B31/C3D8R in contact

[Ciara895]

Hi, I'm trying to wrap a polymer sheet (C3D8R elements) onto a wire (B31 elements) using a pressure applied to the sheet. The wire component is completely fixed. Currently I have general contact with a penalty applied to the entire model. The polymer sheet passes about 1/3rd of the way through the wire before it looks like it comes into contact. Does anyone have any suggestions on how I could change this so that polymer wraps around the outer edge of the beam element?

Thanks!

 

[FEA way]

First of all make sure that perspective is turned off when you create this contour plot (it often leads to confusion regarding deformed shape of the model). Also consider increasing mesh density and using solid or discrete rigid elements for the bar.

 

[Ciara895]

Thanks for your comment. Perspective is already off unfortunately. This simple simulation is a test for a much bigger and more complicated simulation, so it's not feasible to move to solid elements for the bar. I can't understand why it isn't recognising the beam profile, but yet it doesn't completly ignore the profile and travel to the center wire.

 

[FEA way]

Is it Standard or Explicit ? What are the contact properties ? Rigid elements would be the best option, especially that you want to run larger model. Unless you are interested in the deformation of the bar as well.

 

[IceBreakerSours]

As implicitly suggested above, scale up the contact stiffness by an order of magnitude or two and see how that impacts the results.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Ciara895]

Thanks for your advice. This simulation runs with the expected contact in Standard, but doesn't in Explicit. I discovered this problem is related to the following error in Explicit:

***WARNING: In step 1, some contact edge thicknesses for general contact were reduced from the parent element or specified values due to a large thickness compared to edge dimensions. The most significant thickness scaling factor was 0.600 for an edge on parent element 5 of instance BEAM-1. An element set named "WarnElemGContThickReduce" has been created to locate the regions of reduced thickness.

I solved the problem by making the beam mesh more coarse. With a coarse mesh on the beam, the sphere representing thickness at each node doesn't overlap, hence the contact edge thickness isn't reduced and the contact will behave how I want it to. Further information can be found in the Abaqus docs - "Control of contact thickness reduction checks".