Using ANSYS+Solidworks for FEA of torsional stiffness

[Grant Mahler]

OK,

I have read through most of the FEA threads.

I dont want to use GRAPE, I want to use ANSYS.

I have the model of the car in Solidworks, I just want to get the points of intersection out of Solidworks and into ANSYS. Is there a way to either import a wireframe from Solidworks? Or, is there a way to get all intersection points from Solidworks (or a way to plug them into ANSYS via a file instead of typing in a bunch of points?)

Thanks!

[Coombesy]

You can export the model as an .iges from solidworks and import to anysys with that. If you have some of the extras from ansys you can import straight from solid works.

In ansys classic id just shell mesh it, rather than beams or truss elements.

I prefer ansys workbench for this, import the model to the geometry section, use the mid plane extraction for all the piepes, and then mesh away, much easyer to use and apply loads compared to ansys.

Coombesy

USQ Motorsport

[Grant Mahler]

Hrm....I tried importing the frame as an IGES file and ANSYS just sits there and hums....I let it run for 1/2 hour and nothing ever happened so I'm not sure if it was hung or whether I should've let it run longer.

We have the cheapest ANSYS license possible, the school didn't want to get any of the important features that might let ANSYS be useful.

[billywight]

Not farmiliar with Ansys, but a beam model is definately the way to go. Shell mesh would have a lot more elements and take much longer to solve for no real advantage in results. If you have 07 cosmos, there is a beam element feature that uses the structural member properties to create the beam elements. It's all integrated in SW and assosiative so it makes design iterations much easier. Look under the tools, add-ins menu and try to check on CosmosWorks if you haven't already.

[RStory]

I've imported wire frames from Pro/E into ANSYS, I know it's possible, but it's been a while so I don't remember exactly how unfortunately. I don't remember it taking a long time to load though.

[BuckeyeMike55]

I wouldn't use ANY FEA package aside from ANSYS Classical for this analysis (or some equivalent program). Having taken a course on FEM using ANSYS classic, there is no really good way to approach analysis of a tube frame chassis other than ANSYS classic, and I give you this reason:

FEA programs with a beautiful GUI lack the ability to apply a load at a nodal point (where your tubes meet together). Don't quote me on that, but it has been my experience that it is rather difficult to correctly load your chassis using 'pretty' GUI FEA programs, such as ANSYS workbench and COSMOS, because they only allow you to select loads at the following places (in the case of a round-tubular joint):

1) Along the Cross-sectional face (great, if you're doing a tensile test of a beam not at a joint)
2) The outer or inner diameter of the tube at the cross section (unrealistic loading)
3) Along the ENTIRE face of the tube (I don't think i need to explain the errors with this approach)

I taught our chassis leader this year how to model through using BEAM 188 ELEMENT, keypoints, lines meshes, and applied COMMON BEAM SECTIONS and after having used ANSYS classic for analysis of a tube chassis he wouldnt use anything else to approach chassis design of a tube-frame car. ANSYS can be a bit frustrating to new users, as you may know any error and you have to restart the program over. However, if you didn't know the .txt file method this is where ANSYS becomes less cumbersome.

Whenever I analyze anything using ANSYS Classic 10.0, I always save my steps by going to file >> write DB log file >> (select the dropbox) >> write essential commands only. Locate the file, open it with notepad and you can then copy and paste that into the command window and it will repeat every step you made. This also works with IGES / .SAT imported analysis, as long as you have the directory location of the file correct at the top of the text file.

If this is all old news to you, great. I would highly recommend approaching your analysis using the method i described. I've included a file of a square box with displacements and loads so you will have a better idea of what im talking about.

>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>

KEYW,PR_STRUC,1 !Selecting structural menu (preferences)
KEYW,PR_THERM,0
KEYW,PR_FLUID,0
KEYW,PR_ELMAG,0
KEYW,MAGNOD,0
KEYW,MAGEDG,0
KEYW,MAGHFE,0
KEYW,MAGELC,0
KEYW,PR_MULTI,0
KEYW,PR_CFD,0

/prep7

ET,1,BEAM188 !Beam Type

MPTEMP,,,,,,,, !Material Property
MPTEMP,1,0
MPDATA,EX,1,,30e6 !Modulus of Elasticity (30e6)
MPDATA,PRXY,1,,.29 !Poisson's Ratio (.29)


SECTYPE, 1, BEAM, CTUBE, , 0 !Beam Section Type (This case, round tube with .9" ID, 1.0" OD, 10 divisions (finer mesh))
SECOFFSET, CENT
SECDATA,.9,1,10,0,0,0,0,0,0,0

k,1,0 !Entering keypoints for lines
k,2,10,0,0
k,3,0,0,10
k,4,10,0,10
k,5,0,10,0
k,6,10,10,0
k,7,10,10,10
k,8,0,10,10

l,1,2 !Now connect the dots! (like you did in kindergarten)
l,2,4
l,4,3
l,3,1
l,1,5
l,5,6
l,6,7
l,7,8
l,5,8
l,7,4
l,6,2
l,8,3


FLST,5,12,4,ORDE,2 !Meshing the lines with the circular cross section
FITEM,5,1
FITEM,5,-12
CM,_Y,LINE
LSEL, , , ,P51X
CM,_Y1,LINE
CMSEL,,_Y
LESIZE,_Y1,.2, , , , , , ,1 !Mesh every .20 inches
FLST,2,12,4,ORDE,2
FITEM,2,1
FITEM,2,-12
LMESH,P51X !End Mesh

/eshape,1 !View graphic representation, NOTE: Joints shown are purely graphical (for stress plots), and the actual representation of each joint is a node with lines connecting.


d,1,all !Fixing the "left" wall
d,351,all
d,201,all
d,102,all

f,463,fy,1200 !Applying load along tube, near midsection-top, in the x and y direction
f,463,fx,3000

/solu
solve

/post1 !Postprocessing

PRRSOL !List all Nodal Reactions
PLESOL, S,EQV, 0,1.0 !Von Mises Stress Plot

>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>



NODAL REACTIONS:

NODE FX FY FZ MX MY MZ
1 -212.95 -170.84 -86.227 268.47 453.22 -972.43
102 -1088.1 -688.36 -86.227 268.47 453.22 -3442.5
201 190.91 -111.01 86.227 278.52 -563.42 -803.83
351 -1889.9 -229.79 86.227 278.52 -563.42 -2171.2

http://img518.imageshack.us/my.php?image=file002ho5.jpg

As far as importing your chassis into ANSYS... you will most likely have to model it in Solidworks, SolidEdge, Catia, or whatever CAD program you have and then take all of the points relative to an origin and enter them as keypoints. Then connect the dots (This can be a bit tedious, but it can all be done in 1-2 hours, and after it's done, modifying the points is relatively easy).

If anyone wants a more detailed tutorial, I would be happy to help. Some of the commands are fairly self explanatory, but I did skip a lot of the graphical stuff here.

[JR]

Here's a time saver. Measure the x,y,z location of each point using the measurement tool in Solidworks. Highlight the text output of the measurement tool and hit ctrl-c to copy. Paste that into an Excel column with ctrl-v. Do that until you have all important points in Excel (1 column per point.) Add a row of the letter 'K' just above your solidworks data. Now you should have 4 rows (The letter K, X data, Y data and Z data). Then transpose the matrix in Excel so that you have 1 row per point. Export this file as comma seperated values... and you have a ready made ANSYS list of keypoints. You'll still have to connect the dots by hand though.

[Coombesy]

Just a bit on shell vs beam and a little bit on workbench, I can't comment on cosmos as I haven't used it.

I believe anysys workbench to be better for the vast majority of simulation of solid models, particularly because of the loading methods. It is much easier to apply grouped, more realistic loads that in anysys classic. While you can't apply loads to individual nodes in workbench, at least I don't think you can easily; this is not reprehensive of loads in a solid model based structure. Off the top of my head, you can load bodies, faces/surface, lines and vertices, which I tend to think is sufficient for most models.
For doing beam and truss analysis I use classic, for all the above reasons.

In the reference to beams vs shells, both work and beams are much quicker to solve, though slower to setup initially. I prefer using the solid model with a shell mesh, and being able to rip it from cad, to FEA, analyse make any changes in cad, whip it back to FEA, and damn near just hit solve again. (which is partially easy with workbench and the proE interface). Solve time hasn't proved an issue so far, with a good mesh on the front of the chassis, it was less than 5 minutes (probably 2-3, I can't really remember), which is fine for what I was looking for.

Truth be told I am using Ansys Classic at the moment for the chassis, because I am better able to control the mesh from there and manipulate the model. The final analysis of the final chassis will probably be done in workbench.
None the less, I believe both methods work fine, and in this case it's pretty much a matter of preference.

[BuckeyeMike55]

I agree Coomesy. Because of the solidworks plugin for Workbench, and the ease at which you can change parts and update / start a new analysis within a workbench 'project' file, I love workbench for solid model analysis (I.E. drivetrain components, mounts, brackets, etc). I used COSMOS a few years back, but it is much less user friendly when it comes to running several different scenarios for the same part (i.e. different iterations and saving each analysis of the different iterations within the same file). Workbench is extremely easy to use, you never have to overwrite old analysis / iterations, and it has a relatively small learning curve. As I was told by a TA that worked in industry for a while: First you learn Workbench, then you learn Classic ANSYS, then you move on to LS-DYNA. I've never seen LS-DYNA and the university is too cheap to get it, but it appears to be a high-end dynamic solver.

Anyways, don't mean to get off track. I'm curious, however, to see how you are going to get better results with workbench than ANSYS Classic on your final chassis. How do you plan to approach it in workbench (citing the flaws I pointed out above with Workbench and similar programs)? Univ. of Cincinatti helped in pointing me in the right direction of Chassis design (with beam elements), and from their torsional rigidity tests they had nearly spot on data in comparison with their ANSYS classic FEA models. Someone from Cincinatti correct me if I'm wrong...

[Travis Garrison]

Mike,

If a program supports beam elements, by definition it supports point loads. Catia for example gives you the user friendly interface, and beam elements.

To me shell elements on a space frame seems like a waste but if it helps you run itterations smoothly...well to each their own I suppose.

[Coombesy]

The reasoning is a bit rounds about's but here it is:

We started with our chassis model, and instead of making pipes with a wall thickness, they were left as solids.

This was done specifically so we can send it to ansys, and shell mesh all surfaces, with a set thickness, and quickly look at the overall layout of the chassis.

For these simulations accuracy was not a big issue, it was used for comparative sizing and load pathing. The only reason I used classic was because I knew I could mesh the entire external surface as a shell easily.

Now the that the layout for the chassis is locked in, I plan to use workbench, with quicker loading, ease of adding loading situations "environments"�. The plan is to use workbench's mid plane extraction tool, and put the correct wall thicknesses in. The solver isn't any more accurate, but the model is.

I haven't validated this method, but it should not be far off. I am very interested in the fact that the beam method you talked about has been validated and accurate.

[rwolcott23]

When I did chassis development we used Pro Mechanica for the analysis and it worked great. We modeled the chassis as curves and then assigned beam idealizations to each curve. Shear panels were modeled as shells. We also imported this model into Ansys to compare results and they both were in agreement within a few % with a stress profile that was a mirror image.

The great thing about this method was that everything was parametric and the analysis took less that 30 seconds each. I could run ten analysis with design adjustments between each run in the span of 30 minutes or so.

The results were not necessarily accurate but very precise. It worked very well in eliminating bending moments on frame members and distributing the loads throughout the chassis. Great tool for optimization.

Last time I checked (2005) Solidworks did not have beam idealizations as an option making it very unsuitable for chassis FEA.

Bob

[BuckeyeMike55]

[QUOTE]Originally posted by rwolcott23:
everything was parametric and the analysis took less that 30 seconds each. I could run ten analysis with design adjustments between each run in the span of 30 minutes or so./QUOTE]

I found our chassis guys FEA analysis models of the '07 vehicle (ANSYS .txt files) and just to further emphasize why beam models are great for chassis FEA (as bob stated with his method) is that it literally took less than 30 seconds to solve a full chassis model (that includes every step, from keypoints, lines, meshing, applying loads / displacements, etc...). I knew it was quicker than shells, but I couldnt remember exactly how quick.

Here's a pretty picture of one of the early working files we had from chassis FEA for the '07 car.


http://formulabuckeyes.com/uploads/images/mow.JPG

[BuckeyeMike55]

I was informed recently that Solidworks 2007 has beam element analysis. Check it out.

[Grant Mahler]

I ran into so many problems with Solidworks crashing (due to improper installation by the university) and Ansys crashing (when importing the igs file) that I gave up for the time being. I'll try again in September when they install SW 2007.

Oh, and since we did our frame using 3D drawings in SW2006, the coord's given for endpoints/nodes were not universal - instead they were particular to that drawing, which was useless. I'll draw the whole things again in September, in Ansys, and in SW2007, and analyze it then.

Oh, and shell mesh in 2006 or 2007 does not seem to like tubes - even just a simple Y with 2 tubes intersecting crashes SW for me. Not sure what is up with that.

[consig]

I just finished doing a SW2007 FEA on a solar car frame. It is fundamentally the same thing as an FSAE chassis. COSMOSworks beam elements made this extremely easy, after first doing the beam mesh tutorial it took less than five minutes to set up an FEA on the frame. The simulation was solved in less than thirty seconds. I also ran a few FEA's on our old formula frame for practice an it was also very easy.

**note** the frame should not be a series of extrusions and cuts but should be a weldment. This is actually much easier to do, just take a minute to do the weldment tutorial. Also, I don't think that the beam mesh will work with bent tubes so you either have to make an approximation of your roll hoops and such with pieces of straight tubing or maybe try a mixed mesh using a solid mesh for the bent parts.

**also note** I initially had some problems with the SW2007 installation. No folder, or an unavailable folder had been specified for the FEA study temporary files. This is usually due to restricted access to write on certain drives or folders, as is common on school computers.

[billywight]

**note** the frame should not be a series of extrusions and cuts but should be a weldment. This is actually much easier to do, just take a minute to do the weldment tutorial. Also, I don't think that the beam mesh will work with bent tubes so you either have to make an approximation of your roll hoops and such with pieces of straight tubing or maybe try a mixed mesh using a solid mesh for the bent parts.


An approximation (with a bunch of strait sections) should work out a lot easier and more precise than a mixed mesh for a bent member. In 2008, SolidWorks will work with curved beam elements.