Railing Model 2

[Zwicky]

Hello everyone,

I'm a beginner in using Femap, so I would like to receive some comments and tips about how to model a railing type object. I have linked a screenshot of the model: it consists of two plates, which are linked by three pipes welded on the side of the plates. I've fixed the lower sides of the plates, extended the pipe and fixed their bounduary points. For the moment the load case is very simple, just nodal force on the top pipe in the y direction. The plates are modeled through 2D plate-element type, whilst the pipes are modeled with 1D beam-element type. I get several fatal errors (tried param,bailout,-1 and frequency analysis) 4698, 4192, 4690, 307, 9002: due to my poor experience I'm not succeeding in finding the error, I'm just trying different solutions. I guess the error may be in the connection between beam element and plate element (I used as connecting region the curve of the pipe and element on the plate), on the fact that the plate is divided into two surfaces (i'm not sure because the mesh seems to be good around the contact area), or else can be that the plate elements nodes, from what I understood, need to have a rotation DOF especially fixed. For whoever will help me thank you in advance and sorry for any stupid question! Kind Regards.

Simone

http://s13.postimage.org/v7zht5vyv/Railing.png

http://postimage.org/image/ns087d89f/

 

[BlasMolero]

Dear Simone,
Post your FEMAP model here, if not it will be difficult to know what is wrong in your model, OK?.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Zwicky]

Ok, thanks for the tip ( and for the tutorial on your website ).

[URL unfurl="true"]http://speedy.sh/pTkCc/RAIL.MOD[/URL]

http://speedy.sh/pTkCc/RAIL.MOD

<a href="

http://speedy.sh/pTkCc/RAIL.MOD">Download

at SpeedyShare</a>

 

[BlasMolero]

Dear Simone,
Your model is a little disaster, let's see:
1.- Forgot at all the connections defined, delete all, you can not connect a 1-D Beam element with a 2-D Shell element using surface-to-surface glue contact, GLUE contacts are for Shell-to-Shell, or Shell-to-Solid. To effectlively joint Beam-to-Shell, use RBE2 rigid "spider-like" elements.
2.- Also, I do not see any BEAM element in your model, the property is defined but the mesh missing.
3.- The 2-D Plate mesh is very distorted, use "GEOMETRY > SOLID > STITCH" to get rid of internal splits & slivers of plates, and then the mesh will be perfect.

Solid Stitch
2 Surface(s) Selected...
Surfaces successfully stitched.
New solid conforms to Parasolid modeling tolerances.
Created 1 connected region.
Created Sheet Solid 4.
Solid 4 passes Body Checking

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Zwicky]

Dear Blas,

thank you very much. Now I'll follow your advices, beginning to create beam element (i know it's day 1 lesson 1) but can't succeed, i give the section properties and the orientation (and of course beam element type) and the script says in red ''element #12345 orientation is colinear with element x-axis'', i don't even know if it is good or bad sign, but i can't see elements along the curve, so i guess something is going wrong. The stitch command was useful and thank you again, the mesh is better now. For what concerns the connections, can you explain better? I think i need to define the node on the intersect between surface and the curve as rigid element, or the element on the plate must be changed into RBE2 and then connected to nearest beams element or to the curve connection region? Thank you again in advance.

Best Regards,
Simone.

 

[BlasMolero]

Dear Simone,
You need to learn how to orient beam elements, FEMAP ask you to orient the Y-local section of the beam cross section, do not select the COLIENAR axis (is, the GLOBAL X-axis), you will success if select any of the others global axis, take a look to my videos to learn more:

http://iberisa.wordpress.com/2011/04/18/offset-en-elementos-cbarcbeam/

1.- Caution with units, ckeck your model is consistent, units of ALUMINUN are wrong.
2.- Split the surface by the point intersectiing with the curve, simple merge nodes of Plate & Shell there.
3.- Use RBE2 elements to joint the beam with the plate.
4.- Split beam lines in the intersection with the plate surfaces, this way you will have a beam node for sure, use command "Modify > Break".
5.- Also break the curve line in the midle, where the load is applied, and prescribe loads in the point, in geometry, not in the mesh.
6.- The same for cosntraints, delete NODAL constrains, and prescribe constrains in the geometry, in the end points of curve lines.

And that's all!. The following picture will give you a better idea of what you need to do:

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Zwicky]

Dear Blas,

thank you so much, I didn't understand clearly point number 2, but now i'm getting familiar with rigid elements and understanding how connection works. I'll investigate on the advice of giving loads and boundaries on the geometry more than on the mesh, but i appreciate your will to share your knowledge in such a generous way.

Best regards,
Simone.

 

[Naffoussi]

Dear Blas,

we can use glued contact for shell-solid connection??? even if the mesh is not similar between parts??

 

[BlasMolero]

Oh yes!. You must define EDGE-TO-SURFACE GLUE contact regions, this is a great method to joint dissimilar meshes.

The source region for edge-to-surface glue consists of shell element free edges (BLSEG). The target region consists of shell or solid element faces. A simplistic description of edge-to-surface glue is that the software creates pseudo-faces along the edges in the source region. It then connects these pseudo-faces to the shell or solid faces in the target region with weld like connections (the software always uses the GLUETYPE=2 option on the BGPARM bulk entry).

The BLSEG entry is defined by its own unique ID and consists of one or more line segments defined between consecutive grid points. You must enter the grid points that define the edge region in a continuous topological order on the BLSEG entry. If an edge region or curve forms a closed loop, for example, the grid points around the perimeter of a cylinder edge, the last grid point identification number should be the same as the first grid point number. The grid point IDs on the BLSEG entry used to define a glue edge region can only be part of the CQUAD4, CQUADR, CQUAD8, CTRIA3, CTRIAR and CTRIA6 element connectivity. Instead to enter nodes, the better method in FEMAP is to select CURVES, and FEMAP will care of nodes when exporting the model to NX NASTRAN.

Edge-to-surface glue definitions are supported in all solution sequences except solutions 144 -146, 153, 159, 601 and 701. They cannot be used to represent acoustic glue connections.

Best regards,
Blas.


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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Naffoussi]

Thank you Blas, i didn't know that it was possible.