Problem with Strand7 analysis

[DiegoAl]

Hi, i tried to model a structure that supports a pebble crusher and when i assigned a pinned connection to some beams of the model (using Attributes/Beam/End Release/Rotation/1 and 2:Rel), the following error appears in the linear static solver: Global stiffness matrix is singular. And i couldn't figure out why is that.
Then i tried to model a simpler case and i have the same error:

Global Stiffness Matrix Singular at Equation 7: Pivot = 0.000000E+00 (Node 5 DX)

*ERROR[ 4]:Global stiffness matrix is singular.

I just create 3 beams, 2 simply supported and the other one connected to them, then assigned a geometry to the beams and self-weight as load case.
Does anyone have the same error?
Please help!

 

[Denial]

I do not have access to Strand7 since I ceased employment.[ ] Luckily your uploaded model is small enough to be opened using the free Demo version of the program.[ ] Your problem is very simple, even though it is initially quite hard to spot.[ ] You have an H-shaped structure, but your single "cross member" is not attached to the midpoints of the two side members.[ ] Thus the entire cross-member is floating free.

The simplest way to see this problem is to shrink all members by, say, 10%.[ ] Do this via
Entity display > Beams > Shrink

One simple way to fix it is to subdivide each of the two side members into two, then "clean" the resulting mesh.
Tools > Subdivide
Tools > Clean > Mesh
However in your real problem (rather than the hugely simplified example you wisely posted) fixing might not be so simple.

 

[IDS]

Diego - this is essentially the same issue as you had with connecting plates to beams in your previous post.

Denial - The Strand7 viewer is a free download, and will open any size file, including results. It will do pretty well everything except edit the model and run the analysis.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[DiegoAl]

Thanks for the help guys but, i tried to subdivide and then clean mesh but nothing happened.
Do you know can i connect these elements in Strand7?
I'm not get used to this program yet

 

[handofthelion]

Hi Diego,

As Denial explained, there is no connection between your central beam and the two outer beams. These members need to share a common node in order to be able provide stiffness to your central beam.

The easiest way to do this with your situation is to select all members then go to tools-->intersect beams. You model should run fine after this.

Also take care as to the orientation of your beams, they are bending about their weak axis as currently modelled. You can visualise this by by changing the beam entity display mode to section or solid.

 

[IDS]

I just subdivided the top and bottom beam into 2 and it connected the beams and automatically removed the excess nodes. It then runs the analysis with no problems. Did you try it with your simple three beam example or just on the full model?

In general it would be better to use the beam intersect function as suggested by robbievanl because the subdivision process will only work if the intersection point is exactly at the mid-point of the beams being sub-divided. Also for a more complex model you should always clean the mesh to make sure all free nodes are deleted and nodes with common coordinates are merged.

If you can get to a Strand7 training course I can recommend them. For someone starting out with the program the increase in productivity will pay back the course time and costs very quickly.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[DiegoAl]

Thanks for all the help guys!
Unfortunately, it didn't work.
I've tried everything; the Subdivide tool, Intersect Beams, Clean Mesh, and the program is still having the same error about the singularity in the stiffness matrix when i try to assign a pinned connection between the central beam and the two outer beams.
Thanks anyway for the help

 

[Denial]

DiegoAl.[ ] I'm flying completely blind here.[ ] My guess would be that you have "over released" the connection(s) between your central beam and the outer beams.[ ] In the model you posted originally, you had COMPLETELY disconnected the central beam, leaving it able to move in any of its six degrees of freedom.[ ] I'm guessing you have now implemented full translational connectivity at each end of that beam, but have fully released both ends for all three rotational degrees of freedom.[ ] This leaves that beam free to rotate about its own longitudinal (torsional) axis.[ ] If I am right you will need to remove the "torsional" release from one (and only one) of the ends.

This is a classic trap for people in their early days of learning automated frame analysis.[ ] I've fallen into it myself an embarrassingly large number of times.