Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

Questions about suport beam linear buckling analysis

Pioneer
Pioneer

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?

 

20170423233152007.png20170423233311569.png

 

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.

 

 

9 REPLIES

Re: Questions about suport beam linear buckling analysis

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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/

Re: Questions about suport beam linear buckling analysis

Pioneer
Pioneer

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.

 

 

Re: Questions about suport beam linear buckling analysis

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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 ...

PANDEO-MODO40.png

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/

Re: Questions about suport beam linear buckling analysis

Pioneer
Pioneer

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.

 

FREEBODY.png

 

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

Re: Questions about suport beam linear buckling analysis

Pioneer
Pioneer

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. 

Re: Questions about suport beam linear buckling analysis

Siemens Phenom Siemens Phenom
Siemens Phenom

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

 

(view in My Videos)

 

Mark.

 

Re: Questions about suport beam linear buckling analysis

Siemens Phenom Siemens Phenom
Siemens Phenom

2017-05-03 15_18_22-NASTRAN Buckling Analysis.pngI 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.2017-05-03 15_35_07-NASTRAN Output Requests.png

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.

Re: Questions about suport beam linear buckling analysis

Pioneer
Pioneer

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 differentMan Surprised.

 

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

Re: Questions about suport beam linear buckling analysis

Siemens Phenom Siemens Phenom
Siemens Phenom

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.