Srand7: Global Stiffness Matrix is Singular - Frame with Semi-rigid connections

[tvirkler1]

Hello,

I'm trying a simple frame model with semi-rigid connections as connection elements at the ends of the beam. I was hoping to use connection elements so I can provide nonlinear semi-rigid connection data. Can anyone help me find the issue with my model that prevents the analysis from completing?

 

[IDS]

I am not familiar with using connection elements, or how they work, but I suspect the very high stiffness values you have used may be causing numerical problems. I tried reducing the exponents down from 50 to 10 for translation and 5 for rotation and ran a linear static analysis for gravity loads. That ran without a problem.

Update: I also did a non-linear static run with all the load cases factored by 1. That converged quite quickly. Maximum horizontal deflections were over 11.0 m, so the structure design might need a bit of work!

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[rb1957]

I'm also not familiar with your s/ware, but in my own experience I've had a structure completely supported by springs and I've had to fully constrain a node to take out the rigid body motion of the part. Maybe the same issue. Always check that this rigid constraint isn't reacting any load.

"Wir hoffen, dass dieses Mal alles gut gehen wird!"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[ThomasH]

I am also unfamiliar with the software, but I saw something in IDS post. Exponent 50, if that means numbers with 50 zeros you may have have numerical issues.

 

[tvirkler1]

Thanks for that, all, there’s a few things for me to look into.

To clarify, in the connection element properties which in this software is a type of beam element, I can provide nonlinear moment rotation data for each axis individually (for nla) as well as a rotational stiffness for each axis (for linear). The exponent 1e50 was a value I provided for the linear rotational stiffness for axis 2 and 3 just as a way to fix them and not allow rotation. Previously I would get errors if they were left at 0.

Rb1957, do you mean fully restrain a node laterally? I have fixed supports at the bases of the columns of the frame.

 

[IDS]

To clarify a few things:
I am familiar with Strand7, in fact it's the only FEA package I use regularly these days. It's just I haven't used the connection elements before.

The connection elements have to be assigned a stiffness for translation and rotation in each axis direction. If it is left as zero then there is effectively no connection in that direction, so all the transverse members in the model would be disconnected from the columns.

For the connection elements to be effectively rigid, they should have a stiffness 2 or 3 orders of magnitude greater than the rest of the elements in the model. If they are assigned a stiffness about 10^45 times greater than the other elements, the other elements will effectively have zero stiffness in the global stiffness matrix, so it is not surprising if it is singular when evaluated using numbers with about 15 significant figures.

I have attached a copy of the model with reduced stiffness assigned to the connection elements, which solves with no problem with a static non-linear analysis. I haven't tried the dynamic analyses, but they should work.


Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[ThomasH]

If they are assigned a stiffness about 10^45 times greater than the other elements, the other elements will effectively have zero stiffness in the global stiffness matrix, so it is not surprising if it is singular when evaluated using numbers with about 15 significant figures.

That was exactly what I meant .

 

[IDS]

Any feedback on this?

Did you get it working?


Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/