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
- Re: Help with modelling rigid elements on a sandwi...

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

Wednesday - last edited Wednesday

Hi all,

First time posting here, but I have a Femap problem that is most likely very easy to clear up. I am modelling a composite sandwich structure in Femap for a chassis plate design with multiple elements attached to the plate. When I have meshed my plate with laminate properties, and I attempt to create RBE2 mass elements and tie them to my plate using rigid elements, I cannot run any correct analysis. I am curious to what basic things I may be overlooking as I am extremely new to the world of FEA and am running this analysis for a project, and being taught Femap in my spare time. I've tried to use RBE3 as well.

Please check out the neutral Femap file that I have attached and look at the analysis sets to get a picture of the problem. I've been running normal modes analysis to try and see where my errors are. I think that it may have something to do with rigid elements in general, but like I said I am very very new to this and doing this all in my spare time. Any thoughts are appreciated! Thank you, Ethan

file : https://drive.google.com/open?id=1-P7BS4a_m1Oh3nZhMdiPg3W5a5OiTXv4

4 REPLIES

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

Wednesday

I'm not sure what you mean by 'correct analysis'. I was able to run this model without errors when using RBE3's to attach the Mass elements to the mesh.

However, I'm curious about your stiffness values for the material HC (honeycomb core material?). These are very low values and can definitely contribute to suspect results.

Finally, when running a model with laminates, I recommend that you also enable the PARAM,SRCOMPS card as shown below to output Ply Strength Ratios.

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

Wednesday

I got for the Laminate Failure Index was extremely low, around 0.000143,

which would imply that I had an extremely strong laminate that was nowhere

near failure.

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

Thursday - last edited Thursday

Have you looked at the stiffness of your laminate as shown below? The bending stiffness is high, and with the small loads you have on this plate and with a almost zero stiffness of the honeycomb, you're getting higher strains on the XY plane vs bending.

I recommend that you run a test coupon model of this with loads in both axial directions and a simple fixed-fixed beam with a center load to see the behavior.

Laminate Equivalent Properties

11 Plies - Total Thickness = 0.037

In-Plane Properties

Ex = 3.1202E+10 Ey = 3.1202E+10 Gxy = 1.3577E+10

NUxy = 0.524589 NUyx = 0.524589

Alphax = 0. Alphay = 0. Alphaxy = 0.

Bending/Flexural Properties

Exb = 5.5038E+10 Eyb = 4.8873E+10 Gxyb = 2.5432E+10

NUxyb = 0.586824 NUyxb = 0.521089

Alphaxb = 0. Alphayb = 0. Alphaxyb = 0.

A Matrix

1.60150E+9 8.44254E+8 -6.6241E+7

8.44254E+8 1.60150E+9 -6.6241E+7

-6.6241E+7 -6.6241E+7 5.05926E+8

B Matrix

-1.1642E-8 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

D Matrix

3.37445E+5 1.77176E+5 -1.7413E+4

1.77176E+5 2.99957E+5 -1.7413E+4

-1.7413E+4 -1.7413E+4 1.08580E+5

A-Inv Matrix

0.00000E+0 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

B-Inv Matrix

0.00000E+0 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

0.00000E+0 0.00000E+0 0.00000E+0

D-Inv Matrix

4.30442E-6 -2.5259E-6 2.85213E-7

-2.5259E-6 4.84742E-6 3.72294E-7

2.85213E-7 3.72294E-7 9.31524E-6

Using RBE3s (the proper way to load a model using Mass Elements, I get a max Failure Index of 1.78e-5 as shown below.

Best Regards,

Chip Fricke

Principal Applications Engineer - Femap Product Development

Chip Fricke

Principal Applications Engineer - Femap Product Development

Highlighted
#
##### Re: Help with modelling rigid elements on a sandwich structure plate

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

Saturday

Hello!,

As an add-on to great Chip comments if you run a normal modes/eigenvalue analysis using NX NASTRAN (SOL103) and plot the deformed mode shapes you can see the weird behaviour of the composite: you have a problem with material properties values for axial & bending stiffness.

In fact, revising the material properties of HC material (core Honeycomb) I see that a value of EX = 1 Pa = 1e-6 MPa is used, this could cause to have a very low stiffness for shear & bending in the core:

To learn more in composites take a look here:

http://www.iberisa.com/soporte/femap/composites/nafems_benchmark_composite_test_r0031_3.htm

To learn more about RBE3 vs. RBE2 take a look here:

https://iberisa.wordpress.com/2015/10/13/rbe2-vs-rbe3-on-femap-with-nx-nastran/

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/

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc