Solidworks 2009 analysis - Simulation using beam elements problem

[BWill_Inc]

Hi:

I am trying to analyze my frame in solidworks 2009. Using the beam element, I feel my accuracy is way off. I have a previous model that tested torsional rigidity at 1700 lb-ft/deg and I ran the simulation in solidworks and it read 650. I know many of my members are less than the assumed 20X diameter. What can I do to improve accuracy?


I can't really adjust mesh using the beam element method as shown:
http://www.youtube.com/watch?v=jKnfo6I6zJU

the elements are very coarse and I feel it is way off. Any ideas for improving accuracy?

[BWill_Inc]

Hi:

I am trying to analyze my frame in solidworks 2009. Using the beam element, I feel my accuracy is way off. I have a previous model that tested torsional rigidity at 1700 lb-ft/deg and I ran the simulation in solidworks and it read 650. I know many of my members are less than the assumed 20X diameter. What can I do to improve accuracy?


I can't really adjust mesh using the beam element method as shown:
http://www.youtube.com/watch?v=jKnfo6I6zJU

the elements are very coarse and I feel it is way off. Any ideas for improving accuracy?

[Chris Allbee]

I'm not terribly familiar with the settings available in solidworks, but if you can make sure that the joints are not pin connections. If you have a node in the middle of a main tube then a pin connection will not provide the appropriate stiffness (think moment continuity across that main tube). Beyond that just make sure your sections are defined properly, again not familiar with solidworks, but most FEA software require a section orientation in addition to the beam axis.

In general an analytical beam simulation will OVER predict the stiffness of the frame.

In order to make sure you have the best comparison double-check your constraints and make sure they match the test condition as best as you can. If you have the capability, look at the mode shapes of the first few modes, torsion and bending at least, and make sure they seem reasonable.

You will always have a relatively large discrepancy when using analytical elements, and if you want more accuracy then you will need to move to using at least 2D shell elements.

If your school doesn't have access to real FEA software I think that Altair provides university licenses for free, or at least they used to. Their Hyperworks suite is pretty powerful and even has a built-in solver that can handle simple static loadings and even optimizations with relative ease.

In any case I recommend getting a proper pre/post-processor and solver package if you are aiming for decent accuracy, as within 5% of actual.

[Pennyman]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">In general an analytical beam simulation will OVER predict the stiffness of the frame. </div></BLOCKQUOTE>

I find this interesting, because last year we tested the frame the same way we applied loads in SW (holding rear mounts fixed, twisting the front), and the chassis was about 7% stiffer in real life.

[BWill_Inc]

We also have access to ABAQUS, ProMechanica, and the civil engineering program SPFrame. We modeled our frame using solidworks because it was easy to create the 3d sketches and apply weldments as in the tutorial on Youtube.

One teammate knows ABAQUS but only in 2d, and we have had no luck importing our solidworks part into ABAQUS. I would like to know if I can still use solidworks to analyze this frame with accuracy

Thanks for your thoughts again

[Chris Allbee]

Pennyman, thats why I said "generally". The amount and type of welding and any post treatments to the frame can have a significant impact on the stiffness of the final structure. A lot of people seem to think that the HAZ is "negligible" in a frame, but depending on the number of tubes at a joint and the skill of the welder involved (not to mention the equipment) there can be quite an impact on over-all stiffness and durability of the frame. And again, it is very difficult to capture accurate boundary conditions on an analytical body and transfer that loading 100% to a real frame. Take some strain gage measurements near the fixture points on the test and compare that with what your simulation shows. Just remember, one data point does not make a trend.

BWill, like I mentioned in my first post make sure that your joints are not of the pin variety. If you can't make SW work for you, maybe try looking at ProMechanica. Its not very hard to get set up with a basic beam analysis.

[Kirby]

[QUOTE]Just remember, one data point does not make a trend.
QUOTE]

http://www.phdcomics.com/comic...chive/phd040609s.gif (http://www.phdcomics.com/comics/archive/phd040609s.gif)

see bottom right.

[exFSAE]

Agree on durability, but I don't see how the HAZ would affect the stiffness of the frame. Modulus doesn't change.

[ed_pratt]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by BWill_Inc:
We also have access to ABAQUS.... One teammate knows ABAQUS but only in 2d, and we have had no luck importing our solidworks part into ABAQUS. </div></BLOCKQUOTE>

Hi BWill, using abaqus to model the frame is pretty straightforward. Has your team mate used ABAQUS command or ABAQUS CAE? TO be honest it's a whole lot simpler to write an input file with nodal coordinates / element locations / material properties / loading / constraints etc... than it is to actually create a CAE model and try to analyse it. Oviously the resulting pictures will be less pretty as they're line drawings but the results will be the same as you're using the same element.
Give element B33 a try - it's really worth getting to grips with a program like this as it's such a powerfull tool - it's also great with dynamic FEA problems i.e. impact attenuator.

I have a simple .inp file to run in ABAQUS but the constraints are setup incorrectly. Give it a go yourself and if you get stuck, PM me and il'l give you a copy - although, the obvious BEWARE applies as it's my own(rather hastilly done) work, and not yours.

Best of luck,

Ed

[Chris Allbee]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by exFSAE:
Agree on durability, but I don't see how the HAZ would affect the stiffness of the frame. Modulus doesn't change. </div></BLOCKQUOTE>

Sorry, did not mean to imply the HAZ altered the stiffness. That sentence was a bit of a mess. The part about welder skill and equipment was for the stiffness, while the HAZ was geared more toward durability.

Also, I have to agree with ed on the subject of ABAQUS. It is really powerful and writing a input deck is dead simple for a beam structure. At the same time though, I've spent the last 2 days trouble-shooting an ABAQUS/Explicit job...damn spotwelds....

Stick with Standard for your beam analysis. It will give you results in just a few seconds and if you are proficient with Excel you can have a spreadsheet linked to your input file to quickly change points and keep track of your data. Good luck.

[BWill_Inc]

How do I import the solidworks model into ABAQUS? I tried saving the model in solidworks as a .sat file. I then went to abaqus and tried importing it as a part but it failed. How do you import the geometry?

and would this method be more accurate then modeling the frame using shell elements?

[ed_pratt]

I wouldn't bother, unless your SolidWorks model is perfect you'll get dodgy results anyway.
For the purposes of using FEA to better optimise your chassis you're as well to start from scratch with an input file - written in notepad/wordpad - and tell ABAQUS where the nodes are and which which elements to use to connect them up.

Here is a VERY simple example. (copy into wordpad and save as a .inp file to run in ABAQUS)
There are some glarringly obvious problems (purposely) with this model, however, it should be enough to get you started.


Best of luck,

Ed
------------------------------------------------


*HEADING
FSAE CHASSIS ANALYSIS
*PREPRINT, ECHO=YES
*RESTART, WRITE
*NODE
1, 0., 0., 0.
2, 0.41, 0., 0.
3, 0.41, 0.41, 0.
4, 0., 0.41, 0.
5, 0., 0., 1.
6, 0.41, 0., 1.
7, 0.41, 0.41, 1.
8, 0., 0.41, 1.
9, 0., 0., 1.7
10, 0.41, 0., 1.7
11, 0.41, 0.41, 1.7
12, 0., 0.41, 1.7
13, 0., 0.45, 1.
14, 0.41, 0.45, 1.
15, 0.15, 0.53, 1.
16, 0.26, 0.53, 1.
17, 0., 0.53, 1.7
18, 0.41, 0.53, 1.7
19, 0.15, 0.9, 1.7
20, 0.26, 0.9, 1.7
21, 0.205, 0.98, 1.7
*ELEMENT, ELSET=TRUSS, TYPE=T3D2
1, 1, 2
2, 2, 3
3, 1, 4
4, 4, 3
5, 2, 6
6, 1, 5
7, 4, 8
8, 3, 7
9, 5, 6
10, 6, 7
11, 5, 8
12, 8, 7
13, 8, 13
14, 7, 14
15, 6, 10
16, 7, 11
17, 8, 12
18, 5, 9
19, 10, 11
20, 11, 12
21, 12, 9
22, 9, 10
23, 13, 15
24, 15, 16
25, 16, 14
26, 14, 7
27, 4, 15
28, 3, 16
29, 12, 17
30, 17, 19
31, 19, 21
32, 21, 20
33, 20, 18
34, 18, 11
35, 1, 3
36, 1, 6
37, 5, 10
38, 2, 7
39, 7, 10
40, 1, 8
41, 8, 9
42, 9, 11
*SOLID SECTION, ELSET=TRUSS, MATERIAL=STEEL
0.00024
*MPC
TIE, 15, 16
*MATERIAL, NAME=STEEL
*ELASTIC
209E9, 0.3
*NSET, NSET=rollbar
11, 12, 17, 18, 19, 20, 21
*BOUNDARY
rollbar, encastre
9, ENCASTRE
10, ENCASTRE
11, ENCASTRE
12, ENCASTRE
*STEP
*STATIC
*CLOAD
3, 2, 2000
4, 2, 2000
*NODE PRINT
U, RF
*EL PRINT
S, E
*END STEP

[L B0MB]

Did you set material property to 1020 steel?

Did you use the correct restraints?

2300Nm/deg (1700lbft/deg) is pretty good... what weight is that at?

I think our 09 frame is ~28kg and 2400Nm/deg

edit: numbers

[Patrick B]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by BWill_Inc:
How do I import the solidworks model into ABAQUS? I tried saving the model in solidworks as a .sat file. I then went to abaqus and tried importing it as a part but it failed. How do you import the geometry?

and would this method be more accurate then modeling the frame using shell elements? </div></BLOCKQUOTE>

This is what I've been doing:
To import your tubing, make a solidworks part file containing a 3d sketch that includes all the members you want to have in a single part. Save it as an iges, and import it to Abaqus. Doing this, I sometimes got the "too many attempts made for this increment" error. I fixed it by editing the step, and turning automatic stabilization on.

[Patrick B]

Oh hey, I just found this:

http://web.cecs.pdx.edu/~hormo...eframe_3d_points.pdf (http://web.cecs.pdx.edu/%7Ehormoz/me455555/winter10/wireframe_3d_points.pdf)

Extremely useful. If you import a 3d sketch, you can't edit anything on it. Following this little tutorial, you can make your own wireframe in Abaqus CAE, and be able to edit it in Abaqus.