Jump to content
LFSS

Working with Rigids

Recommended Posts

Hello everyone. 

 

I'm working on a project which consists of a rod-trussed structure .I'm having some difficulties working with rigids. I have followed the Altair's student frame linear static analysis.

Since I need my SPC to be in a rigid, the configuration is this one:

image.thumb.png.f0de64d5f9f94c89716b284863cc3673.png

 

I am using two rigids: one for the SPC and another one for applying a force (brown line). Whenever I use the configuration above, OptiStruct says there's dependency between rigids (because the two rigids are applied to the same node). So, in order to fix that, I have tried this configuration:

image.thumb.png.d4fb125afd4ba97105af8da5115b2a8c.png

 

Which yields this result: 

image.thumb.png.9a8a733bbddd8c520d49deb984f98d31.png

 

But if I try to run a different configuration (for example, linking the SPC rigid to 3 nodes, except the one where the force rigid connects), I get this result:

 

image.thumb.png.811b57eec848c3244d82d8e2d1c6e3ea.png

 

Which basically zeroes my displacements and stresses in the model. I have no ideia which one is giving me more realistic results and I'd could use some help trying to figure it out!

 

Thanks

File_Forum.hm

Edited by LFSS
Added model file

Share this post


Link to post
Share on other sites

your rigid elements (yellow, and brown) are composed of only 1 rbe each, or are they made of 2 small elements each?

 

If you are using 2 rigids for creating each one, make sure that the independent node is the middle one for both of them. The independent node should be the one with SPC.

 

For the force it is ok. Alhogh maybe a RBE3 would be better to avoid adding stiffness.

Share this post


Link to post
Share on other sites
1 hour ago, Adriano A. Koga said:

your rigid elements (yellow, and brown) are composed of only 1 rbe each, or are they made of 2 small elements each?

 

If you are using 2 rigids for creating each one, make sure that the independent node is the middle one for both of them. The independent node should be the one with SPC.

 

For the force it is ok. Alhogh maybe a RBE3 would be better to avoid adding stiffness.

 

They are composed of two rigids, one for yellow and one for brown. I've made sure the middle one is the independent node for both of them, as well as where the SPC and the force is applied. What's the difference for an RBE3? is it better for my case?

 

Share this post


Link to post
Share on other sites

RBE2 creates a kinematic condition between nodes, thus artifical stiffness is added to your model. So the dependent DOFs will follow exactly what the independent DOF does. That's why it is called rigids.

RBE3 is used for load and mass distribution, and does not add stiffness to your nodes. Dependent node will be calculated from "an average" of the independent nodes. Actually it depends on the weighting factors.

 

Maybe sharing your model would make it easier to check what is going on.

Share this post


Link to post
Share on other sites
14 hours ago, Adriano A. Koga said:

RBE2 creates a kinematic condition between nodes, thus artifical stiffness is added to your model. So the dependent DOFs will follow exactly what the independent DOF does. That's why it is called rigids.

RBE3 is used for load and mass distribution, and does not add stiffness to your nodes. Dependent node will be calculated from "an average" of the independent nodes. Actually it depends on the weighting factors.

 

Maybe sharing your model would make it easier to check what is going on.

I understand. I'll try it later today.

I've attached the model file to the original post.

Share this post


Link to post
Share on other sites

I think I didn't get what you see as a problem.

 

Running your model as it is, this is what I got (just adjusting the legend a little bit, and adding a couple 'measures').

By adding a RBE2 you're essentially imposing that the same ZERO displacement (SPC 123456) of the central node will the carried to the 3 nodes connected to it.

Which is exactly what you got here.

For sure you should look again at what are the BCs in your real structure and try to bring them to your model.

 

There is some stress in the whole structure, although it is low compared to the stress in the red regions.

 

For buckling you requested only the 1st mode, which is ok, as it is the lowest one, but you would probably want to look at others too.

 

image.thumb.png.9473408559b54c60a2a2d2b2d524bc1f.png

image.png

LFSS likes this

Share this post


Link to post
Share on other sites

That's interesting.

So the difference between my first model (with the SPC rigid linked to 2 nodes) to my second one (SPC rigid linked to three nodes) is that in the second one I get a overstiffened structure relative to the first one, did I get it right?

 

As for the buckling, thanks for the advice!

 

Just out of curiosity, how do you display the tubes like that? I only get the line contour, but this one you showed here has a better visualization!

Share this post


Link to post
Share on other sites
20 hours ago, Adriano A. Koga said:

correct. 

2nd model was stiffer thatn the 1st one.

 

This image was just a display, not the real section.

I went to Preferences and turned on visualization for 1D elements as a cylinder.

image.png.108bd2f8da9b30c9bf98243efecb46a2.png

Thanks a lot man! 

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...