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
- Heel to Toe Interaction in FEMAP

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

11-26-2015 12:03 PM

Hi,

A colleague who is working on simualting a heel-toe interaction and we were wondering on how to model it in FE.

I suppose one could use 1D Gap elements but our concern is as follows. We replicated the FEMAP supplied 1D cantilever gap contact example and while viewing the deformed model, it seems like the beam didn't really stop at the node which is fixed i.e. the fixed node (the other end of 1D gap element if one end originates from a node on beam) is not acting as a ground.

Was wondering if folks here could point us at some tutorial or literarture on how it can be accomplished using Nastran.

16 REPLIES

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

11-26-2015 02:11 PM

Hello!,

Please post any picture to understabd better your needs, or much better is to post the FEMAP model with the pictures denoting the error, OK?.

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

11-27-2015 03:29 AM

Hi Blas,

I can think of a couple of situations. I am inserting pictures of loading scenarios.

Case 2:

Please feel free to ask further information if needed.

Thx

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

11-27-2015 06:02 AM

Well, depending the detail of your model (global or local) you can use perfectly CGAP elements to define the contact in CBAR/CBeam elements, or surface-to-surface contact in local models meshed with 2-D Shell or 3-D Solid elements; without an specific FEMAP model to comment this is all I can tell you, what´s your problem exactly?.

Best regatds,

Blas.

PD

In the **Support Website** of my company IBERISA you have plenty of problems explained step-by-step of how to use contacts, for instance this one dealing with bolt preload (well, this was the old method having to use a CBEAM element to aplly bolt preload, now with NX NASTRAN V10.2 you can prescribe the bolting preload directly in the 3-D solid mesh of the bolt):

http://www.iberisa.com/soporte/femap/tornillos_pretensados_chexa8.htm

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

11-28-2015 06:37 AM

Dear VN1981,

The **CGAP** element is very, very useful to study **node-to-node explicit contact**, is the classical (nonlinear) contact element we had more than 25 years ago (yes, how old we are!!). Now the CGAP element can be use it in linear static analysis with NX NASTRAN (SOL101) solver, the caution you must have is to activate the option **GAPS AS CONTACT** in the Nastran Bulk Data Options when used in linear static analysis, if not the CGAP will run like a spring element, not contact element.

Here you are an example of using the CGP element with the CBEAM element with multiple supports. The intermediate supports are modeled using CGAP compression-only elements to allow the beam to move free in the positive direction of the Y axis.

If you run the linear static analysis you will see the following results written in the **F06 **file. Also the FREE BODY DIAGRAM is an excellent way to study results, the intermediate support with CGAP element allows the beam element to move free in the vertical direction.

C O N T A C T F O R C E SPOINT ID. TYPE T1 T2 T3 R1 R2 R3 8 G 0.0 3.274576E+03 0.0 0.0 0.0 0.0 13 G 0.0 -3.274576E+03 0.0 0.0 0.0 0.0I N I T I A L C O N T A C T S E P A R A T I O N D I S T A N C EPOINT ID. TYPE DISTANCE 4 G 0.0 8 G 0.0D E F O R M E D C O N T A C T S E P A R A T I O N D I S T A N C EPOINT ID. TYPE DISTANCE 4 G 6.054296E-02 8 G 1.041701E-15

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

11-30-2015 02:17 PM

**Blas,** can explain why after using the *Gap as Contact* disappear from the results of the calculation values Gap X Force, Gap Y Shear Force, etc?

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

11-30-2015 02:57 PM

Hello!,

If you run a genuine nonlinear analysis using NX NASTRAN (SOL106) you will get plenty of CGAP results.

CGAP element forces (or stresses) and relative displacements are requested by the STRESS or FORCE Case Control command and computed in the element coordinate system. A positive axial force Fx indicates compression. For the element with friction, the magnitude of the slip displacement is always less than the shear displacement after the slip starts. For the element without friction, the shear displacements and slip displacements have the same value.

Best regards,

Blas.

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

11-30-2015 03:36 PM - edited 11-30-2015 04:01 PM

~~When the linear solution (SOL101) these results do not have?~~

I understood. When the linear solution (sol 101) using the Gap as Contact no results 3226..Gap X Force, they are replaced by the result 230..Total Contact Force

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

05-15-2016 10:12 AM

Blas,

I was trying out a simple test model for Heel-Toe Interaction between two plates in a cantilever configuration. Obviously, I ran in to issues and I have a few questions to get a better understanding of the process.

1. PGAP Properties: Initial Gap Opening Distance. So this is based on the actual distance between nodes after taking in to account of thickness of plates elements, right? So if I have a scenario where the two plates are 0.1in thick and they are modeled such that, the separation between them is zero after taking thickness consideration, that would be the initial gap opening distance?

A couple of pics to illustrate the structure setup.

The green elements represent CGAP. I have enabled "Treat Gap elements as Contact" options and the analysis is a simple linear static.

2. The second issue I am facing is of 9050 error. I am getting rigid body motion along T1, T2 & R3 directions in one of the nodes connected to CGAP element in the top plate.

So, is CGAP incapable of handling the above type of scenario since there will be an axial load along with bending involved?

I will review NX Nastran manual to find out about the above.

But, I would appreciate any insights from your experience.

Thx

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

05-15-2016 11:26 AM

Thx

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc