beam element FEA

[adrial]

Yeah, this is another FEA thread related to the chassis...but I dont think this has been discussed yet.

How do you do a beam element FEA? I draw say a single line in mechanical desktop and then try to bring it into ansys 9.0 workbench but it is unable to. I was told Ansys was capable of doing this...was I told wrong?

Do any of you guys have any experience with the Mechanical desktop/Ansys combo? We also have Algor and cosmosexpress available to us, but again we havent had any luck. There must be something simple that I am missing.

I have a year and a half of experience FEA'ing various parts with Ansys, but they have always been solid models.

thanks for any help... I am not asking for anything to be handed to me... just point me in the right direction.

--Adrial

[adrial]

Yeah, this is another FEA thread related to the chassis...but I dont think this has been discussed yet.

How do you do a beam element FEA? I draw say a single line in mechanical desktop and then try to bring it into ansys 9.0 workbench but it is unable to. I was told Ansys was capable of doing this...was I told wrong?

Do any of you guys have any experience with the Mechanical desktop/Ansys combo? We also have Algor and cosmosexpress available to us, but again we havent had any luck. There must be something simple that I am missing.

I have a year and a half of experience FEA'ing various parts with Ansys, but they have always been solid models.

thanks for any help... I am not asking for anything to be handed to me... just point me in the right direction.

--Adrial

[Jersey Tom]

I wouldn't trust Cosmosexpress...

Mechanical desktop? I feel sorry for you guys.

So you're trying to basically take a 3d line drawing, bring it into an FEA suite, and define those lines as structural members and then analyze it? Can't say I've got the solution to your problem, but the quick and dirty way of doing it would be to just sweep solid bodies along all those lines, trim as appropriate, and analyze that.

[Sisyphus]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">
....How do you do a beam element FEA?...

...We also have Algor and cosmosexpress available to us, but again we havent had any luck. --Adrial </div></BLOCKQUOTE>

I use Algor to analyze tube frame race cars and it works well. I use an older version (V12 and 13) and like the relatively simple set of drawing tools it has.

ANSYS will certainly work but it is a more complex package. It's mainly a function of what software package you are used to but you might give Algor a try. It's easy to combine shell elements with beams to model sheet metal gussets.

Oh, and you are going to check your results with a simple test piece regardless of which software package you use, right?

[Will Steed]

It's easy if you use Ansys not shi**y workbench. Make two keypoints in Ansys, then make a line, define section or real constant, set line divisions and then line mesh. There is no "3D solid" geometry to beams. If you use section properties you can turn on element shapes by typing "/eshape,1" at the command prompt. Then it will look "3D". To turn off element shapes replace the "1" with "0". Ansys is the way to go with designing these frames. You should be able to figure out the rest.

[Captain Redbeard]

I would suggest NOT sweeping solid bodies along your lines as the calculation times will skyrocket. ANSYS is a little funky but I have had success importing an IGES file from ProE and defining the elements from there. The easiest way I have found to do frame analysis is using ProE/ProMech. I can change the frame and re-run the FEA in less than 2 minutes. Super easy, fast, and its all in one package.

-Redbeard

[adrial]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">The easiest way I have found to do frame analysis is using ProE/ProMech. I can change the frame and re-run the FEA in less than 2 minutes. Super easy, fast, and its all in one package.

-Redbeard </div></BLOCKQUOTE>

I think we have promech but I haven't used it yet. I will give that a shot. How do you have the frame drawn in pro/e when you bring it into promech? We have the chassis drawn in pro/e as a solid model, with points at every node so this would be the easiest way for us.

thanks for the tips

--Adrial

[Captain Redbeard]

So, you are probably using pipes to fill in between the points. The best way would be to suppress all the pipes and replace them with just simple datum curves. Then, switch over to ProMech and define you idealizations (beams), loads, and constraints. You can define different beam elements and select all the appropriate curves. Assigning loads and constraints is as easy as picking the points and giving them values. Then, run the simulation, on our 3ghz machine it takes around 5 seconds. Viola! Hope this helps. See if you can find someone who knows ProMECH because nothing in either of these programs is easy to figure out on your own. PTC puts out the most non-intuitive software on the planet, but once you learn it, you're golden.

-Redbeard

[adrial]

Awesome. We do have promech and it looks like it'll work great.

We will have to redraw the chassis because some of the points are referenced off of protrusions...but that shouldn't take too long. I did a quick FEA of a single axis and everything looks good...

thanks a lot everyone
--Adrial

[adrial]

We have the chassis drawn up and have assigned properties to each of the tubes using primarily the point to point reference system.

Whenever we attempt to run the FEA (regardless of number of constraints or loads), we always get an error saying "The model is insufficiently constrained for the analysis.
Please review the element connections, properties, and
constraints."

I have run a simple FEA on 3 points with no trouble.

Does anybody have any suggestions?

thanks for any help,
Adrial

[Matt Gignac]

Just tried a frame analysis with pro/mechanica and I agree it couldn't be easier. Did a few quick comparisons with Ansys and analytic solutions of simple beams, and it's reasonably accurate.

How do you refine your mesh though (or even see how many elements per beam or unit length). I don't imagine it's a big deal in most cases, but in some areas we have many tubes close together, and I can't figure out how to get proe to have smaller beal elements in these areas.

Matt Gignac
McGill Racing Team

[Ppada]

Well Maybe the problem you have with pro-E is that you don´t define how you mate the things together. There is propably a tool where you could do all the weldings you want.
I´m not sure thought. I suggest you do the fea with a fea program.

[Matt Gignac]

We already do beam element FEA with Ansys, but having the analysis directly linked to your model is interesting in terms of how quickly you can iterate. More than likely we'd do a trend analysis in pro/mechanica, and do physical testing to see how the predictions correlate.

I imagine the equations used for the beams are the same, so the only thing I can see that will affect the accuracy of the solution is how you discretize the problem, so how many elements you split your beams into, especially in critical areas.

Matt Gignac
McGill Racing Team

[buddy]

adrial,

have you tried making sure all real constants for the beam are specified? i.e. Ixx, Iyy, Izz Probably some menu for it in 9.0

or you can type
r,real number,c1,c2,c3... try help for the r command

alternately from the mech GUI input you can just program the model...

/prep7
et,1,beam4 !can use higher order ifnecessary
n,1,x,y,z
n,2,x,y,z
r,1,c1,c2,c3... !sets real properties of element
real,1
type,1
e,1,2
e,2,n

d,1,all,0 !sets displacements on node 1
f,2,all,2 !sets forces on node 2 to value 2(units)

/solu
antype,static
allsel
solve
fini

!commands should still work in 9.0, that took like 5 seconds. Make sure your beam elements have the nodal coordinate systems are oriented correctly

[Erik Whoa]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by adrial:
"The model is insufficiently constrained for the analysis.
Please review the element connections, properties, and
constraints." </div></BLOCKQUOTE>

How do you have your model constrained?

[adrial]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by Erik Whoa:
<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by adrial:
"The model is insufficiently constrained for the analysis.
Please review the element connections, properties, and
constraints." </div></BLOCKQUOTE>

How do you have your model constrained? </div></BLOCKQUOTE>

I am using a displacement constraint, fixed in all translation and rotation. I've tried overconstraining the model just by throwing constraints everywhere...with little luck.

When you define a beam as a point to point and it asks for the Y direction. I typically just use "Vector in WCS" and assign a value of 1 to either Y or Z depending on the tube. Is this OK? What is this actually doing?

buddy,

I am running the FEA in Pro Mechanica now, not Ansys 9 workbench.

Ppada,

Thank you for that piece of advice, but if you read some of the other posts in this thread you will find that Pro Mechanica works great in this application.

Matt,
Do you use the traditional version of Ansys or Workbench?

--Adrial

[Erik Whoa]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by adrial:
When you define a beam as a point to point and it asks for the Y direction. I typically just use "Vector in WCS" and assign a value of 1 to either Y or Z depending on the tube. Is this OK? What is this actually doing?
</div></BLOCKQUOTE>

After you input all of the keypoints for your frame, you should be able to construct the frame using "Create lines from keypoints." It should not ask you about any direction. You should be able to click on the keypoints one by one. As long as you have the correct element and material properties, and correct real constants, the model should work.

Do you have a node specific for the suspension mount? If you only include the "nodes" of the frame, and then apply a force in the middle of a beam, it will not work. There must be a node/keypoint for your force.

Also, what happens if you only constrain the model in translation, not rotation?

This is all with Ansys.

[Captain Redbeard]

Hey Adrial, I can't tell if people are giving you advice about Pro/MECH or ANSYS. To answer your question about the "vector in WCS" problem, I have always just entered whatever did not throw me an error. I have never had the problem you are having so I'm not sure what to tell you. I can tell you that I have always defined datum curves between the points to represent the frame tubes. I then define the types of tubes we use (one element for 1 x .095, one for 1 x .049, etc.) and select all the datum curves that are built from that element. I would suggest doing this and seeing if it solves the problem. I imagine that Pro/MECH might not like defining everything from points as there are no actual connections defined in the model. Hopefully that will work for you.

-Redbeard

[buddy]

Sorry about the mix up. I like ANSYS if you can't tell (because I use it all day).

The vector you are specifying sounds like the orientation of the beam. i.e. two axis will be bending axis and one will be an axis of rotation (or twist) for the beam. I am not familiar with Pro/Mechanica specifically, but this information is usually important for determining what value of Inertia to use for that axis. (Ixx, Iyy or Izz) In ANSYS the solution output (for beams) is also sensitive to the orientation of the nodal coordinate system for each node, Pro/Mechanica may be similar.

Best of luck,
buddy

[Gareth]

You should load your FE model using a torsion fixture similar to what you use to test in real life. Look for previous torsion fixture threads for a description of how to twist the car without over-constraining it. This is extremely important in FE as it will jack up your stiffness predictions and give you meaningless results.

For simple comparisons and reasonable predictions you should use a 1D beam element model, as suggested above. Most of the solvers mentioned above should be capable of this, provided they offer a decent range of constraints/connections. You MUST load the chassis through the suspension, thus you need ball joints at the appropriate places. Again, without them you will be led in the wrong direction by the FE and the results will be meaningless.

We use Hypermesh for pre/post processing and the ABAQUS solver. ABAQUS bar elements (B31s) do not have stress gradient information and do not predict shear through the cross-section accurately due to their formulation. I would imagine this is the case for all of the above solvers. The result is that they become less predictive over short lengths. I'm sure your solvers will have documentation on this. To do detailed design on particular nodes I think you'll need to mesh the actual tubes and stitch them together at the weld locations. You can tie this into your 1D beam element model such that the joint is still properly loaded. Tragically I'm not sure how capable Pro/Mech is in this respect. I v2001 and didn't think that much of it. Maybe it's improved in WF/2? Ansys is a good solver if you have a good pre/post-processor...ICEM is the good one right? I don't really have any experience with it, but I haven't heard people bad talk it too much. ;-)

Again, the most important part of setting up your chassis FE model is the boundary conditions. Make sure your joints are working properly and do some quick checks to ensure they're behaving properly. Include appropriate sections of all the suspension components. Do a quick check to see where the stiffness should be gained by making the suspension rigid for a run and then the chassis rigid. Then start looking at relative displacements of nodes for tube placement and finally strain energy to see what tubes should be up/down-gauged. Our chassis designer made huge improvements this year on our method and consequently the stiffness result over our previous car. We're very pleased with him. ;-)

If you've got the time, you could setup the model in Optistruct (also made by Altair) and do a tube gauge optimization. Something tells me you need to define a design variable for each tube element (one each for wall and diameter) to get this to work. An excel macro could probably spit out most of the deck for this though...

[adrial]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by Captain Redbeard:
Hey Adrial, I can't tell if people are giving you advice about Pro/MECH or ANSYS. To answer your question about the "vector in WCS" problem, I have always just entered whatever did not throw me an error. I have never had the problem you are having so I'm not sure what to tell you. I can tell you that I have always defined datum curves between the points to represent the frame tubes. I then define the types of tubes we use (one element for 1 x .095, one for 1 x .049, etc.) and select all the datum curves that are built from that element. I would suggest doing this and seeing if it solves the problem. I imagine that Pro/MECH might not like defining everything from points as there are no actual connections defined in the model. Hopefully that will work for you.

-Redbeard </div></BLOCKQUOTE>

Bingo, defined datum curve between the points and assigned beam properties to the curves and it works like a charm. Now just have to bring the rest of the suspension in and we will be good to go.

[carbontub]

I have done exactly what you have stated above.I plotted all the points from the chassis in ANSYS 15.0 (manually) and applied a circular beam element as the
frame members are expected to be in Torsion and bending.

I had initially constrained all the 8 in-board pickup points and applied loads on the front pickup points and i got the following error" There is at least 1 small equation
solver pivot term (e.g., at the UX degree of freedom of node 1225). Please check for an insufficiently constrained model."

I randomly constrained more points to resolve the issue but my attempts were futile.I am successfully able to simulate simple truss configurations.

What could be the issue(s) here?

[Adam Farabaugh]

Try running a modal analysis with no boundary conditions. There should be 6 free body modes with really low modal frequencies. Other low-frequency modes should show mechanisms.

Also make sure your material properties make sense, orders of magnitude off could be a problem.

[apoorv]

Hey Adrial,
Try using Ansys workbench. Start with defining node points of the chassis and then join the hard point using the lines. U can insert points manually or use a notepad format in ansys workbench design modeler. Give cross section to each line.
Make sure u create a single part after all this in design modeler. Other wise it will show illconstrained error. This method is accurate, fast and easy. results are very good with this method.