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
- Gaps as Contact - Compression Stiffness

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

08-28-2017 04:36 AM

Hi guys,

Quick question about gap elements.

We've always assumed that the compression stiffness value entered is a spring constant value (= to N/mm for the units we use).

I made a few test models and found that gap elements behave as expected when we run nonlinear analyses. 2300 N applied to a compression gap with stiffness of 2300 N/mm results in a 1 mm deflection.

This is not the case for a linear analysis with the option "Gaps as contact" checked. The deflection is zero. As if the stiffness were infinite. So I thought at first, OK, linear contact gaps are just infinitely stiff. But that's not true for low values of compression stiffness. The stiffness is finite! But not the spring constant value one would expect!

Any ideas?

Solved! Go to Solution.

9 REPLIES

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

08-28-2017 05:11 AM

Dear,

CGAP 1-D contact node-to-node elements are running OK in both linear & nonlinear analysis till now, for linear contact you need to activate **GAPS AS CONTACT** option, if not you CGAP elements will behave like an spring with the stiffness defined in the gap properties. If the deflection is zero, it means you got solution error, or the contact convergence is not achived.

Please post your FEMAP model and we can take a look to it.

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

08-28-2017 05:42 AM

Hi Blas,

Thanks for the quick reply. It's not that the gaps aren't working, it's just that the resultant deflections are not as expected.

__First, the test with a spring element: __

__Then, a nonlinear analysis with the gap element: __

__Finally, a linear analysis with the gap element (gaps as contact checked): __

Hope that helps to explain the issue better.

Adam

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

08-28-2017 06:22 AM

Dear Adam,

Post your FEMAP models here and we can take a look to it, the "evil" is in the model, sure!.

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

08-28-2017 06:43 AM

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

08-28-2017 07:02 PM

Dear Adam,

The explanation is easy: your problem setup is nonlinear, then a linear contact static analysis using NX NASTRAN (SOL101) will give you wrong results for sure. Why is nonlinear?. You are mixing very stiff elements & materials with others with low stiff, also the applied load is very high (please remember what is linear static, we run with small displacements). Please note when you run a nonlinear analysis the solver updates both the stiffness & contact matrix at every step increment, and in linear static the solution is unique (well, we have contact iterations as well ...). In summary, do not try to compare linear & nonlinear contact solutions with CGAP elements, the differences are small or negligible only when small displacements & small loadings exist.

A good recommendation: with nonlinear analysis using NX NASTRAN (SOL106) the value of compression stiffness for the CGAP element must be carefully chosen, since a very large value may lead to numerical problems: the closed gap stiffness shouldn’t exceed the stiffness of the adjacent degree-of-freedom by 1000 times.

If you are looking for stiffness in uniaxial direcction, instead to use a **CGAP** element you can use a **CROD** element and play with Young Module **E**, length **L** and cross section **A**, as you know** K= AE/L**.

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

08-29-2017 03:05 AM

Dear Blas,

Thanks for all the time you put into these answers. It's much appreciated.

But still, I think a question is still open. I'll try to make it even simpler. Just a single gap element.

The problem is, for the linear analysis, the gap does not compress according to the given stiffness value! We enter a compression stiffness -- is it too much for me to expect that the gap compresses according to that stiffness?!

The simplified file is attached.

Thanks again,

Adam

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

08-29-2017 09:57 AM

The unexpected behavior for your problem is caused by the interpretation of the PGAP entry when "gaps as contact" is used. This causes the stiffness input on the PGAP to be treated as penalty values in the contact algorithm instead of stiffness values. If you turn off "gaps as contact" for the linear solution then the gaps will behave as ordinary springs with the stiffness values from the PGAP entry.

There is PR 1825260 which describes this issue, see documentation from the PR below:

The closed and open spring stiffness is not supported as such when using linear contact

but instead they are used as the penalty factors in the contact algorithm

Regards,

Joe

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

08-29-2017 10:23 AM

Dear Adam,

Investigating, in your model if you want to obtain the same results between linear & nonlinear analysis simply desactivate the option "**GAPS AS CONTACT**" in the BULK DATA section and the CGAP element will be treated the same as a linear spring element, and remains linear with the initial stiffness dfined in the PGAP entry. The vertical displacement is TZ=-1mm, when the applied load FZ=-2300mm and the GAP stiffness K=2300 N/mm.

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

08-30-2017 03:39 AM

Thanks Blas and Joe!

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc