safety factor in FEA behaving opposite to how it should?

[Anonymous]

Hi All,

I carried out a parametric FEA analysis on a tube from a dynamic simulation. I changed the outer diameter of the tube but as I make it thinner the safety factor displayed (using 'Min Safety Factor' as a design constraint in the parametric table) increases and the Max Von Mises stress decreases, but it should be the other way around, more material means that it should be stronger so a higher safety factor. I have no idea what might be wrong, this makes no sense to me.

Even if the loads would be wrong in case I did the D.S. wrong, the tube would still be subjected to loadings, so it should have a lower safety factor with a thinner thickness. 

Any thoughts?

[JDMather]

Is this a long slender part?

Could it be bending easier because of less material?

If you sign up for this class

https://events.au.autodesk.com/connect/sessionDetail.ww?SESSION_ID=6583

I will be demonstrating a parametric analysis that exhibits exactly the behavior you describe and is the desired behavior that will be the goal of the exercise.  (A given amout of force - in this case thumb pressure - to release a latch by moving a specific displacement.)

[Anonymous]

HI JDMather,

The tube is 1m long and 3.5cm diameter, 0.02cm thickness, made of aluminum, connected between a gear and a propeller. You're right it probably can bend easier because of less material, but it doesn't convince me that a tube that thin can stand the forces involved in rotating the propeller powered by the gear.
If I keep decreasing the thickness of this tube, should I reach a point at which the tube would have a lower SF?
I'll definitely look into that class, thanks for the notice.

[swalton]

Two things come to mind.

Have you done a hand calculation to verify your FEA?  You should be able to make some assumptions to get a basic idea of your expected stresses.

Did you really mean your tube has a wall thickness of 0.02 cm (0.008 inches)?  That seems wrong. 

[Anonymous]

Hey swalton,

you're right, my bad. The thicknes is 2 mm (0.2 cm).

I will try to do the hand calculations. One thing I notices is that as I made the thickness even smaller eventually the SF started to drop, which would mean that tube would be really weak and not that flexible anymore.

[JDMather]

---

@swalton wrote:

Two things come to mind.

Have you done a hand calculation to verify your FEA? 

---

I have never figured out how a hand calculation is any faster than a computer model - can you post an example?

Is there some secret formula that the computer programmers don't know about?

[swalton]

My intent is to "sanity check" theFEA results.  If the OP does not agree with the FEA results, how else is he/she to check them?  Hand calcs are cheaper than strain gages.

The OP could also use the shaft design tools in IV.

It is true that a quick hand calc will not give the entire stress field on the part, but it can be a place to start the validation of the FEA.

If the OP knows the required torque or power carried by this shaft, he/she can get a quick idea of the stress to expect in the shaft.  If necessary, overhung loads and bearing reactions can be added too.  Heck, put the calc in a spread sheet and save it for future use. 

Once that is done, then the user can start applying constraints, loads, and meshes to have greater confidence that the stress predictions from the FEA are more than fancy colors.

[JDMather]

---

@swalton wrote:

... how else is he/she to check them?  ....

.... start the validation of the FEA.

.....greater confidence ....

---

For several years and on several forums I have been asking for someone to please post an example.

Nobody ever has provided me with an example.

I have my students do hand calcs of several of the trivial different examples from the Machinery's Handbook.  But how does that validate FEA?   How does that equate to greater confidence? 

After the hand calcs we start out with the Beam and Column Design Accelerator (no geometry and then selected geometry), then Frame Generator, then FEA solids then FEA thin features and verify that all give essentially the same results.  But how does this verify, validate, whatever the software solution?  Are we saying we don't trust the software developers?  Or are we saying we don't trust our setup of the software solution?  Are we saying we trust hand calcs over all else?

Until someone convinces me otherwise - I am convinced the ubiquitous, response, "Did you do your hand calcs?" is nothing more than rote repetition by everyone who has had to do the hand calcs. The only defense is a historical one, not a technological one.   Have you ever seen the results from significant numbers of student hand calcs?  (I need a sanity check myself after such an exercise.)

[JDMather]

---

@Anonymous wrote:
HI JDMather,

The tube is 1m long .....

---

From your assembly there was no support for the tube at the prop end.  Why do you need a 1m length with no support?

[raviburla]

Hi,

I tried a similar model as yours (len = 1.0 m, dia = 3.5 cm, thickness = 0.2 cm). Since, I don’t have the loadings that you are using, I have applied a bending load that would be “similar” to loads coming from DS export.

There are few things I would like to mention with respect to load transfer from DS.

1.        There will be no constraints.
2.        The loads are all-balanced. This means that Sum of all forces and moments acting on the body equate to zero.
3.        In FEA engine, a special mode  to eliminate rigid body modes is enabled by default for these solves. This ensures that the rigid body modes are removed automatically and a solution corresponding to balanced loads is provided.

I am attaching the model here. I set up a  parametric simulation with parameter as the wall-thickness [1.5, 1.75, 2.0, 2.25, 2.50]mm . Also, I have modified the mesh density to 0.01 to ensure that proper geometry/solution is captured. I applied opposing moments on two ends of the pipe, so that we have a balanced loading condition. Here is the summary of my results

1.5 mm thick -> Stress = 0.7975 MPa

1.75 mm thick -> Stress = 0.7068 MPa

2.0 mm thick -> Stress = 0.6215 MPa

2.25 mm thick -> Stress = 0.5646 MPa

2.5 mm thick -> Stress = 0.522 MPa

As we can see the stress increases with decreasing thickness which is in line with expectations. Can you try using a finer mesh on your model to see if you see the expected solution. You can also post your model  and we can take a look into the model to understand any model-specific issues. Please let us know if you have questions/comments.

Thanks,

Ravi Burla (Autodesk)

[Anonymous]

This structure will be used for a paraglider and the 1m length is needed to provide some distance between the body of the paraglider and the propeller, otherwise the propeller would hit the body or be too close to the pilot. I've thought of this before but I want to see if it would work enough without a support first.

[Anonymous]

Hi raviburla,

Thanks so much for that. That is the behavior I expected but I'm not seeing that. I attached my model there, the full assembly is called

'Assembly2,2 v1'. 

Now I'm seeing a weirder behavior because the SF alternates between less than 1 and above 5 as I increase the tube's thickness by 0.05cm (you'll see in the parametric table). I can't attach the simulation files because it's too big so let me know what results you get and if a pop out window comes out asking for missing reference documents just click 'open' because they are probably old simulation files.

Also when you see the reactions it looks like a mess but the thing is that there are 6 fastaners so that is where they all come from.

Let me know if you have any doubts. I've been learning Dynamic Simulation through the community here so I hope that my setup is not too bad, but definetely not perfect I would say.

Thanks again

[raviburla · Accepted solution]

Hi,

Thanks for the dataset. I looked into it in detail and made some changes to the simulation:

1. Copied the Simulation and made changes to the copied one.

2. Suppressed the constraint and the loads from DS should be in balance already.

3. Removed the local mesh control.

4. Changed the mesh density.

One of the things I observed is that the min-SF (max-Stress) are corresponding to a point with spurious stresses. The reason FEA solution leads to spurious stresses is due to certain singularities in the FEA Model. The singularities could be due to sharp corners, due to a boundary conditions, or other issues. As FEA users, we have to understand the spurious stresses and carefully interpret them.

Keeping the singularity in mind, I have modified the color bar property so that the max stress is limited to 15 MPa and plotted the stresses for all configurations. As we can see the stress behavior is in accordance to expectations - the stress decreases with increasing thickness. I am also attaching the models and stress plots. I hope this answers your questions. Please let us know if you have more questions/comments.

Thanks,
Ravi Burla (Autodesk)

[Anonymous]

Hi Ravi,

Sorry for the late response. Thank you so much for your help, things make more sense now (still a couple of months later). Now I only have two questions.

1. In order to explore whether these spurious stresses actually mean something I'm assuming you do a mesh sensitivity analysis, is there such tool in the FEA module? I tried playing around with convergence but I'm not really sure how to use it.

2. The base of the shaft looks like it detaches from the main gear once the simulation is complete. Is there any way to enforce the fixed constraint so that the result looks more like a "bending cantilever beam" rather than what is shown right now:

thank you,

Nestor

[raviburla]

Hi Nestor,

What you are seeing  the side effect of solving a system with balanced loads. Basically, since there are no constraints, the solution obtained from a system with balanced loads is unique for stresses, but not for displacements. Lets say that "d" is the solution for this problem, then any solution of the form "d+ r" is also a solution, where "r" is a rigid body displacement. Rigid body displacement of the entire body does not induce stresses. Inventor simulation provides one of these solution, currently its not possible to show the solution that you are requesting. But please note that the stress solution is still correct. Hope this helps.

Thanks,
Ravi Burla