Explicit analysis

[mrmartins]

Hi, I am working in the analysis of a large structure made with beams welded toghether. At this time I am still modeling but I do not know whats the best:
- model the structure as an assembly of beams
- or model the structure as only a part

Anyone can help me?...

 

[Drej]

I would say almost 99% that you should use beam elements to model this, although you need to consider some of the factors below. It all depends on the results you need, the nature of the structure (how big it is, how the cross section of the beams look, etc. etc.) and the type of analysis you need to carry out (static, transient, thermal, contact, coupled, etc. - none of which you've described). Also, I'm not sure what you mean by "part", do you mean as a solid? Is the subject of your post applicable here as well? When you say "explicit" do you mean explicit integration or explicit in the sense that you need to explicitly know? Modelling in an explicit code brings its own problems.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[mrmartins]

Thanks for your post. I will be more precise. The structure is made of square beams, 60x30x3, althougth there are diferent sections and thickness around this value. The structure is quite large, I would say a hundred of bars. The purpose is to study the impact of such a structure (explicit analysis) using LSDYNA. My question was if I build the stucture as an assembly of parts (in solidworks for example) or I built it as a single part. I t is supposed that all beams are welded together. Because later in Ansys I need to GLUE all the parts... and this can be time consuming. I do not know. What is the best aproach to build the model for posterior integration in ansys and having all the beams welded.

 

[corus]

As your beams can be of different thickness it's simpler to have them as seperate parts so that stress averaging doesn't occur at intesrsections. If all the degrees of freedom are coupled at the intersections then the result for displacements will be the same as if the structure was one complete part. If the structure was one complete part, though, you can always remove the stress averaging facility, it's all a matter of which way is quickest to build the complete structure.

corus

 

[Drej]

My preference for this job would be as follows. Firstly (I'm assuming you may already know this) but you will have to represent the structure as an assemblage of lines in your CAD model, in order that you can mesh these with beam elements. In this sense, it may be easier to just model the whole thing in ANSYS/Pre (very easy to learn this if you don't know already). You could then build your model "bottom up" using techno-speak, which would save you the time/effort in Solidworks and give you more control over your model. You should model the structure as a series of connecting lines which, when meshed, would behave as if each connection (between beams) were welded. The easiest/quickest way to then assign correct "beam" attributes to each line would be to use the LATT command, then you can assign an appropriate element size for the whole model using ESIZE (or LESIZE) and mesh the whole dang thing in one go using LMESH,ALL. Job done.

Hope this helps.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[mrmartins]

Thanks a lot for your posts, they help a lot. But imagine that I have already the structure done in solidworks as an assembly of all bars. What should I do to analyse it in ansys..

Thanks again

 

[Drej]

It depends how you've modelled it in Solidworks. If you have just a series of lines representing the centre of the beams then you can import this into ANSYS no problem (as an IGES say). But if you've explicitly modelled the cross sections (i.e. as a 3D solid object) in Solidworks then you have problems, which is why I suggested you start in ANSYS. Two things to look into if this is the case. There are some CAD software packages that allow you to extract the mid-line or surface of the geometry. This is what you need. On the other hand, if you import your geometry into ANSYS, the CAD software may have already put the centre-lines in the geometry for you. Have a look.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[crisb]

It sounds like mrmartins doesnt want to model this as beam elements, but wants to use 3D elements applied to the solidworks model. This will result in a much bigger model but may be much more accurate for an impact analysis. There may also be connection details and/or offsets etc that are difficult to accurately represent as beams.

It sounds like the members are hollow section members. Using shell elements for the walls might be another option that will be quicker to run.

If possible I would try to mesh the whole assembly first rather than meshing individual parts, otherwise one has to be very careful to get the mesh to align at all the intersections.

From the desciption be prepared for a large model that is slow to mesh and run!