calculate the stresses in a complete trailer 1

[matrix027]

Hello ,

I use solidworks 2003 to design the trailer.
The complete trailer , has a chassis and a box (mounted on the chassis)
We want to find the weak places in the trailer.
Is it possible to calculate the stresse on a complete trailer model (in solids)?
Do i convert the trailer into surfaces before calculating.
Is this possible with cosmosworks2003 or do i need an other FEA-package ?

 

[tstanley]

I used to be in the trailer business and have also done some FEA. I don't believe it is as simple as you are expecting, particularly if you include the suspension. As well you have to give careful consideration of any joints. You don't say what kind of trailer, but anything with sheet metal would not be modeled very well with solid elements. Even a lowbed would probably be better with plate elements.

Tom Stanley

 

[matrix027]

thanks for your reply

The trailer that we want to calculate, is a trailer with a moving floor ( not a tipping trailer)
At the moment designed in solidworks 2003 (solids)
But they say that the calculatetime will be faster if the trailer is modeled in surfaces.

are u agree ?

 

[corus]

If you use a single solid element through the thickness then you would have 8 nodes with 3 degrees of freedom each. For a plate/shell with 4 nodes there are 6 degrees of freedom to each node, ie. there would be little or no difference in solution time in using a solid element to a shell element. It may be quicker to generate the model in solid form if you're reading in a 3D solid drawing and then mesh with a solid element, rather than trying to find the mid-surfaces and meshing with shells.

corus

 

[analyzer]

If your trailer is simple, without curved beams, transitions, drops, etc; you might consider using beam elements.

 

[Softedge]

I have been looking at doing a similar analysis for a trailer. I think that using plate elements would give the desired results. A 3D analysis using bricks would be far too costly from a standpoint of time. Using beam elements would be fine for the sizing of the frame and lateral members, however, problems usually occur at points on the frame where an analysis using a mesh is required. If you are using C or W sections for the frame rails, problems can show up at the flange tips that you will want to know about and design for. I use Solidworks 2004 and Algor FEA software that will automatically create plate elements from my solid model.

 

[miketo]

I want to use cosmosworks2003
Does anyone have experience with this software?
Softedge , you say that algor automatically create plate beams from a solid model.
The chassis has a I-form and the lateral members also.
When i try to mesh the chassis in cosmosworks i have to split the surfaces.
Does algor creates a good mesh without split the contactsurfaces?
If you start from a solid model ,does algor automatically extend the surfaces together? (for example the midsurfaces of a I-form solid).

 

[jeeleong]

Hi!

I hope you will allow me to share something with you. I think I agree with tstanley that to model the complete trailer will not be a simple task. I have not used CosmosWorks2003 but I have some experience in using CosmosWorks6 with Solid Works and I personally feel that it is good for undertaking simple single part analysis. However, it may not be desirable for analysing your complete trailer unless it is a really simple trailer. I am using Nastran for Assembly and more complicated Parts.

It is difficult to give an exact answer to your question. The answer is not simply knowing if your FEA software can auto-mesh a solid model with either solid or shell elements and give you fancy colourful results but understanding the problem itself and then devising a strategy to obtained the desired results with the right tool. You might start with identifying the type of analysis that you would like to undertake to show you the weak points. Will you be looking at Static, Dynamic or Buckling Failures? Perhaps the FEA software will be able to auto-mesh your trailer with solid or shell or plate elements but it might take forever to solve the problem especially in dynamic or buckling analysis. Sometimes, you will not be able to auto-mesh your solid model because of some very fine details in your design. It maybe more appropriate to reduce and idealise your trailer with a mixture of solid (for solid components or fittings), shell/plates (for thin sheet metals) and beam elements (for beams and stiffeners), which would give the correct structural response for the type of analysis that you undertake, and the model can be solved within an acceptable time frame. Solid and Shell/Plate elements will give you for example the Von-Mises stress to calculate your margin of safety. Axial and bending or combined axial-bending stresses can be extracted from beam elements to verify the strength of your beams and stiffeners. If you like to see the actual stress distribution in the components that you modelled with the beam elements, you can always extract the internal loads and then apply them as loads to the actual detail component in a separate analysis. Additionally, you may not want to use the auto-mesh capability because you may want to omit the very fine detail designs in your solid model, which are non-critical structures to reduce the size of your finite element model.

If the above is applicable to you and you have addressed them, all you need to do is to find the software that can help you to do the job. I hope this helps.

 

[feadude]

I agree with jeeleong however if you mix solid elements with shell and beam elements you might get singularities at the juncture of shell or beam elements and solid elements since solid elements do not have rotational degrees of freedom whereas shell or beam elements can rotate.
I hope this helps.

 

[jeeleong]

feadude, you are right. I forgot to mention that. However, some software will allow you to use constraint equations to ensure compatibility between elements of different number of nodal degrees of freedom and shape function. There are also some other techniques to embed the shell of beam elements to the solid elements to remove the singularity. I have to caution that all these have to be used with CARE and will very much depends on the judgement of the analyst on their appropriateness. Many thanks.

 

[feadude]

jeeleong, Can you elaborate on this please?
"There are also some other techniques to embed the shell of beam elements to the solid elements to remove the singularity."
Thank you

 

[jeeleong]

First of all, Happy New Year Everyone!

Take for example when we try to connect a node of a 2D Beam element (3DOF) to a node of a 2D plane element (2DOF). If a transverse force is applied to the other node of the 2D Beam element, only force is transmitted at the connection. Moment will not be transferred because the 2D plane element only uses the translational DOF. Hence, there will be mechanism and the stiffness matrix would be singular. To enable both force and moment to be transferred, we can extend the 2D beam element ‘into’ the 2D plane element body by adding another 2D beam element. However, I don’t normally use this method because we can quite easily apply a constraint equation with some of the softwares. This way, I will not have to worry too much about the properties for the additional beam element.

I am sorry if the above is a little fuzzy. It is better if I can illustrate with some figures. Do look into section 3.9 of “Finite Element Modelling for Stress Analysis” by R.D Cook for a better clarification.

I hope this helps.