FEA rigging design

This post is probably premature, but I have just downloaded a "student version" of a civil engineering FEA program called AxisVM-8 (free!) that has so far blown my socks off! There is no time limit on this trial version, but it is limited to 40 beams, etc.

I can do a lot with 40 beams, especially if those "beams" are masts and spars and shrouds!

There is the ability to enter your own custom materials into the database (5083 al, for example) and your own custom "shapes" as well. After playing with this program for a few hours I think that it could be used to design the rigging on a sailboat if that boat had less than 40 masts and stays, etc.

But I haven't tried it yet. I hope someone who actually knows what he is doing will go and watch the demo programs to see what this thing can do and express another opinion here. After looking into the usual ways of working through a rigging design with a spreadsheet . . . this approach looks great to me. Go here to get a copy and watch the tutorials: http://www.axisvm.com/demos_dwnlds.htm.

BillyDoc

 

Giving it a try . . .

Well, I guess I'll have to get a little more specific about this approach to rigging design. I am very reluctant, because I live in the United States and we are up to our eyebrows in lawyers here, with all of them apparently just waiting to slap a liability suit on somebody given any excuse at all. They wouldn't get enough from me to make it worthwhile because I would spend every last dime fighting them . . . but who needs the grief? So, let me be very plain here, I AM NOT AN ENGINEER OF ANY SORT!!!!! I'm just trying to design my own boat and I think I found a nifty way to spec out the loads on the rigging which I would like to share, but I refuse to be liable for any stupid thing you do with the following information, in any way, and at any time. I mean it. You paid nothing for it, and that's what it's worth!

That said, I am going to go ahead and ACT like I know what I'm doing just to keep the English manageable. I repeat though, I DO NOT know what I'm doing here. Moreover, I have no idea at all why anyone would read the following post and give it any credence at all given the aforementioned non-engineering background. I really, really hope that some of the members here who DO know what they are doing will tear this post apart and explain why.

So, onward.

The question is: if I put a pole up in the air on the deck of my boat, and then hang a bunch of sails on it, how strong do I have to make my rigging and pole to keep things intact under all foreseeable conditions. I know I could use very rugged materials, but the weight aloft does all sorts of nasty things if I do, so I am very interested in the lightest rig commensurate with sufficient strength.

Assuming the amount of force that will have to be absorbed and handled (the force to heel the boat 30 degrees, or whatever), and the area of the sails to hang up on the poles and wires is known, then the AxisVM-8 program mentioned above seems quite capable of doing a very nice job solving this problem and reporting exactly how much force is applied where under any given conditions. I have only played with this program for about 6 hours now and got this far, which should encourage the feint of heart quite a bit. Let me show you what I think it can do with an example.

Keep in mind that I am making up the numbers used as I go along just to see if something workable can be done here.

Assume a double-masted schooner with a gaff main and twin headsails. There are at least two ways to enter data in AxisVM (this program has so much, it is amazing!), but in the first figure below (Setup) I simply used the graphical interface with a snap-grid and eye-balled in a couple of masts about 12 meters high, with shrouds and stays as shown. I then just picked some aluminum tubes for the masts and spreaders (actually two pipe sections for each mast, but you can enter into the program any cross-section you want) and some steel rod for the rest of the rigging. All this can be refined later.

Just to add some realism, assume the following areas for the four sails:

Outer jib: 22 square meters.
Inner jib: 13 square meters.
Main: 45 square meters.
Mizzen: 25 square meters.

Areas for the two foresails are the areas you would actually see on a side-view drawing showing the fully deployed sails. In other words, the part of the sails “masked” by other sails is not included in the area for that sail.

OK, so we have 105 square meters to play with, distributed as shown. Now assume the force that will heel the boat 30 degrees (or whatever measure you use) is 10 KiloNewtons. (For the metrically illiterate, just remember that the Newton is roughly equivalent to a quarter pound. Remember the Newton-berger that the fine Scottish Restaurant with the Golden Arches made famous?) Anyway, the first thing we need to know is how that force is distributed on our sails. We can do this by doing a “ratio and proportion” calculation: So, for example, the outer jib with 22/105ths of the total sail area will need to handle 22/105ths of the 10 KN we are applying. Dividing 22 by 105 gives us roughly 0.209 and we multiply this by 10 (for the 10 KN) to get a total of 2.09 KN for that sail.

The outer jib is masked by the inner jib, leaving an exposed area that is a tall rectangle with a triangle at the top. AxisVM allows you to set up “nodes” anywhere you want to, so you can represent this force by following the menus and linking together the forces on the fore stay as two separate sections. In the example the fore stay is 8.8 meters long near the bottom where the sail appears rectangular, and 4.7 meters of “triangle” at the top. This is a total of 13.5 meters, but the top 4.7 is a triangle so effectively has only half the area as an equivalent length on the bottom. No problem, just divide that 4.7 by two, add that to 8.8 and lie about the length. That makes the “effective length” 11.5 meters. Now, the program wants the force applied in KN per meter, so divide the 2.09 you obtained above by 11.5 to get the force per meter and fill in the appropriate window. You just do each section separately. So the bottom section has roughly 0.2 KN to start and to finish, but the upper section has 0.2 to start and 0 to finish. This gives you a force distribution equivalent to the force actually applied by that sail.

You can take the same approach to any sail that isn't too weird, and if it is a strange shape you can just assume an “oversize” but regular approximation of it for these calculations. The object is to tell the rigging what the forces really are and how they are distributed, not how the sails look in all their sophisticated glory.

After applying the forces to all of your “beams” (masts and stays), you must indicate how the “nodes” on the deck are attached. That is, are they rigid and can't flex or rotate, or something in between. It's dead simple to do this with AxisVM, you just select the node or nodes and fill in the boxes in a window. After all of that you might have something that looks a little like the second figure (Forces).

Then you can go to the “static” tab and tell the little man in the box to get to work and make those calculations! Now take a look at the third figure (Analysis). In much less than a silly second on my computer all the information I need to design my rigging has been produced. the figure shows the magnitude and location of the forces applied. This is all I really need to pick a shroud wire, for example. With a safety factor, of course! If you bother to use actual cross-sections for your members the program will calculate the max (or min) stress applied per square mm, and where it is located. At this point, if we were doing this for an actual boat, I would go back and enter actual dimensions and materials and re-run the analysis. The program will calculate the buckling forces on the mast, and on the spreaders. It will do a vibration analysis. This program seems to me to be capable of anything I need to do here, in fact. Oh, and in the figures I show here the forces are applied directly abeam, but you can rotate them to any angle you want by playing with the proportion applied in, say, the x and y directions (sines are helpful for this, assuming your orientation is z up, then the sine of the angle of interest times the force applied will give you the “y” value, which can be subtracted from the force for the “x” value . . . I think. I could have my sines and cosines mixed up here . . . hell, it's easy, just try it and see how it works!).

If you get the impression that I really like this program, you would be right! And especially at this price (did I mention that the “student” version is free?). I assume that the people at AxisVM that have developed it appreciate my “spreading the word” about it, even though our application is downright trivial compared to what it can actually do. I also sincerely hope that they get a few real sales from our interest in sails, they definitely deserve them.

But let me repeat once again for the benefit of all the #$%**! lawyers out there: I AM NOT AN ENGINEER AND I DON'T KNOW WHAT I AM TALKING ABOUT!!!!! SO YOU ARE ABSOLUTELY RESPONSIBLE FOR ANYTHING YOU DO WITH THIS INFORMATION, DEFINITELY NOT ME.

BillyDoc

P.S. The “Rigging.zip” file has the model data in it for the example I used here, if you are interested.

 

Be very cautious of doing FEA of rigging. There are two things that can easily kill. One is the unknown eccentricity, the other is the unknown fixety. Both effect Euler buckling. I know of none that use FEA for FINAL rigging design....too many unknowns.

 

How well do you know the load case?

There are some very bright people working on CFD for sails. You can't just guess a load case with FEA.

Tim B.

 

Welcome to the world of FEA! Congratulations on grasping the principles so quickly. Be warned however, I do this stuff full time and I still learn new things every day – there is a world of difference between drawing a pretty picture and getting accurate results. To be able to fully understand, interpret and trust the results you need a sound understanding of structural engineering. Otherwise you will have no idea whether a simple typo has ruined your analysis, or whether you have applied realistic boundary conditions, or whether you have selected suitable element types (shrouds, for example, should be tension only elements – wire obviously doesn’t provide support in compression). Deciding on a Factor of Safety is always tricky, especially if you don’t know what you don’t know (if you know what I mean!).
Finally, make sure you do a sanity check by comparing your results against a more traditional rig sizing method.
Have fun, FEA is a very powerful tool.
I don't know Axisvm - we use Ansys, but I don't think you can get a free trial/student copy of that and the licenses are hugley expensive.

 

Thanks everyone!

Thanks for your replies, everyone!

I am well aware of the old adage that says: "To err is human, but it takes a computer to REALLY foul things up!" and certainly intend to verify any results obtained in this way with the more traditional approaches.

Tim, I sure wish some software would come out that used a CFD approach for the sails (software that I could actually afford, that is) but I don't know of any at this time. So, it looks like I will be forced to determine rigging loads "backwards" by inferring them from the heeling moment, or some similar approach. This will obviously work, backwards as it may be, but tells me nothing at all about the distribution of forces developed by the sails themselves. For this, I have to guess. Even worse, when trying to balance the sail plan against the hull I will be reduced to either cutting out a cardboard model of the underwater profile and balancing it across the edge of a ruler or the mathematical equivalent of the same to determine the point of lateral resistance; and then aligning this balance point with the mathematical average of the sail area plus some "fudge factor" based on experience with the particular type of boat. This approach is not very satisfying, to say the least. But, is there a better way? At least with the FEA I can define a distributed load that looks like a better guess than no guess at all . . . which seems to be the available alternative.

PI, you are so right about a basic understanding of the stresses and strains being absolutely necessary. I guess you noticed that the leeward shrouds were in compression in the example given, which isn't going to work too well in practice. On the other hand, I think that if I add the compressive force on the leeward shrouds to the tensile force on the windward ones the result should be something close to the real number I need to size those wires prior to multiplying in a safety factor. Does this seem reasonable?

jehardiman, I hear your warning loud and clear and agree completely. This is just another tool that must be used with a bunch of others. On the other hand, this particular FEA program is specifically designed for structural design (buildings) and I would expect it to be fairly accurate when determining loads and the location of those loads . . . which is very useful even if it is not used for anything else. As for the buckling of a specific mast, I would trust the mast manufacturer's numbers on that one.

 

I'm honestly not too sure about that. As you should be well within your elastic limit it might be okay, but the fact that the leeward side is providing support will be affecting the deformed shape and hence the stress distributions. Have a look the programme in more depth - it may well offer a tension only beam as an option. If its a civil enginerering code it should be able to cope with suspension bridges, which use cables obviously.

 

Exactly right PI design

I went back to the program and looked for a way to define a beam as tension-only . . . but there is so much here that I couldn't find it. So, I just deleted all of the shrouds and spreaders on the leeward side of the model and ran the analysis again. And you were exactly right, the stress distribution changed and the numbers moved accordingly. Just adding the compressive and tensile stress for, say the main mast lower shrouds would have given a value of 7.553 KN (taking the mean of the two extreme values, 4.067 and 3.486 from both ends of the scale and adding them) but when the leeward shrouds are removed to simulate tension-only the windward ones then show a 6.879 KN loading (again, averaging 7.805 and 5.953) for the same shrouds.

This seems like a fairly significant change to me, probably because of deflection in the mast transferring more of the load to the upper shroud. AxisVM does give deflections as well, but I didn't think to look at this when I had windows booted (I normally use linux).

 

Deleting the leeward shrouds was a good idea. I find it very useful to look at the deflections. It is one of the simplest ways of checking that the loads and constraints are at least vaguely right. Its so easy to get your signs wrong, or miss a decimal place...

 

You are so right, PI, and I need all the "sanity checks" I can get. Here are the deflections for the model above, but remember that the "rigging" picked was very arbitrary and damn stout for this example, so there simply wasn't a lot of deflection to show. Still, things do look like they should to me.

 

As you want your tension only shrouds to only carry tension not any bending, make sure each shroud is made up of only one element, and that each shroud element only has two nodes, i.e. one at either end so they cannot carry any bending loads, these are often refered to as spring elements. Also make sure there are no rotaional contraints in those nodes. All three rotational freedoms should be free.

Sometimes it is hard to tell which shrouds really are in tension, so this should be an iterative process. Check all your shrouds to make sure none are carrying compression loads. Then delete those that are are, rerun the analysis and check again. You will know if you have gone to far as the solution will fail if you have.

All the best

Gareth
www.fourhulls.com

 

Hi Gareth,

In the model above I did leave the rotational constraints free, but I was guessing about that, and I'm glad to hear that the guess was good. You mention "spring elements" and AxisVM has those as well as "link elements." I suspect that the "link elements" may be the "tension only" elements I was looking for, but couldn't find. Unfortunately, I couldn't figure out how to use either, at least without spending more time than I have this morning. I definitely appreciate your excellent advise on this.

Has anyone else downloaded this program to play with it?