Weldments Analysis

[mark_mcd]

Hi,

I have made a wire frame sketch of my chassis in Solidworks and used the Weldments tool to add the correct tubing over the members. I have come to the stage where I want to analyse the design using Cosmos.

The issue I am having is that when I start up the COSMOSXpress tool within Solidworks all of my extruded tubes dissapear leaving just one. I am told that my design contains multibodies and that only one is supported for design at any one time... How do I get the program to treat the entire frame 'as one'?

I am using Solidworks version 2007 if that makes any difference?

Also if anyone could give me any tips on the Weldments tool in general it would be much appreciated - have been through all the videos on youtube etc as well as the tutorials etc but am still finding trimming/joining members fustrating at times.

Many thanks in advance,
Mark

[mark_mcd]

Hi,

I have made a wire frame sketch of my chassis in Solidworks and used the Weldments tool to add the correct tubing over the members. I have come to the stage where I want to analyse the design using Cosmos.

The issue I am having is that when I start up the COSMOSXpress tool within Solidworks all of my extruded tubes dissapear leaving just one. I am told that my design contains multibodies and that only one is supported for design at any one time... How do I get the program to treat the entire frame 'as one'?

I am using Solidworks version 2007 if that makes any difference?

Also if anyone could give me any tips on the Weldments tool in general it would be much appreciated - have been through all the videos on youtube etc as well as the tutorials etc but am still finding trimming/joining members fustrating at times.

Many thanks in advance,
Mark

[rjwoods77]

Its because you have student version. Full bore Cosmos supports multibody assemblies.

[fixitmattman]

Cosmos Xpress only supports a single body.

Tools - Add ins - Check Cosmos Works

When you run the full program you can specify contact/gaps, either individually or globally.

[mark_mcd]

Thanks for the quick reply - I will look into this http://fsae.com/groupee_common/emoticons/icon_smile.gif Should I be trying to create the chassis with as few multibodies as possible or does it not matter?

I also have a question about the trimming and extruding of members if anyone has a moment - how crucial is it to get this exact? I have for example two members side by side at a very small angle - how do I know that these are 'together' and assuming they are not, how do I make them so? It is easy when the gap is larger as I can simply extend one member to the next members leading surface, but when the gap is very small (too small to see on screen), how do I tell Solidworks to assume they are welded?

Hope that makes sense http://fsae.com/groupee_common/emoticons/icon_confused.gif

Thanks again.

[billywight]

For the cosmos analysis, it is not at all important to use the trim/extend features to get the tube joints perfect (sometimes it's even better to leave them alone). Your question about the members that don't touch is not an issue either, the software has you define a "pinball" which is the area around one joint that it will look for another one (and assume they are "welded").

You want multibodies when doing a weldment analysis, but you will need a cosmos license to do this (the express version in pretty worthless). As stated earlier, Tools - Add-ins - Cosmos.

I suggest you look for a beam element turtorial or similar in the help files.

[Drew Price]

What Billy said (as usual).

If you don't have access to or can't get a COSMOSWorks license, you could always use the 'combine' feature to join all of your individual bodies into a single one to do rough comparisons with COSMOSExpress, just make sure to save your master model with the elements separate first, I have had bad luck trying to cut them back apart after they have been combined.

The beam mesh analysis in COSMOSWorks is extremely convenient for this though, and the student sponsored copies you can get for your team come with it, you just have to an extra validation during install to activate the license. For the 2008/2009 version we got the beginning of this year it installed the COSMOSWorks equipped module in a separate folder on my machine, but you can also add it to your default startup sequence in the 'Add-ins' meny, I think it's under tools. It will give you a COSMOS tab up in the tool bar when it's loaded correctly.

Best,
Drew

[mark_mcd]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by billywight:
For the cosmos analysis, it is not at all important to use the trim/extend features to get the tube joints perfect (sometimes it's even better to leave them alone). Your question about the members that don't touch is not an issue either, the software has you define a "pinball" which is the area around one joint that it will look for another one (and assume they are "welded").

You want multibodies when doing a weldment analysis, but you will need a cosmos license to do this (the express version in pretty worthless). As stated earlier, Tools - Add-ins - Cosmos.

I suggest you look for a beam element turtorial or similar in the help files. </div></BLOCKQUOTE>

So, just to clarify, I should just forget about trimming and generally tidying up the nodes of the chassis to get the best results http://fsae.com/groupee_common/emoticons/icon_confused.gif Why is it sometimes better to leave this alone - I will need to explain this to some people.

What is the point in trim/extend then - is it just a cosmetic thing i.e. something to do at the very end?

Thanks to everyone who's posted a response.

[Bazanaius]

It's useful when you're trying to make the chassis - whether you print out paper tube wraps, or send them off to get laser cut, someone needs to know where to cut.

B

[billywight]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">So, just to clarify, I should just forget about trimming and generally tidying up the nodes of the chassis to get the best results Why is it sometimes better to leave this alone - I will need to explain this to some people.

What is the point in trim/extend then - is it just a cosmetic thing i.e. something to do at the very end? </div></BLOCKQUOTE>

Trimming the ends is useful in the CAD world - for manufacturing, looks, getting proper mass representations, etc.

Not trimming is useful in the FEM world - the tubes will be represented as beam elements, preferable with the beam's axis running along the tube profiles CG. Ideally you would be creating the weldment structural members along sketch lines that are placed at the tube profiles CG (easy to do with a tube, it's at the centre, not as easy with wierd cross sections though). By not trimming the tubes for the FE model, it makes it easier for the software to find the joints (it will require a smaller "pinball").

CAD models are often very different from FE models and for good reason. They're not meant to perform the same function, though your CAD reseller may attempt to convince you otherwise...

[mark_mcd]

Thanks for clearing that up.

I have enabled the required Cosmosworks file and proceeded to create a static study of solid mesh. I chose my material and selected a fixed boundary condition at the rear of the chassis and a small force at the front, just to test the results. When I click 'run' the part fails within seconds as the program evaluates the 'processing boundary' but I cannot seem to get it to get to the end of the process without crashing. It always sticks at '23 of 66'? How long should it take realistically as perhaps I am not leaving it long enough - the computer becomes unresponsive although perhaps this is just the software using so much resources?

edit: Just tried a simulation with a simple 100mm x 100mm at 90deg of L-shaped angle bar and the software worked fine for that. Also did a cube framed structure with my custom profile 25x1.5mm round bar and although it worked fine for that too the cube failed under only 100N load - I am suspecting that the program is having issues with my custom profiles?

Sorry for all the questions but I know nobody who has done any Solid/Cosmosworks with Weldments so am very greatful for peoples time here.

[Drew Price]

Sounds like you have the full license, so in order to get up to speed with the beam mesh modelling, yo uneed to do two things:

1) Click the 'Help' tab at top on startup, ---&gt; 'Solidworks Tutorials' ---&gt; 'Special Types of Models' ---&gt; 'Weldments'

That will show you how to build up a spaceframe made from 'Structural Member' bodies, so you don't have to insert a sketch of a cross section to make your members from extrusions or swept bodies.

2) 'COSMOSWorks' tab ---&gt; 'Help' ---&gt; 'COSMOSWorks Online Tutorial' which opens a new window. Then under lessons block, click 'Static' and then do both the 'Beam Diagrams' and 'Truss Structure' tutorials.

You will pick it up from playing with these much faster than we can help you troubleshoot your error messages, especially if there is no-one there for you to ask for help.

Also, when it gets stuck during the count up to your total number of bodies in the solid bodies analysis, it is often because there is some error with the boundary conditions of how that member joins the others, make sure you don't have the end of one body floating in space, or two tubes occupying the same space, or any number of things. You could have the model not constrained in enough places, all your loads have to balance to that the structure doesn't end up with a net acceleration, remember that free body diagram stuff? You have to think it it like that.

That count tells you how far along the meshing process is, which is the process of breaking each body up into little elements.

Something you might try, I have received that error on decent sized models made up of thin bodies if your element size is set too large, a single element requires more space than some feature in your model. You can try setting it smaller to see if that fixes the problem, but it will run slower.

By the way, the beam mesh solver will solve your structure in under 5-10 seconds usually, whereas a solid body mesh can take up to 4-5 minutes to do the same calculation on my laptop.

Anyways, go do all the COSMOS tutorials, then report back. It'll probably answere all your questions.

Best,
Drew

[mark_mcd]

Thanks for the help people (and Drew for the detailed answer). Have taken on board as to what has been said and I believe I have found the problem.

In my sketch the roll hoops each have a '3 point arc' on top. I think this may be what is causing my errors? If so what is the best way to get around this - should i just draw their profile in roughly with the line tool and let the program treat them as several straight members? Basically what is the best way to draw these in?

On a side note the beam mesh seems to work fine (apart from it seems to remove my '3 point arcs'). It is the solid mesh study that causes the issues.

Thanks,
Mark

[Wes Burk]

Yes the beam mesh is definately the way to go, our computer won't even solve a solid mesh if I tried.

I've been using the beam mesh for a while in COSMOSWorks, how do you set the "pinball" size? Or is that a setting only within the static solid study?

[mark_mcd]

Pinball size is set by editing the Joint group menu. It's explained under the COSMOSWorks tutorial 'Analysis of a Frame Using Beams'.

Is there any benefit to the solid mesh analysis for analysing the chassis or should I just be using the beam mesh anyways?

What do you use to model the roll hoops Wes?

[Wes Burk]

We use SolidWorks for all our modelling, so I"m going to assume you mean what feature did I use to make the CAD model. Everything was done with one 3-D sketch, followed by the structural element feature (pretty much standard). You don't need to worry about trimming for analysis, the only reason to do that would be to see how much your frame tubing will actually weigh once it is notched.

I would suggest drawing the roll hoop sketches as separate 2-D or 3-D sketches, then linking them with 3-D sketches. One big 3-D sketch was nice because when you changed one thing you could watch how it changed all the other lines, but it is very prone to errors and when you have something you like its hard to keep everything from changing...

Our hoops are hexagonal so i just made a hexagon and dimensioned every part of it, quick and easy to change it.

[exFSAE]

And how do you know the mechanical properties in the weld pool, and in the HAZ? The dilution of the base metal with your filler, and subsequent heat treat.. is not trivial.

Sketchy business...

[mark_mcd]

Cosmos does not seem to like the fact that my rear roll hoop has been modeled as a '3 point arc'. I recall reading somewhere that the beam mesh tool is unable to analyze anything other than straight tubing? I just wanted to know how people got around this with the rules stating that the rear hoop must be made up of one continuous length of tube.

Thanks

[Mike Macie]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by mark_mcd:
Cosmos does not seem to like the fact that my rear roll hoop has been modeled as a '3 point arc'. I recall reading somewhere that the beam mesh tool is unable to analyze anything other than straight tubing? I just wanted to know how people got around this with the rules stating that the rear hoop must be made up of one continuous length of tube.

Thanks </div></BLOCKQUOTE>

The 2008 version can do a beam element analysis along curved paths. If you have an older version, I would save the file as something else and modify the 3d sketch so that all of lines are straight.