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 - NX Nastran Forum
- Gap Element using non-linear analysis

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
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-18-2016 05:07 AM

Hi My Brothers

Now I am feeling really sad and frustrated, because my project is going to deadline, however I am not able to work it out. Here is my condition in Femap, help me please.

Now I am doing in-place analysis for a mat-supported jack-up paltform, I want to use gap elements to simulate the real soil condition which can not take tension but can take compression, and gap element rightly has this kind of property. But everytime analysis so far tells me that the computation can not converge, I tried many probable combinations of non-linear setting option, but I still can not reach convergence.

I really hope some expert, friend can help me out, pls pls pls, I am here waiting for your reply.

Solved! Go to Solution.

Labels:

9 REPLIES

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

03-18-2016 05:46 AM

Hello!,

Post your FEMAP model here (or make a small "pilot" study that shows the same behaviour) and document the problem(s) you have, this way we can take a look to it and help you for sure, OK?.

Here you have a FEMAP example explained step-by-step where CGAP elements (among others) were used, and both linear & nonlinear analysis was performed:

http://www.iberisa.com/soporte/femap/soldadura_punto_a_punto.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
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-20-2016 10:16 PM

Hi Bro,

Thanks for your reply, may I ask you in this way: How to modle soil which only provides transverse stiffness, compression, no tension.

Use gap element, or functional spring, or something else?

Cheers

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

03-21-2016 05:03 AM

Hello!,

If you want to study the contact separation/penetration between two bodies then the **CGAP** element is what you need, you can define a compression-only element, simply input a value in the field "Compression-Stiffness", this way the element will work only in compression, allowing freely separation between the two bodies. But take care with singularities, the FE model should be properly constrained, if not you will have the error "**stiffness matrix is singular**".

Also, when defining the linear static study make sure to activate the option "**GAPS AS CONTACT**", if not your CGAP element will behave as an spring:

But if contact separation is not your problem (ALL the element will work always at compression!!), then you can use an spring **CELAS2** element (or a simply CROD element playing with **K=AE/L**, is the same!!). Here you can define different properties for the spring element in function of the influence area of every spring. Take a look to my web site where I explain step-by-step how to solve a spring problem:

http://www.iberisa.com/soporte/femap/nolineal/celas2_nolineal.htm

And if the case where you need to define a nonlinear relation between force vs. length (ie, nonlinear stiffness) then you can use a CBUSH element and solve the problem as nonlinear:

In summary, as you can see you have many options, always use the simplest one !!.

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
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-21-2016 05:53 AM

I really appriciate your reply, now I am trying to use the first method, and the analysis has completed, but it looks somewhere several gap elements are able to carry tension.

Would you mind to leave your email address to me, so that I can directly send the picture to you?

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

03-21-2016 06:04 AM

Hello!,

Tension in CGAP elements is absolutely impossible if you dont have defined any tension stiffness, revise your CGAP properties.

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
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-21-2016 11:17 PM

Dear Molero

Just now, I attempted to use the first method(gap as contact in linear analysis) which you recommonded me. But the behaver of the plate is not consistent with the force arrangement, the plate goes to infinity, and the gap property is compression only, I really have no idea how it behave like that, please have a look and help me.

I attached the gap trial file, please have a look, and give us some comments.

Sorry to disturb you at this time being, hope we have no time zone difference.

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

03-21-2016 11:24 PM

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

03-23-2016 03:42 AM

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

03-23-2016 08:07 PM

Hello!,

This model is impossible to run with success, it will give you error for sure, is not properly constrained. Please note in your model the PLATE is "**floating**" in the space at the very first moment of the analysis, **NOT ANY CONSTRAIN IS PRESCRIBED** in any node of the Shell elements, then the error, OK?.

Please understand the CGAP element is NOT a spring element, is a contact element, at the beginning of the analysis the CGAP element don't have any stiffness, the NX Nastran solver has to perform contact iterations to know the state of every CGAP element of the FE model to see if it is working in tension or compression, ie, to know if the CGAP is open or closed. For a Compression-only CGAP element if the gap is closed then NX Nastran will use its stiffness to compute displacements & stresses in the FE model, but this is after performing the contact iterations.

In summary, your model is singular, you have rigid body motions, then your stiffness matrix is singular and a FATAL error will appear written in the F06 file. When solving contact problems the user should take in account the symmetric & antisymmetric boundary conditions in loads & geometry to stabilize the model, OK?.

You need to define a **HINGE** at the center of the plate simply constraining TX=TY=TZ=0 along the center line, this way you can arrive to a solution (well, the solution is useless, I note you have defined a plate of length = 30e3 mm, and thickness = 2 mm, the the resultant displacement has a value of kilometers, this is all less linear!!).:

Best regards,

Blas.

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

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

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc