Robot Structural Analysis Forum
Welcome to Autodesk’s Robot Structural Analysis Forums. Share your knowledge, ask questions, and explore popular Robot Structural Analysis topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Is it possible to limit a bar force to a certain value?

18 REPLIES 18
Reply
Message 1 of 19
Rafacascudo
891 Views, 18 Replies

Is it possible to limit a bar force to a certain value?

I want to limit the axial force of a columm or a vertical reaction force to 90tf .I tried using nonlinear supports but it didn´t work. Is there a way to do this?


Rafael Medeiros
Robot Structural Analysis

18 REPLIES 18
Message 2 of 19

Either using  a non-linear release or a non-linear support. Mind to set the parameters of the non-linear analysis as shown on the attached picture.

 

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.



Artur Kosakowski
Message 3 of 19

Hi Artur

  That´s exactly what I tried to do  except for marking " matrix update after each iteration" . But also doing that I keep getting a zero reaction value where I get 100tf when the UZ direction is fixed



Rafael Medeiros
Robot Structural Analysis

Message 4 of 19

Please send the model and indicate the node number and load case to look at.



Artur Kosakowski
Message 5 of 19

Artur,

     I solved the problem using Bilinear model with a very high K (10000000)for the 1st spring, zero K for the 2nd spring and a corresponding D1 for the force I wanted to limit.It worked great!

     But now I´m having a weird problem when running the model.I have like 120 combinations and ,it takes like 20secs to solve each one .But after something like 25 combinations ,it starts to not converge. So I stopped the calculations ,deleted most of combinations and only left some that robot reported as non convergent.Ran it again without saving the model and to my surprise they converged also in 20secseach  and without using  " matrix update after each iteration" !!!

Nodes with non linear supports are  10 ,21 ,32 ,33 . Combinations are 41,73,75,89

Model is attached. Rename it to .rar



Rafael Medeiros
Robot Structural Analysis

Message 6 of 19

Try to use the parameters from the attached picture. I have calculated the model and all combinations converge.

 

Case 132

: 1,35xPP+1,05xSC+0,84xVTsuc+0,84xVT270-1,2xTPgrad

Analysis type:

Nonlin. Combination

  

Non-linear process: convergent.

Maximum value of process parameter when convergence is obtained

: 1.000

Maximum value of process parameter when convergence is not obtained :

1.000

 

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.



Artur Kosakowski
Message 7 of 19

Thx a lot  Artur,

It worked.

  But What I don´t understand is why a combination that doesn´t converge in the first run (without marking "matrix updating after each iteration"), converges if I use calculation restart without modifying anything?

Why the calculation process behaves differently??

The problem is solved, but I´d like to understand that.

thx



Rafael Medeiros
Robot Structural Analysis

Message 8 of 19

I have to admit that I do not fully understand the sequence of actions you made and the idea behind them. Definitely deleting some of the load cases/combinations while the analysis was terminated and then restart of the analysis is not the thing I personally do. The intention of this option was to change the parameters of the analysis when you can see that the process has got little chance to converge with the current settings. I can try to investigate this situation providing you give me the detailed (step by step) description to follow.  As you could see all I did was to use the settings I suggested before Smiley Wink

 

BTW: Have you checked in the calculation report that they actually converged?



Artur Kosakowski
Message 9 of 19

Artur,

 

    For just an example to show you ,I limited last load case to be number 41.Combinations 39,40 and 41 don´t converge in the 1st run .After I get the no convergence warning for load case 41 ,I just  click OK and do an analysis restart for just case 41 without changing any settings.The result is completely different and now the combination converges

Watch it in this video.

 

http://screencast.com/t/jbHGlJc2z



Rafael Medeiros
Robot Structural Analysis

Message 10 of 19

As far as I can see Robot starts to have difficulty to converge the last of many non-linear cases for the BFGS method and the multi-threaded solver (when you restart calculations or delete some of the previous cases then divergent cases will converge). Thank you for pointing this situation out - we will check what exactly happens.

 

The solution is to either use the Full Newton-Raphson method for the multi-threaded solver (the settings I used) or use the Automatic solver (Sparse_M in this case) for the BFGS method.



Artur Kosakowski
Message 11 of 19

Ok Artur,

 

Thanks!



Rafael Medeiros
Robot Structural Analysis

Message 12 of 19

As far as I can see Robot starts to have difficulty to converge the last of many non-linear cases for the BFGS method and the multi-threaded solver (when you restart calculations or delete some of the previous cases then divergent cases will converge). Thank you for pointing this situation out - we will check what exactly happens.

 

Corrected in Robot 2015.

 

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.



Artur Kosakowski
Message 13 of 19

Great!!


Rafael Medeiros
Robot Structural Analysis

Message 14 of 19
Rafacascudo
in reply to: Rafacascudo

Is it possible to limit a bending moment (directly) in a shell structure?? thx


Rafael Medeiros
Robot Structural Analysis

Message 15 of 19

No, it is not possible.



Artur Kosakowski
Message 16 of 19

   I think ( still testing) I found a way to do it using non-linear bar releases .

Structure to the left - panels are normally connected

Structure to the right - Exact same structure ,(with same load ,10tf/m2 on the top slab area) except that the vertical panel is 2cm shorter   . Mesh is 1 mt . Created very stiff bars (2cm) connecting the panels at each node. Then I created a non-linear release limiting the moment at 25tf.m(12.5tf.m on the sides) using " rigid with linear hardening" type. Seems to be working nicely. For a load that does not reach 25tf.m on that edge , both structures show the same bending moment. Is there anything else that I should be aware?

 

Non linear releases for shells.jpg



Rafael Medeiros
Robot Structural Analysis

Message 17 of 19

Very very nice work Rafacascudo, take a look to the stress distribution in the panels. I think that the over value of the bending moment is due to the shear force applied in the point linked by the 20mm non linear released bar. This could be a solution for your problem, my suggestion (I've never tested before) is to try to use compatible nodes in common line of the panels. Just for test, this can be an elegant solution.

Greetings

PasProStudio

www.pasquiniprogetti.eu

Structural + Detailing engineers
Message 18 of 19
Rafacascudo
in reply to: Rafacascudo

Hi Stefano,
I used the 20mm bars as rigid links. I didn't show the panel moment maps but they are perfectly normal with no spike moments values. I thought about compatible nodes but I think they can only be used with bars.


Rafael Medeiros
Robot Structural Analysis

Message 19 of 19

 I thought about compatible nodes but I think they can only be used with bars.
It is the only way you can define (or shall i wrote control to which object they are assigned) them but you may achieve this goal in the following way:
1. Define compatible nodes (with the intended nonlinear function) at the intersections of bars created at the intended location of a common edges of panels.
2. Delete bars
3. Move one of the set of nodes either vertically or horizontally
4. Define panels with (temporarily separated) edges at the lines of these nodes and mesh them (make sure the generated meshes match number of nodes along the edges)
5. Freeze meshes
6. Move the 'shifted' nodes (as well as the panel's edge if you want) to their 'original' locations

 



Artur Kosakowski

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report