Strand7 help - Global Stiffness Matrix Singular error

[Gavla]

Hello,
I have read a number of posts regarding this error, noe of which have helped me to ge this to run. Mine is a simply supported beam in three point bending, though the cross section conssits of three SHS stacked with plates top and bottom (a double web i-beam of sorts). Is anybody able to take a look and give me some advice as to how i can get it running?

Thanks
Gavin

 

[IDS]

From a quick look:

1. Your beam elements have no properties.
2. Your plate elements are much too big and are not connected to each other or to the beams. For plate elements to connect they must share nodes along the contact edge.

I'm not sure why you are using beam elements in this model. I suggest deleting the beams and subdividing the plates. Then use Global Clean followed by Detect-Plate edges, to make sure they are connected where they should be.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Hi Doug,

Thank you so much for getting back so quickly. Clearly I do not really know what I am doing.
I agree that I had intended for the model to consist of plates only, so will attempt this and let you know how I get on.

 

[IDS]

It's worth looking through their web-notes if you have access. They have sample models and details of how to create the model and display results.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Thanks Doug,

I have deleted the beams and subdivided the plate and now all works ok. I am a mature student so using the eductaional license,so limited access to Webnotes unfortunately.

Regards
Gavin

 

[centondollar]

A singular stiffness matrix in a static problem tends to indicate that rigid body motion is not suitably suppressed: the system of linear equations does not have a unique solution. This may occur due to there existing no geometric boundary conditions for primary variables, or it may occur due to too few geometric boundary conditions (e.g., only zero deflection at clamped edge of a cantilevered plate).

 

[Gavla]

Hello again,

I will try and follow on from my earlier post rather than start a new one.

I have a flexural member built from plate elements in Strand7. I applied load to the top of the member, split 50/50 over the webs (it is a closed member). However, the point loads are buckling the top in an unrealtic way, so want to change the point loads to line loads of a specific width (say 50mm). I cannot find any advice anywhere on how to take measurements in the model. For example if i delete the point loads, how can i tell where the midpoint is, or quarter or third point is without measuring? If I want to change the point load to a line load of a specific width, how can i measure between nodes to know what the node grid is, especially for plates that have been subdivided several times? I can delete the point loads and replace with line loads over 4-5 nodes, but would like to place a line load over a specific width, or close enough anyway.

Thanks

Gavin

 

[IDS]

There are lots of options for getting information about the model, but the main ones are:

Hold down the shift key and point at an element or node, it will display information such as coordinates, side length, etc.
To get info about only a particular element type, or only nodes, select from the icons immediately above the main window.
To measure distances or angles and get a copyable list of element properties, open the whiteboard: View-Show/hide-Whiteboard or Ctrl-Alt-W
To get a listing of node coordinates, or element details, select the nodes or elements you are interested in, go to the TEXT tab, and select view selected nodes only. You can copy the displayed data and paste to a spreadsheet, and do whatever calcs you want there.

But are you doing a non-linear analysis? I'd suggest doing linear until you get it working properly.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Thank you Doug. Very helpful!

 

[Gavla]

Hi once again,

Can you please confirm how one might be able to identify the direction of the local axis? For example, I need to model orthotropic properties, which have maximum material properties in the long direction (pultruded direction). So max properties should be along the member, with minor properties in the transverse direction. However, orthotropic properties are labelled E1,E2,E3 etc under plate and brick property and it is not clear which way this is orenting the properties with respect to the X,Y, and Z axis. This is giving me spurious results.

I have attached a model that uses bricks (maybe not better than plates, but was sort of an accident when extruding a 2D plate rather than beam elements), and it would be very nice to be able to know if the material props are in the correct direction.

As a side a note, are you able to please shed some light on the warning message when solving.

Thanks you!

Gavin

 

[Gavla]

Hello again, I ave now resolved the axis issue so please disregqrd. However, if you have any coments on the model and solver warning, that would be appreciated.

Regards

Gavin

 

[IDS]

I'm a bit busy this evening, but I'll have a look next year

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Thanks Doug,

Please review the attached model. I have tightened the mesh and the deflected shape is a bit crazy. Looked more reasonable with a larger mesh. Now it looks very 'spikey' for lack of a better term. I had hoped for a smoother curve.

Also still getting the same warnings.

I really appreciate your help.

Regards (and happy new year!)

Gavin

 

[Gavla]

Hello again,

I think the issues in the last model started when i tried to subdivide the mesh. I have noticed that this has pretty much ruined the mesh. I am struggling with how to subdivide in a controlled manner, especially when the A & B axis for subdividion are oriented differently from one brick to the next. Also bricks have three axis of subdivision which makes it even harder to subdivide consistently. I think this has caused the most issues. Is there a way to globally align the subdivision axis with the x,y,z axis, so that i can select all of the bricks in the flanges say and subdiivde each brick the same way? This will save me a lot of headaches. Is there a way to highlighte whole model and execute a global uniform subdivision task?

Probably easier if I just post my model with the 25mm mesh before i ruined it with subdivision. I am trying really to improve the accuracy, as would expect worst case mid span deflection to be ~6mm.

Thanks

Gavin

 

[Gavla]

Not sure i model attached last time. Sorry for spamming the thread with multiple posts!

 

[IDS]

There may be other issues, but the obvious one is that the bricks are not properly connected because edges are not aligned. If you want two bricks continuous across a face then that face must have the same nodes in both bricks. For instance, if you want the top and bottom flanges of the central box to have three layers, then the webs need to be divided into 3 layers of the same depth at the top and bottom.

I suggest creating a cross section with plate elements, making sure all the plates are properly connected, then extrude the plates into bricks, starting with the end diaphragm thickness, then longer bricks up to the next diaphragm. You can then copy all the bricks for as many sections as you need.

Remember to delete all the plates when you have finished extruding. I also note that your model has some rigid links which may be causing problems.

To display the axes, right click on the brick icon in the left margin and select the Draw Axis boxes, but note that when you select an element to be subdivided the A,B,C directions are displayed.

For the support conditions, remember that nodes should be free to move in the horizontal plane, except for one fully fixed node, and sufficient restraints to prevent rotation about the vertical axis.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Thanks Doug,

Yes I had come to that conclusion about the brick mesh also. I still do not understand though why if you subdivide a brick surface, the A,B&C directions can vary sometimes. It makes it very difficult if you need to subdivide an exsiting model. However, it is probably just easier to rebuild it from scratch.

With your last comments, are you saying that only one arbitrary node at each end (along the bottom where current restraints are shown) needs to be fixed?

I think i have sufficient grasp of this now to complete the modelling. Is there any benefit to using bricks over plates?

Is there a way I can run the model so that it incrementely increases the middle point load and generates say a load deflection graph of the results?

Thank you!

Gavin

 

[IDS]

HI Gavin,

Restraints: The main point is that there need to be sufficient restraints to prevent global translation and rotation, but one end of the beam must be free to move in the longitudinal direction, so you don't get loads transferred through arching action. For a bridge beam with X longitudinal and Y vertical it makes sense to restrain all the nodes at bearing locations in the Y direction, then at one end restrain X and Z at the base node on the CL and at the other end just the Z direction at the CL node.

Benefit of bricks: In general, I can't see any real benefit in using bricks, in fact I would normally go for beams (or beams + plates for the top slab) rather than plates! Bricks may have advantages with complex geometry, say if you want to do a detailed model of beams + bearings + headstock.

Incremental analyses: Yes, use the Non-linear Static Solver. Set the non-linear conditions to what you want (so you can do a linear analysis with the non-linear solver, if you want to). Then go to the Loads tab, and you can create as many load increments as you want. You can factor loads, or you can create a loadcase with unit applied deflections at the load points, and factor the deflections. You can also do a staged analysis, so you can start with separate precast beams, then add a top slab, then apply loads to that, for instance. It's quite a bit more complicated, but for some applications it's important to model the load stages properly.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Gavla]

Thank you once again Doug.

I have re-built this model again from scratch. I am pretty certain all blocks connected, have adopted correct restraints, no links included etc, and still getting a material warning and strange results. I am lost as to how to fix it. I am now trying to build this particular profile from plates to see if it is easier.

I have attached the updated model if you had time to have a quick look to see what I am missing.

I really appreciate your help

Gavin

 

[Gavla]

Hi once again Doug,

I think i have sorted this now by moving away from bricks to a plate mesh. Thank you so much for your help.

Regards

Gavin