Spar Stress FEA and Spread Sheet

Homebuilt Aircraft & Kit Plane Forum

Help Support Homebuilt Aircraft & Kit Plane Forum:

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Attached is a fairly famous spread sheet with my numbers, and a FEA report at the target location. I used pin constraints of the same diameter as my target design conversion. I only pretend to know what I am doing so any help the more experienced can give will be appreciated. I have many questions about the proper FEA inputs and about the proper spread sheet input. I promise not to sue you if I die in an aircraft accident.
 

Attachments

  • WS2_5stress Stress Analysis Report 6_3_2014.pdf
    72.5 KB · Views: 397
  • CopyWS 2_5 SparA.pdf
    14.9 KB · Views: 308

Matt G.

Well-Known Member
Joined
Nov 16, 2011
Messages
1,271
Location
Kansas, USA
Can you explain "pin constraints of the same diameter"? Constraints in a finite element model are dimensionless and refer only to the degrees of freedom at the node(s) that are being constrained. You don't appear to be applying a shear load to the FEM. How are you modeling the attachment between the spar fittings and spar caps? How about the spar cap to web attachment? What mesh density are you using? The way the mesh density is defined in the output, it is really difficult to tell.

If you want to even approach realistic stresses in your spar, you need to apply more realistic loads. The only thing I'd expect to get remotely close to reality with a concentrated moment representing the wing loading would be reactions at the wing attach pins. Everything else is going to be garbage. Stresses will be unrealistic near the load application point. You need to use a distributed load on the spar such that the shear and moment at your analysis location are consistent for both the FEM and spreadsheet.
 

Topaz

Super Moderator
Staff member
Joined
Jul 29, 2005
Messages
14,942
Location
Orange County, California
...You need to use a distributed load on the spar such that the shear and moment at your analysis location are consistent for both the FEM and spreadsheet.

And that load needs to be representative - spanwise and chordwise - of the actual load imposed by the wing at various critical parts of the flight envelope, including cases for flap and aileron deflection, which alter the load distribution significantly.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Can you explain "pin constraints of the same diameter"? Constraints in a finite element model are dimensionless and refer only to the degrees of freedom at the node(s) that are being constrained. You don't appear to be applying a shear load to the FEM. How are you modeling the attachment between the spar fittings and spar caps? How about the spar cap to web attachment? What mesh density are you using? The way the mesh density is defined in the output, it is really difficult to tell.

If you want to even approach realistic stresses in your spar, you need to apply more realistic loads. The only thing I'd expect to get remotely close to reality with a concentrated moment representing the wing loading would be reactions at the wing attach pins. Everything else is going to be garbage. Stresses will be unrealistic near the load application point. You need to use a distributed load on the spar such that the shear and moment at your analysis location are consistent for both the FEM and spreadsheet.

Well we have this spread sheet that checks the loads at a target location. I am comparing the spread sheet results with the FEA. The Model needs to be constrained, which becomes a problem to me as the constraints interfere with the result and I do not know how to apply them to check the target location. The only constraints that made sense were the attach pins at the root. The Carbon Dragon which I am trying to convert on paper had these fittings and bolt diameters. The spread sheet calls out for a moment at the target location and that Wing Station 2.5 is all that I am looking at to compare to the spread sheet. Shear is a question of mine, as to if the load at that location is correct, then does that include the "shear resistant web"? The mesh density is noted in the report, and was automatic and seamless by my program. The attachments of the fittings and all the caps were one of my questions, again I modeled it as "bonded" in my program but wonder if I should model the rivets and bolts. I was having problems with the program separating the various parts so this test is an extrusion with only the fittings bonded to the caps. As far as I know the bending load (moment) is realistic at that location (WS 2.5) , but that is why I posted. The stresses and safety factor at that location shows up good in the spread sheet and the FEA. There is a slight overstress at the bottom bolt hole, which is not the target location.
 

Matt G.

Well-Known Member
Joined
Nov 16, 2011
Messages
1,271
Location
Kansas, USA
Well we have this spread sheet that checks the loads at a target location. I am comparing the spread sheet results with the FEA. The Model needs to be constrained, which becomes a problem to me as the constraints interfere with the result and I do not know how to apply them to check the target location. The only constraints that made sense were the attach pins at the root.

Constrain the model at the fittings, using constraints representative of how the spar interfaces with the part it connects to. This is completely independent of what location you are trying to check. Then, as Topaz alludes to, apply a realistic load distribution. Use the methods in Peery, Bruhn, Hiscocks, etc. to develop the external loads applied to the spar. Apply those in the FEM and to do a hand analysis of a cantilever beam, the latter of which will give you the shear and moment to plug into the spreadsheet. Then you can compare stresses at whatever location you want. The applied external loads need to be the same for both analyses so that the internal shear and moment needed for the spreadsheet correspond to the internal loads in the FEM.

The spread sheet calls out for a moment at the target location and that Wing Station 2.5 is all that I am looking at to compare to the spread sheet.

The load in the spreadsheet is an internal load at a section cut at the analysis location of interest.

Shear is a question of mine, as to if the load at that location is correct, then does that include the "shear resistant web"?

Does what "include the shear resistant web"? Not sure what you mean here.

The mesh density is noted in the report, and was automatic and seamless by my program.

This is precisely the reason why the built-in FEA tools in CAD software are only used in industry for making pretty pictures and not real analysis. The accuracy of the results depends on mesh density, among MANY other things. If you can't control that, you have lower chance of success.

The attachments of the fittings and all the caps were one of my questions, again I modeled it as "bonded" in my program but wonder if I should model the rivets and bolts.

Well, if the actual structure isn't bonded, you're going to get a different stress distribution than if it were riveted. If you want something quick and dirty, you can model the rivets with rigid body elements, but I'm guessing that the FEA you are using is too automated to allow you to do something like that.

As far as I know the bending load (moment) is realistic at that location (WS 2.5) , but that is why I posted. The stresses and safety factor at that location shows up good in the spread sheet and the FEA. There is a slight overstress at the bottom bolt hole, which is not the target location.

The moment used in the spreadsheet is an internal load. You cannot apply it as an external load to the FEM. This is not even remotely the same thing. Honestly, you're scaring me when you say "stresses and safety factor at that location shows up good in the ... FEA." It is not modeled well enough to come to that conclusion. You are comparing Von Mises stress (and to quote a more experienced stress engineer at work- "Von Mises is a failure theory, no one ever said it was a good failure theory") to stresses in the spar caps and shear web that are with respect to a certain direction. You need to select directional stress outputs, i.e. fx, fy, fz, etc. in the same direction as the stresses computed by the spreadsheet.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Does what "include the shear resistant web"? Not sure what you mean here.

Sheet 2 of the spread sheet has "shear resistant web" results with only the inputs shown. I am not sure the shear input of line 25 is correct, that number comes from line 2. that is one reason I am also learning/using FEA. It certainly would be nice to have 30 or 40 years of aircraft stress experience,.....I do not.

This is precisely the reason why the built-in FEA tools in CAD software are only used in industry for making pretty pictures and not real analysis. The accuracy of the results depends on mesh density, among MANY other things. If you can't control that, you have lower chance of success.

there are inputs for mesh size what mesh size do you recommend. The size of the spar is an input, the caps are approx 1/6 spar height and also an input in the spread sheet.

Well, if the actual structure isn't bonded, you're going to get a different stress distribution than if it were riveted. If you want something quick and dirty, you can model the rivets with rigid body elements, but I'm guessing that the FEA you are using is too automated to allow you to do something like that.

I read and saw video that said to simplify the model, Do you really model every rivet? I can do tests to see the difference, after I learn to model a riveted structure.

The moment used in the spreadsheet is an internal load. You cannot apply it as an external load to the FEM. This is not even remotely the same thing. Honestly, you're scaring me when you say "stresses and safety factor at that location shows up good in the ... FEA." It is not modeled well enough to come to that conclusion. You are comparing Von Mises stress (and to quote a more experienced stress engineer at work- "Von Mises is a failure theory, no one ever said it was a good failure theory") to stresses in the spar caps and shear web that are with respect to a certain direction. You need to select directional stress outputs, i.e. fx, fy, fz, etc. in the same direction as the stresses computed by the spreadsheet.

The loads are lines 1-6 of the spread sheet,..the fittings are actual fittings for the spar however the web is missing from WS 2.5 to WS 0, the spar joins at WS 0. The moment was located at the edge/inboard face of the spar web/caps extrusion at station WS 2.5. It is internal, and is the same moment from the spread sheet, as to weather that is a proper way to do this,....well that is another matter. My program will give other outputs I only mounted those two. I used the probe to check actual numbers at WS 2.5

In the last 4 weeks spending approximately 60 hours with the FEA program, this is the first output that I considered reasonable results with a simple understandable model. It is a first-cut, and in no way a reasonable "bet your life" model.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
I have used the Cell M23 number for the moment, 109134 in-lb. It is located on the face with the prob labels, and I believe it is internal at that location. The prob labels show Von-Mises at given locations. I would like to understand how this plot relates to the EAA spread sheet shown and why if possible it is not exactly the same results. I would like to ask if this is a reasonable graphical check of the EAA spread sheet. The numbers are less than what the Spread sheet shows, but one might say "in the ball park"
 

Attachments

  • WS2_5stress.jpg
    WS2_5stress.jpg
    34.7 KB · Views: 213
  • WS 2_5 SparA.pdf
    20 KB · Views: 170
  • WS2_5astress.jpg
    WS2_5astress.jpg
    26.9 KB · Views: 261
Last edited:

Monty

Well-Known Member
Joined
Jul 15, 2010
Messages
1,365
Location
Fayetteville, AR / USA
The reason for the different results is you have not applied the same loading. A moment can be placed anywhere on the structure. It is the product of a force and distance. The wing sees a distributed load. Which may be integrated to yield a force at the centroid of the distributed load. If you try to use just a moment, you are missing this info. You need to study and understand this. Start with the Schrenk approximation. You need to work through a shear moment diagram using a hand calculation BEFORE using either the spread sheet, or FEA.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Start with the Schrenk approximation. You need to work through a shear moment diagram using a hand calculation BEFORE using either the spread sheet, or FEA.

I have used the flat platform method as it is easier to understand and more conservative. My numbers for shear and moment came from there. I can mount the graphical calculations but they are summarized on Rows 1-6 of the spread sheet.
 

Monty

Well-Known Member
Joined
Jul 15, 2010
Messages
1,365
Location
Fayetteville, AR / USA
I have used the flat platform method as it is easier to understand and more conservative. My numbers for shear and moment came from there. I can mount the graphical calculations but they are summarized on Rows 1-6 of the spread sheet.

I guess I'm having a hard time understanding what you are trying to accomplish with this analysis. Using shear and moment only is not going to give you any meaningful result other than to size the bolted connection. In that case as discussed in other threads, there is no point in using FEA. If you are trying to analyze the spar itself, you must use a properly distributed load, as others have already pointed out above.

The limiting condition in the bolted connection is almost always the bearing load on the aluminum, or tear out in the aluminum. All of this is very easy to calculate with pencil and paper. FEA is not useful or required for this. If you are trying to analyze the spar, you fix the bolted connections and apply the distributed load. Ignore the high stress around the bolt holes, because it is not real. The reaction forces should match hand calculations or something is very wrong.
 

Monty

Well-Known Member
Joined
Jul 15, 2010
Messages
1,365
Location
Fayetteville, AR / USA
I have used the Cell M23 number for the moment, 109134 in-lb. It is located on the face with the prob labels, and I believe it is internal at that location. The prob labels show Von-Mises at given locations. I would like to understand how this plot relates to the EAA spread sheet shown and why if possible it is not exactly the same results. I would like to ask if this is a reasonable graphical check of the EAA spread sheet. The numbers are less than what the Spread sheet shows, but one might say "in the ball park"

Also looking at your FEA result, it appears that you have not constrained the bolt holes properly. Top should be in compression, bottom in tension. Only one half of the hole is seeing a bearing load, and they should be opposite each other.
 

wsimpso1

Super Moderator
Staff member
Joined
Oct 18, 2003
Messages
9,293
Location
Saline Michigan
I looked over your FEA. You told it to hold the wing steady, then applied a moment to wing root. This is not anything like what the real thing does. This means the model output does not reflect what the real stresses will be. Let’s look at what the real thing does.

Spars – The main spar carries the shear and bending moments that result from applying aeroload over the half-span of the wing and restraining the root of the wing. For FEA, you do the same thing.

First off, the spanwise lift distribution along the wing is approximately an ellipse, with the load (in lbs/in) being virtually zero at the tip and increasing as you go to the root. The shape of the distribution is because the high pressure air on the bottom of the wing “leaks” around the wingtip to the low pressure air on the top, reducing the difference in pressure more and more as you approach the tip. The Schrenk approximation is pretty good, and easier to work with than a purely elliptical distribution.

Next, the spar accumulates loads from this spanwise lift distribution. At any point along the wing, the total lift outboard of that point is the shear load in the spar. This number is bigger than the lift distribution. You can calculate it by integrating the spanwise lift distribution over the length outboard of the point in question. Integration is a fancy word for adding up area under the curve. In this case, for each increment along the spar, starting at the tip, you multiply the lift on that increment by the spanwise increment and add up the total lift outboard of the point. While the lift distribution is small, the shear will be equal to the lift of the wing at the root. You can find all of this beam theory in Mechanics of Materials by Timoshenko and Gere.

Next is the bending moment on that spar. Now we add up not the lift, but the product of the lift times the distance from the point in question. This number gets bigger than the shear…

Now, in FEA, you just get the spanwise lift distribution applied to the spar, constrain the two holes where the pins go to allow zero translation, but be unconstrained in rotation. That is what putting a bolt through each of those holes and into a fixed structure on the airplane does to it. Now when you let it run, FEA takes care of distributing loads among the many elements, and you do not need to calculate the moments, etc. In fact, if you get the constraints right and the spanwise loading right, it will compute the total loads in the pinned joints.

But I can tell you something. Compute moments correctly at the root, divide by the distance between your pins, and that is the horizontal load at each pin. In positive g flight, the top one is pushing towards the wing while the bottom one is pulling on the wing. Next, if you compute the shear correctly, and divide it by two, you will have the vertical load on each pin. Do the vector sum at each pin to get the total pin load, and you can check the shear load on the pin, the bearing stresses in the pin holes, etc.

Not only that, but if you have the bending moments and shear loads, you can use nice simple equations right out of the chapter in Mechanics of Materials on beam theory to compute your stresses in the caps and in the shear web. No FEA needed. MOM even tells you how to compute the loads in the rivets.

You do need to understand how FEA works before you can use it for much. In the meanwhile, you do need to understand the basics of how the loads develop and how they produce stress in the parts. That means study of some beam theory. Once you can do that, for a beam this simple, you really do not need to do FEA...
 

Topaz

Super Moderator
Staff member
Joined
Jul 29, 2005
Messages
14,942
Location
Orange County, California
Propastie, please consider the excellent advice being given by Monty and Wsimpso1 in posts #10 and #12. If your goal is explicitly to learn FEA, then by all means, do so. If your goal is to design an airplane, the traditional methods are more than adequate and can be implemented with a spreadsheet and some manual-calc checking. You'll get the job done faster and - ironically - probably more accurately than trying to dive into FEA.

Using a realistic lift distribution on the wing is going to be vital to your work. It cannot be simplified out to a simple point or evenly-distributed load. Schrenk's Approximation for lift distribution can be done in twenty minutes with pencil and paper; doing it in Excel allows you to change parameters and recalculate almost instantly. If the least bit of care is taken in the development of a spreadsheet implementation, you can also get the spanwise values of torque due to pitching moment, and can easily run cases with flaps and ailerons in various deflections.

Tie this into the types of calculations (implemented in the same spreadsheet) that Billski is talking about, and you can get a comprehensive load-case development for the entire wing structure, at as many stations along the span as you want.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Also looking at your FEA result, it appears that you have not constrained the bolt holes properly. Top should be in compression, bottom in tension. Only one half of the hole is seeing a bearing load, and they should be opposite each other.

yes, I used pin constraints on the holes, there is a screw up somewhere
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Not only that, but if you have the bending moments and shear loads, you can use nice simple equations right out of the chapter in Mechanics of Materials on beam theory to compute your stresses in the caps and in the shear web. No FEA needed. MOM even tells you how to compute the loads in the rivets.

You do need to understand how FEA works before you can use it for much. In the meanwhile, you do need to understand the basics of how the loads develop and how they produce stress in the parts. That means study of some beam theory. Once you can do that, for a beam this simple, you really do not need to do FEA...

I have not studied that book, but the ones I have studied, did not explain the shear resistant web with lightening holes leastwise simple beam theory.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
Propastie, please consider the excellent advice being given by Monty and Wsimpso1 in posts #10 and #12. If your goal is explicitly to learn FEA, then by all means, do so. If your goal is to design an airplane, the traditional methods are more than adequate and can be implemented with a spreadsheet and some manual-calc checking. You'll get the job done faster and - ironically - probably more accurately than trying to dive into FEA.

Using a realistic lift distribution on the wing is going to be vital to your work. It cannot be simplified out to a simple point or evenly-distributed load. Schrenk's Approximation for lift distribution can be done in twenty minutes with pencil and paper; doing it in Excel allows you to change parameters and recalculate almost instantly. If the least bit of care is taken in the development of a spreadsheet implementation, you can also get the spanwise values of torque due to pitching moment, and can easily run cases with flaps and ailerons in various deflections.

Tie this into the types of calculations (implemented in the same spreadsheet) that Billski is talking about, and you can get a comprehensive load-case development for the entire wing structure, at as many stations along the span as you want.


I do not want to be ungrateful or foolish or stupid and pig-headed, but it seems many (not all) what to tell me how they do it rather than help me do it the way I want to do it. I am attempting to understand this in a way that makes sense to me and is understandable to me. If I am flat wrong in my assumptions inputs or results ....just say thats wrong such as post 11. I know it is unreasonable for you to check my numbers, I promise not to sue you.
 

Topaz

Super Moderator
Staff member
Joined
Jul 29, 2005
Messages
14,942
Location
Orange County, California
I do not want to be ungrateful or foolish or stupid and pig-headed, but it seems many (not all) what to tell me how they do it rather than help me do it the way I want to do it. I am attempting to understand this in a way that makes sense to me and is understandable to me. If I am flat wrong in my assumptions inputs or results ....just say thats wrong such as post 11. I know it is unreasonable for you to check my numbers, I promise not to sue you.

I can't help you then. I think everyone here has been very clear. I don't know what else to say.
 

autoreply

Super Moderator
Staff member
Joined
Jul 7, 2009
Messages
10,792
Location
Rotterdam, Netherlands
I do not want to be ungrateful or foolish or stupid and pig-headed, but it seems many (not all) what to tell me how they do it rather than help me do it the way I want to do it. I am attempting to understand this in a way that makes sense to me and is understandable to me. If I am flat wrong in my assumptions inputs or results ....just say thats wrong such as post 11. I know it is unreasonable for you to check my numbers, I promise not to sue you.
If we looked at the highlighted part, what could the other explanation be?


This is one of those topics where how many people think about CAD/CFD/FEM and how it really is have a slightly violent, not always pleasant collision.

A friend of mine is doing a PhD in what is essentially CFD, but equally true for FEA. Also one of the most outspoken voices to do everything by hand/Excel/Java/Matlab.
 

proppastie

Well-Known Member
Joined
Feb 19, 2012
Messages
5,743
Location
NJ
If we looked at the highlighted part, what could the other explanation be?


This is one of those topics where how many people think about CAD/CFD/FEM and how it really is have a slightly violent, not always pleasant collision.

A friend of mine is doing a PhD in what is essentially CFD, but equally true for FEA. Also one of the most outspoken voices to do everything by hand/Excel/Java/Matlab.

Somewhat cryptic here, I try to be more straightforward, like "its wrong, your input or constraint is wrong" "should be xxxx" I would love to have complete confidence in my hand calculations, but I do not. This is not a trivial subject.
 

Topaz

Super Moderator
Staff member
Joined
Jul 29, 2005
Messages
14,942
Location
Orange County, California
... I would love to have complete confidence in my hand calculations, but I do not. This is not a trivial subject.

Well, since you're asking for "direct"...

I think this post above is pointing out the actual problem. You don't have confidence in your ability to do this by hand, or calculator, or Excel, but somehow you think "computer FEA" will remove that perceived risk. What I, Autoreply, Monty, Wsimpso1, and the others are telling you is that this not true.

For you to even have a hope of using FEA properly, you're going to need to be comfortable and knowledgeable with the traditional methods - in that those methods contain more-explicit approaches to the problem that avoid some of the mis-use that FEA allows without complaint. Using a computer to do structural analysis isn't safer or better; it's more efficient for a structural expert working in a high-end, profit-oriented design situation. If you were working on the next Boeing wide-body, yes, computer FEA would be a virtual necessity to complete that work in a modern, shortened design cycle for a design-cost investment that will help the company achieve a profit from producing the aircraft. Incredibly good tool for that, especially if you're working at the bleeding edge of structural and weight-reduction technology and methods.

For a homebuilder, you have to learn the good design and analysis techniques that are the foundation of any "safe" structural analysis, be it traditional or FEA. Without that, you'll be making mistakes from which FEA can't "save" you - the computer will happily swallow the error in methodology and give you "an answer" that may not bear the slightest resemblance to reality. You're seeing some of that with your example here.

Since you have to learn good structural analysis methodology anyway - and that's generally taught using the traditional, "by hand" methods so that reasons for the methodology are abundantly clear - why layer another mass of learning on top of that which is already perfectly adequate for the design of almost any airplane we can actually build in our garages? It's more work that just keeps you away from actually building the airplane.

I fully and completely understand the insecurity that goes with trying to learn something as complex as structural design - I'm in the process of launching into that sea of knowledge myself! I look at the next chapter ahead in Bruhn (whichever chapter that might be) and shake my head in frustration sometimes. But the answer to insecurity is learning what you're doing so that you can do it right, not simply tossing the issue at a machine to somehow "do it better" for you.

Believe me, we're all pulling for you here. Nobody think's you're "ungrateful or foolish or stupid and pig-headed." We're just trying to give you the answer we think you need, rather than what you think you want.

Fair enough?
 
Top