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
- CAE Simulation - Femap Forum
- Re: Questions about suport beam linear buckling an...

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

04-23-2017 12:11 PM - edited 04-29-2017 08:26 AM

Dears,

I'm trying a beam linear buckling analysis. A heavy water tank located on the roof of the steel house. There are two girders under the roof and two long beams support the tank. I want to check if these two beams are stable enough, I use buckling analysis to simulate the model. But the results show the side wall of the house will buckled first. This is actually not what I focused. I just want to verify the stability of the beams. Even i try to use Group to see the eigenvalue of the beam, but it does not work at all. Please see below screenshots. What shall I do if I just want to see the results of the beams?

Is there any way to get the force and moment of the top end of the support beams from the results?

What I'm thinking is, build the beams and apply the load from the results, then do the buckling simulation again. I know it maybe a very stupid way but as a newbie, this is the only way what I can think out.

Can any expert guide me to solve this problem? Many thanks.

model file attached.

Solved! Go to Solution.

9 REPLIES

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

04-23-2017 12:26 PM

Dear Gerry,

Use FREE BODY diagram cutting the model by the beams and then you will get the resulting loads in the beams. Next isolate beams in a new model and run the buckling analysis, simply!.

Investigate command **MODEL > LOAD > FROM FREEBODY**, is really powerful ..

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

04-24-2017 11:38 AM - edited 04-24-2017 11:40 AM

Dear Sir,

Thank you so much for the reply. The idea is perfect and I can easy understand logically. But it is still hard for me to follow your methode because I'm not familar with the FEA software. Frankly speeking, I have no much experience with the software. I studied this software by reading the manual and some viedo posted on the YouTube. I enen studied lots of viedo posted by you, although I could not understand Spanish but it doesn't matter, I leaned a lot and thank you and other pepole who shared the experience with the newbie.

Come back to my question, I do build a freebody and can get the loads on each interface nodes. I tried to isolate the beams and apply the loads from the freebody, but I could not simply run the buckling analysis because the boundary of the base model are pinned connection. In this case, the lower end of the support beam is pinned, only loads on the top of the supports beams, it caused a insufficent constraint error. I'm pretty sure I missed something. But I don't know how to deal with.

If I may, could you please be so kind to post a presentation viedo on the Youtube? I know I ask too much, but this is really the good way for a newbie to catch the point.

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

04-25-2017 08:08 AM

Hello!,

Do it the reverse: the resulting reaction force in the base of the beam after performing a linear static analysis SOL101 is directly the loading to apply to the top of the beam to perform a local buckling analysis.

Or using the full model ask for more buckling modes SOL103 untill reaching the local mode shape related with the beam colum meshed with Shell elements ...

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

04-29-2017 08:25 AM - edited 05-07-2017 01:25 AM

Dear Blas,

Thank you very much, it's perfet answer what I'm expect. I try the "freebody tools" today and I think I got your point. I know how to get the intersection moment and force now, that wonderful.

The only thing I still can't manage is how to __"____ isolate beams in a new model"__ as you mentioned before. I really don't know what the exactly meaning of this guide, totally have no idea. Please help me again. Thank you in advance.

PS. I studied your vedio regarding the Global / Local breakout model (submodel) analysis, is that the way to __"____ isolate beams in a new model"__ ?

Best regards.

Gerry

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

05-01-2017 04:24 AM

Dear Blas,

I open opened a new window by FILE - MERGE - FROM GROUP to build the beams, am I correct? Is this so called "__ isolate the beam in a new model__"?

I tried load the eams by means of "loads from freebody" but it still dificult for me to manage. So I try to use load map from model and enforced the intersetction nodes, then run the buckling, I finally got the eigenvalue of the beams.

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

05-03-2017 01:43 PM

I made a video of the entire process of a breakout model of just the beams with the loads from the full model -

Mark.

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

05-03-2017 03:48 PM

I believe the most efficient solution in your case is to ask for more modes from the linear buckling analysis. See the form below which highlights some suggestions. For the lower bound, use a small positive number to prevent the eigensolver from looking for negative eigenvalues. Next select the upper bound, based on the picture from Blas, I picked an eigenvalue of 20.0 and finally set the number of modes to zero or blank, which means Nastran will look for all modes between the lower and upper bound.

The other methods using combinations of Load/from freebody and the global-local tools are good as long as you properly consider the boundary conditions and set up the freebody properly. After inspection of the modfem you provided, I see that in output requests, you did not request force balance, this is required to generate a proper freebody. This may explain the "out of balance" message you received while trying to use the "multi-model" part of global-local.

If you choose to use the submodel or global-local approach, note that just applying the freebody force to beams where you removed the attached structure, is not exactly the same as the boundary provided by the structure you removed. You need to decide based on "engineering judgement" what restraint the removed structure provides. If you add lateral constraints that would likely come closer to matching the results from the buckling run with the complete model.

Highlighted
#
##### Re: Questions about suport beam linear buckling analysis

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

05-06-2017 09:25 AM - edited 05-06-2017 12:21 PM

Dear Mark,

Great job! Thank you somuch for the vedio, very helpful to me.

One more question, I noted the final eigenvalue under the freebody load is 1.728, but Blas's result is 19.121, there is a over 10 times gap. I suppose that the model and the load applied are the same, but why the results are so different.

I trust the freebody diagram methode you showed is generally reasonable.

And I also believe that Mr fembrackin's notice - "note that just applying the freebody force to beams where you removed the attached structure, is not exactly the same as the boundary provided by the structure you removed" is correct. There must have moment and displacement on top of the beam nodes which could not get from the freebody diagram and apply on the beam at the same time. Maybe this the reason why the results have so big gap?

Anyway, I got a lot from both of you, that's great, thank you very much for the sharing.

Best regards

Gerry

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

05-06-2017 02:01 PM

By disconnecting the rest of the structure, I removed a lot of stiffness at the top. Blas' answer is much more realistic. However, by isolating the beams by themselves, and the fact the eigenvalue is still greater than 1.0, is a secondary check that we not buckle under that load, even without the rest of structure stabilizing them.

Mark.

Start with these Femap Basics videos

Watch Femap How To videos on YouTube

Watch Femap Tips & Tricks videos on YouTube

Download the Femap 45 day Free Trial

Download the Femap Student Edition

Watch Femap How To videos on YouTube

Watch Femap Tips & Tricks videos on YouTube

Download the Femap 45 day Free Trial

Download the Femap Student Edition

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc