turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- Contact in 2D Plane Stress

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-06-2016 01:18 PM

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

Solved! Go to Solution.

7 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-07-2016 04:47 AM

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.

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**.

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:

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/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-07-2016 07:16 PM

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.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-07-2016 09:08 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-07-2016 09:19 PM

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.

Best Regards,

Chip Fricke

Principal Applications Engineer - Femap Product Development

Chip Fricke

Principal Applications Engineer - Femap Product Development

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-07-2016 11:29 PM - edited 08-08-2016 01:44 AM

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?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-08-2016 12:59 AM

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

Chip Fricke

Principal Applications Engineer - Femap Product Development

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-08-2016 01:46 AM

Thank You very much Blas and ChipFricke for all your help

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc