Best method to join/weld parallel midplane extracted shell elements? 4

[ExDrill]

My situation is:
I am using solidworks to generate designs for manufacture and exporting these designs into Ansys Workbench 12. The designs are weldments made up of common structural grade steel profile and plate. I can successfully extract the midplanes of all profiles in Design Modeller and I can successfully "surface extend" and model the joins of the shells that intersect one another (where obviously a weld would exist in the reality).

My Problem is:
All Ive described above is very efficient and to my liking. I hit a brick wall however when I need to join parallel midplanes (where a weld would exist in reality, eg around the edges). When you extract the midplane of two plates sitting on each other (Like a special Girder)they are offset from each other and therefore they have a gap. This gap causes me no end of drama. I just need to know if anyone can point me in a clear direction. The join in reality for example sake is a continuous fillet weld around a plate that is attached to a Rectangular Hollow Section (RHS) to increase its capacity locally (See Attached pdf).

Ive read about spot weld connections in Ansys Workbench that tie the shells across the gap with a beam element but how they are setup efficiently from solidworks is a mystery to me. It appears Unigraphics is the best for this but...
I can't give up solidworks.
I can however move to another FEA package if necessary.

Thankyou for your responses. I will not explain my method of connecting these now as I know its incorrect.

 

[spongebob007]

Using 2D elements is a valid way to make the connection. You can use beams, rigid elements (bars), or spring elements with a high stiffness.

These connections will transfer the load from one plate to the next, but if stresses in the weld area are your concern, there is probably no good way around 3D modeling.

As far as software specific advice, can't help there unless you are using NX.

 

[ExDrill]

Thanks Spongebob, The weld stress is not my concern, does the NX user face have convenient, user friendly tools for midsurfacing, extending and adding 2D elements? There are hints Ansys Workbench may have but they are illuding me. I just dont want to go backwards from the GUI of ansys which is easy and fast (could be faster and more back modifyable but...).

 

[BlasMolero]

Dear ExDrill,
You have a few methods available: the more simple is to define midsurfaces and mesh with Shell elements and use RBE2 rigid elements (constraining the 6 DOF) to joint mesh of both plates simulating the weld joint. The advantage of this method is that Shell elements (well, CQUAD4 elements, I run NX NASTRAN & FEMAP) give you plenty of information of internal forces & moments, then you can dimension the throat size of the fillet weld. FEMAP is able to extend & trim automatically midsurfaces in order to mesh with Shell elements and define RBE2 elements between nodes of both plates.

Another approach available with NX NASTRAN are CWELD elements, ie, spot welds, but this is valid only if you have point-to-point welded joints, not a linear weld.

Another approach is to create a 2D plane strain FEA model considering both membrane & bending loading. But this is a very localized study, not valid for full structure.

Best regards,
Blas.

 

[seymours2571]

ExDrill,

If you are not interested in the stress in the weld itself you can bond the edge of your shelled tubing to the surface of the plate by creating manual connections in Ansys12 WB.

However, note that if the distance between the edge of the tube and the surface of the mating plate is large the solver may not be able to automatically create the bond. Therefore, you will need to change the "Pinball Region" setting from Program Controlled to "Radius". Then type in the radius of a sphere that will encapsulate both the welded edge of the square tubing and the mid surface of the corresponding plate. A blue sphere should appear in the graphics window to help with this.

I just modeled your example provided using the methods described and it worked fine.

Hope this helps,

Steve

 

[ExDrill]

Thanks for some good feedback guys, Cheers Steve I didnt even try that to see if it works.

 

[Onda]

If you are modelling a large structure and you are not interested in the stress in the weld itself you can model only one shell with the thickness of the sum of the two shell. Just pay attention of position of neutral axis.

I'm not sure you can do this in WB because you should assign different property (thickness) to the row of elements. But this is the way I would go to model this part in Patran/Nastran.

Onda

 

[spongebob007]

NX is the best preprocessor I have ever worked with. I am surprised at some of the complex geometries that NX is able to midsurface correctly. If NX can't do it correctly, there are tools available that allow you to repair surface entities. You can trim, extend,sew, and split surfaces to fit your needs. Manual creation of elements in NX is also a breeze. The smart selection tools of NX can be a time saver. When selecting, you can filter by what type of entity you want (point, line, element, volume, etc). You can also filter to an even greater level of detail for certain entities. For instance, I was modeling two thin shells that were bolted together. I used beam elements to model the connection at the centers of the holes. I set the selection filter so that the only types of selectable entities were centerpoints. You don't even need to have created a point, just pick any circular arc and NX snaps to the implied center point. This saves time when you have to do this operation over and over, you don't waste time selecting and desleecting the wrong entity types and you minimize the zooming and panning typically required to get to the entity you actually want.

Another great thing about NX is history free modeling. The problem with most FEA is that if you don't create the geometry in an FEA preprocessor all you have is a dumb solid. With NX I can import STEP files from PRO/E and make some impressive modifications to the geometry without any model history.

 

[EngAddict]

You can create midplane offset in SolidWorks, surfacing features are better too.

If you were using solidworks simulation you can easily create bonded contacts between non-touching surfaces. Also when using SWx Sim, weldments are automatically converted to beam elements. You can then create bonded contacts between nodes and plates or in your case between a member and a plate.

However if you have ansys 12 I wouldn't give it up for SWx Sim.

I actually have job in at the moment, same weld configuration but they need the stress in the welds so it is a sold weld to a shell member.

 

[mlamping]

The connection type I see most often in welded structures is to use shells. That is to represent the weld as shell elements so that the top and bottom plates are represented with shells and connected by shells. In addition to midsurfacing in your CAD modeler, you could generate these "weld" faces by extruding participating edges on the source plate to adjacent target faces. Then stitch the "weld" faces to the source and target faces and mesh. You get shell-shell connections and you can represent the weld with an appropriate material and shell thickness. Usually the weld mesh is just a single row of elements perpendicular to both plates.

I use/support NX and have also seen models that take advantage of NX Weld Assistant. It creates solid geometry for welds and it can be leveraged to represent welds in various ways using solids, shells, and 1D elements.

 

[ExDrill]

MLamping, Thankyou for your reply, this is what I have been doing up until now. Creating perpendicular shell elements at, where I believe, the welding is physically possible (this approach is the most efficient and I can control all aspects easily as it is very clear visually). You say you've seen this before. Do you know the thickness that is prescribed the "weld" shell elements and whether it relates to maximum thickness (space between) of the shell elements its joining?

I have been noticing very high stresses and am unable to accept the stress values in these "weld" shell elements (and therefore the entire structure), I believe that due to their inconsistancy with the actual physical geometry e.g. the width of them being from one midsurface to another in comparison to actual weld that is between the plates on the their outer surface is introducing secondary large bending stresses on top of the shear reaching 10 times yeild in some cases making the models rubbish.

The last thing I want to do is to increase the thickness of these welds to a value that will render the results unconservative.

Something just dawned on me that I should test whether the results are unconservative using a series of simple models.

Your experienced comments would be most welcome.

 

[mlamping]

Sorry for the delayed response here. I haven't gotten used to periodically checking the list. A typical thickness for weld elements is to use the average thickness of the plates that the weld joins. It's an attempt to create a somewhat contiguous representation in the joint. Another option is to specify a fixed thickness for weld elements regardless of the plates being connected.