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
- Applying a moment Directly

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

09-14-2017 04:49 PM

Hello,

Starting off with a little background, the analysis I’m attempting to run is a bolted Monopole that is about 60 ft tall subject to wind loading. Now I’m not wanting to model 60ft of pole structure otherwise I’d be waiting for the analysis to finish for days so instead i cut the pole leaving a couple of inches protruding above the weld. I have a direct shear value I’m going to add to the pipe, with an additional moment (across the highlighted area) I’d like to add to representing the reaction the pipe provides. I'm still pretty fresh moving from Abaqus to FEMAP so I’m still learning the ends and outs. I've got the model setup with the shear loading but cannot seem to figure out the bending moment portion. Any help would be greatly appreciated.

I have attached an image which shows the configuration along with the highlighted area representing the area which the shear and moment are to be applied to.

-Jerod

7 REPLIES

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

09-14-2017 05:15 PM

Dear Jerod,

You can apply any loading at the surface meshing with an spider rigid **RBE3** element, make sure to activate ALL the six DOFs at the DEPENDENT node (the center node). Also, make sure to activate only the translational DOFs TX, TY, TZ at the INDEPENDENT nodes.

Best regards,

Blas.

PD

1.- To reduce the model size by a factor of 10 and increase the solution accuracy at the same time I strongly success to mesh with HEX 8-nodes elements.

2.- To learn more about RBE2/RBE3 elements visit my blog in the following address:

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

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

09-15-2017 09:13 AM

Blas,

Thank you for your prompt reply. I'm still figuring out all the features and lingo of FEMAP, but I’m guessing RBE3 elements are similar to Abaqus's feature of tying a surface/node-set/element to a single node. That way you can toy with that one node which in return translates to your tied region? Just wanting to make sure I understand the logic behind RBE3.

-Jerod

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

09-15-2017 09:30 AM

Here's a little info from the NX Nastran Element Library Reference:

"The RBE3 element is a powerful tool for distributing applied loads and mass in a model. Unlike the RBAR and RBE2 elements, the RBE3 doesn’t add additional stiffness to your structure. Forces and moments applied to reference points are distributed to a set of independent degrees of freedom based on the RBE3 geometry and local weight factors."

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

09-15-2017 10:08 AM

Blas,

I'm having difficulty defining the point i wish to tie the region to. I have attached an image of what i'm talking about. If i use the "new node at center" its going to throw the controlling node at the COG and not at the center of the pipe. What is the best way to define a new node for this purpose?

-Jerod

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

09-15-2017 11:08 AM

From your screen shot, it appears that you can apply a Torque load to surfaces. You define an axis to apply the torque load around.

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

09-15-2017 11:21 AM

Chip,

The first image i sent only had the shear loading put onto it, i quickly learned trying to add a moment directly to this surface was not working. I'm attempting now to tie this region to a single node and add both the shear (X direction) force and the bending moment loading (about the Y axis). I understand you need to apply the torque about an axis but first i'm trying to tie this region together. Is this not the correct approach?

-jerod

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

09-16-2017 09:33 AM

Chip is correct, the Moment Load in FEMAP gets expanded to nodal moments. For a solid mesh, there are no DOFs in rotation, therefore they don't do anything. Use the Torque load in FEMAP, it expands into nodal forces to achieve the torque specified.

Mark.

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc