stress in the pinion? (I presume the blue color in your attached image indicates a non-zero stress. Please include the legend in future plots to help us interpret the image.)
  4. What version of the software are you using? (The annotation and legend colors imply a really old version, but perhaps you like that color scheme :-) The current version (2014) has some enhancements related to contact that would be helpful to you. (Such as grouping the  teeth surfaces so that you only need to define one contact pair, etc.)
  5. Until you get the bugs worked out, I suggest that you reduce the contact to just a few teeth.
  6. Why do you want to do a full rotation of the spur gear? Does something change so that the results after 360 degrees rotation are different than after 90 degrees? (2+ teeth on the pinion)
  7. Another option is to perform the analysis using 2D elements. Smaller model, faster run time. This can be done if the two gears are the same width (or you are willing to neglect the effects that occur when they are different widths.)

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.