Cancel
Showing results for 
Search instead for 
Did you mean: 

Contact in 2D Plane Stress

Creator
Creator

Hi,

 

I am trying to model a plate with a hole in the middle. Then, I create a circle surface with the same diameter as the hole to simulate the case of neat-fit contact. The plate is fixed on one edge, and a load is applied at the center node of the hole. What I'm interested is the contact region between the circle and the hole edge after deformation due to applied load so that I can see how much it has been displaced. 

 

Everything in this model is 2D plane stress( property membrane). I defined contact regions with the option of selecting the curves, but the deformation shows that the circle edges and the hole edges seem to be glued together. 

 

Can someone explain to me what type of contact I should use for 2D plane stress? Any resources would be much appreciated.

 

Thank You

7 REPLIES

Re: Contact in 2D Plane Stress

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

The use of 2-D PLANE STRESS, 2-D PLANE STRAIN and 2-D Solid of Revolution (Axisymmetric) analysis is not clearly explained in FEMAP with NX Nastran, the options are hidden, or bad located and confused (in my opinion). If you plan to study a problem as 2-D Solid Plane Stress Analysis using QUAD 4-nodes elements and the NX NASTRAN solver you need to make sure to define first the correct property using the following steps:

  • Go to MODEL > PROPERTY and in TYPE select PLANE STRAIN (first controversy, why not including PLANE STRESS as well??).
  • Next in FORMULATION under NASTRAN select to use CPLSTSX elements, this is the corresponding plane stress element in NX NASTRAN.
  • And finally in the PLANE STRAIN property (confused, because your element is plane stress) enter the thickness and material.

plain-stress-strain-property.png

Regarding 2-D EDGE-TO-EDGE CONTACT you need to define correctly both the CONTACT REGIONs:

  • In DEFINED BY select CURVES.
  • In OUTPUT select NODES.

CONTACT-REGION-EDGE.png

And you are done, you will be able to solve 2-D contact problems in an easy & fast way: please note this is a linear contact solution, if you have large displacements the solution is not correct.

The following pictures demostrates that a 2-D solution could obtain exactly the same results that solving the 3-D solid model, with the advantage of reduced model size and solution time. In this case is a 2-D axisymmetric analysis, but the same can be applied to plane stress or plane strain problems:

URES_axi_2d.gifURES_CHEXA.gif

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Contact in 2D Plane Stress

Creator
Creator

Hi Blas, Thank you for your prompt reply. 

 

Do I need to define the contact property as well as the connecter for the edge to edge contact ?

 

Sorry for many questions because I'm still new to Femap.

Re: Contact in 2D Plane Stress

Creator
Creator

By the way, Blas, It looks like the pictures that you attached cannot be seen. It shows "the triangle" for all of the pictures. 

Re: Contact in 2D Plane Stress

Siemens Phenom Siemens Phenom
Siemens Phenom

For contact defined using a Connector, you must assign a contact property.

 

When creating a new Connection Property, first, select the Connect Type (Glued or Contact), then push the Defaults button in the Define Connection Property dialog box.

 

For Contact, adjust the values such of Min Contact Search Dist and Max Contact Search Dist appropriate for your connection.

 

For a Glued property, adjust the value of Search Dist.  Note that for NX Nastran, only the first Glued connection property is used, so when multiple glued connections exist in a model, you should set the values for the entire model.

 

2016-08-07_18-10-32.jpg

 

 

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: Contact in 2D Plane Stress

Creator
Creator

Thank you for your reply.

 

I set up the model like how you and Blas suggested, and the contact seems to work fine. Can you explain about the error for me?

 

Capture.JPG

 

 

Re: Contact in 2D Plane Stress

Siemens Phenom Siemens Phenom
Siemens Phenom

Please see Chapter 19 of the NX Nastran User's Guide.  You can access this with the Help > NX Nastran command in Femap.

 

From the User's Guide, note that Membrane and Plate elements are not supported for Edge-Edge contact.  A Membrane element is a CQUAD4 element.

 

Edge-to-Edge Contact Summary
Edge-to-edge contact can be defined on the edges of the following elements:
• Axisymmetric elements CTRAX3, CQUADX4, CTRAX6, CQUADX8.
• Plane stress elements CPLSTS3, CPLSTS4, CPLSTS6, CPLSTS8.
• Plane strain elements CPLSTN3, CPLSTN4, CPLSTN6, CPLSTN8.

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: Contact in 2D Plane Stress

Creator
Creator
Thank You very much Blas and ChipFricke for all your help