Grid point singularities

[sushi75]

Hi everyone,

I am facing a problem with my model; it's a pretty simple one but generates singularities. So I hope somenone can clarifiy why this is happening!

Basically I have several curves making a closed boundary (defining a L shape surface). I have created internal curves with approach on curve to define the number of elements in order to locally refine the mesh.
From that I have created several boundary surfaces, then meshed.

I revolved these QUAD to create solid elements, applied constraints and load.

Nastran doesn't crash, but I end up with grid point singularities, giving no results.

I guess the problem comes from the presence of several boundaries surfaces, but I cannot really understand why theses singularities occur.

Hope someone can find out why, I'm very curious to understand what is happening!

Thanks for your help

tom

 

[BlasMolero]

Dear Tom,
Post your FEMAP model here to take a look to it.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[sushi75]

Hi Blas,

Thanks for your quick reply. I will post the model asap, but is's just a simple L shape. What I don't understand is that if I create the boundary surface from curves without qny meshing attribute on them, then mesh the surface, and revolve the quad to create solid elements; it works.

If I select meshing attributes on each curve to choose the number of elements, then create the boundary surface and mesh the surface, then revolve the elements as done before, the analysis ends up with all grid point singularities.

It's a bit of a mystery, it's like the created nodes have no stiffness.

Formy understanding, usually, what's behind grid point singularities? Is this something to do with constraints?

Thanks a lot!

 

[BlasMolero]

Dear Tom,
You have a mechanims (a rigid body movement), then your stiffness matrix is singular, surely any unmerged node. The trick is simply: run a normal modes / Eigenvalue analysis using NX NASTRAN (SOL103) and animate your modes, you will see the error inmediately.

https://iberisa.wordpress.com/2011/...run-terminated-due-to-excessive-pivot-ratios/

Best regards,
Blas.,

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[sushi75]

Thanks for your support on that query.

I've checked the coincident nodes so I assume this is not the cause of the problem, but I will follow your advice and run 103 solution.

So you agree that having a boundary surface made of curves with meshing attribute on each one is not a problem?

A bit a mystery but I il investigate until I understand !!

 

[rb1957]

"I revolved these QUAD to create solid elements" ... ?

are you sure your constraints are adequate ?

another day in paradise, or is paradise one day closer ?

 

[sushi75]

Hello,

I'm still struggling to understand the issue with these solid elements generating grid point singularities. For clarity I have attached a screenshot of the model.

I have been told that Nastran does not constrain 456 on solid even if AUTOSPC is set to YES.
So I guess the idea is to manually constrain 456 on each node, but it's a bit painful for large models.

It makes sense as the f06 lists the grid point singularities on 456 only.

Still, it's not very clear why revolving quad into solid creates so many problems!!

 

[rb1957]

solid elements have no rotational freedoms. NASTRAN assumes by default that each node has 6 dof. Forget about doing anything with the rotational freedoms; you could constrain all nodes in 4,5,6 and nothing should happen.

what global constraints have you applied ? enough to take out rigid body motion ?

another day in paradise, or is paradise one day closer ?

 

[sushi75]

Hello,

Thanks for all your replies. You are right, the problem is the 456 dof that should be constained. However, the model is large, and I don't know how to efficiently constraint each internal node. I start from a 2D problem, and then revolve the quad elements to create the solid ones. So the number of nodes to constraint is massive!!

Can't find a way out!!

help !!

thanks!

 

[rb1957]

param,autospc,on ... we do solid models quite often without NASTRAN complaining.

if your model is all 3D elements, then constrain all nodes (nodal constraint, select all, ...). To be careful, check the constraint reactions (should be zero or 10^-15)

if your model is 2D and 3D elements, make groups of the different types (select the elements, then add the nodes on the elements (in the group) then in the 3D group remove nodes associated with the 2D element group; then constrain all nodes in the 3D element group. this way nodes in the 2D elements will be unconstrained.

but i'm surprised you have to. it could be that your model is a mechanism (as far as the FEA cares)

another day in paradise, or is paradise one day closer ?

 

[sushi75]

Hi,

Thanks rb1957 for your answer. This is actally what I don't fully understand, the autospc is turned on, and despite that I have to go through the process of manually constrain those nodes.

I'll follow your advice by creating a group of nodes on solids, then exclude the one connected to the shell so that I can only have the internal ones, which I can then apply a 456 constrain on.

I'll give it a try!

Cheers,

T

 

[rb1957]

what FEA are you running, inside FeMap ?

it sounds very odd ... these rotational freedoms are zero energy freedoms (which is why autospc should work). we run many 3D models without constraining the rotational freedoms deliberately. what constraints have you applied to you model ? 3-2-1 translational constraints ??

another day in paradise, or is paradise one day closer ?

 

[BlasMolero]

Dear Tom,
Post your FEMAP model here, after revising it should be easy to explain the source problem you are having.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[vectorKZ]

Assuming you are running static linear analysis, here would be my approach:

FIRST:
Hand calculate a global freebody or use an FEM "stickmodel" to completely define your input loads and system constraints. Export both the reactions and loads as INPUT loads to your actual FEM.

SECOND:
Define a generic system constraint at a far-field stress location in your FEM.
SPC #1 = 123 place at origin of local system
SPC #2 = 23 place along 1-direction axis
SPC #3 = 3 place along 2-direction axis

be sure nodal analysis system for each of your constrained nodes is the generic constraint local sys.

This way, you KNOW you are feeding your FEM balanced loads and don't have to dive into error and energy jargon.
Any "load" that piles up in your system constraints point to errors, inertia relief, etc.

 

[ThomasH]

Hi

A simple way of testing is to turn of AUTOSPC and run an Eigen modes analysis. It here are any rigid body modes they should be clearly visible.

Thomas

 

[sushi75]

Thanks for all your replies. I could sort it out by creating a group containing the internal nodes and then constraint the rotaional dofs.
But it still mysterious why AUTOSPC doesn't do the job...!!

I'm using MD Nastran, perhaps it could be the cause?
Any idea is more that welcome )