FEA analysis stress value not correct

[Anonymous]

Hi,

I have some issues with the stress analysis. I have attached two picture files. One is with support and another without support. All the setttings for stress analysis are made already. All the factors are same for both files. You can just simulate directly.

Practically stress must be less in the case which has supprot while here in the software its opposite. When I add support, stress increases which is not quite promising.

thanks,

Manish

[Anonymous]

---

@Anonymous wrote:

But in inventor displacement is quite low, around 0.2 mm. Not matching with actual results.

---

You have to remember that most FEA computations assume an _elastic_ deformation of the part or assembly; therefore, once your stress/strain exceeds the yield strength, the analysis will _not_ necessarily represent the real world results.

Inventor's calculated displacement of 0.2mm is the deformation which would occur while the part is under load.  If the real world part permanently deformed 2mm, it clearly indicates that it did indeed enter the plastic elongation region of the material -- as soon as the yield strength of the material was exceeded, the geometry of the part would permanently change to reduce the loading (and changing the zone of the most highly stressed material).

If the geometry has changed significantly enough (due to plastic deformation), it is possible that your 2.5 times loading would induce stresses/strains that remains below the material's yield strength.

HTH

[JDMather]

---

@Anonymous wrote:

can you please check what stress you get with this part.

---

I do not see a file attachment of the part?

Find the red End of Part marker in the browser.
(End of Folded on sheet metal parts EOF)
Drag the red EOP to the top of the browser hiding all features.

Save the file with the EOP in a rolled up state.

Right click on the file name and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here.

It would also be useful to see the part in it's actual in-use position and in the testing position which you refer to.

(When we simplify constraints for simulation - sometimes we are changing the way the forces actually act on the part.  The key is to get a (simplified or not) digital simulation to match the analog world, then we can use for predictive purposes.)

[Anonymous]

hi Please check this file.

[Anonymous]

Hi,

can you please check this.

[Anonymous]

Hi,

Attached in are the files and pictures required.

Yield strength: 330 MPa

Tensile Strength: 520 MPa

Force: 405340 N

Problem:

1. Inventor (even some other FEA softwares, not specifically inventor) results and actual results don't relate each other.

Using more finer mesh, more stress is developed, meaning it will fail but thats not the case in reality.

2. Adding ribs or supports must reduce stress and increase safety factor but the stress increases. For customer, high stress and low S.F means it will break faster or something in that part will crack faster at lower force.

3. Adding fillets and stress reducers increase the stress in software(very strange)

Inventor lacks in fillets and creating smooth surfaces. ecspecially in very complex curves.

If you have any solutions please help

[Anonymous]

This is for reference, our test modal.

[JDMather]

1,2 & 3

I recommend that you take a class on FEA.

These statements indicate to me that you do not have a good understanding of FEA.

[JDMather]

---

@Anonymous wrote:

hi Please check this file.

---

Before I even begin to run any anaylsis on this part I will have to remodel it correctly from scratch.
I am sure I will then have a lot of questions about how the forces and constraints (particularly the constraint(s) are really applied on real world part.

It might take me a while to get back to this problem since I have to recreate the model from scratch.

[Anonymous]

---

@Anonymous wrote:

2. Adding ribs or supports must reduce stress and increase safety factor but the stress increases. For customer, high stress and low S.F means it will break faster or something in that part will crack faster at lower force.

---

Take a look again at your first example:

If you look only at the magnitude, it does appear that the model with the rib has the higher stress loading at 15.83MPa while the original has only a stress of 13.88MPa.

However, when you look _at the location_ too, the stress in the corners of the first model due to the loading is 13.88MPa (red) and has been reduced to somewhere near 9.56MPa (lime green) in the revised design with the rib.

I suspect that if you change the thickness of the rib, you can reduce the overall stress in the second design to be at or below that of the original; furthermore, you can probably reduce the stress in the corners even more by adding fillets.

As JDMather stated, FEA is a tool and, like any tool, you have to understand both how to utilize it and how to interpret the results that it provides.

HTH

[blair]

One of the problems with going to a finer/smaller mesh is the introduction of stress-risers. This is common through out all FEA software. You really need to be able to interpret the results you are getting.

[Anonymous]

May be you can use the files uploaded in meassage 25 and 26.

Lets wait for your analysis results.

And Please note I have applied 40 tons of force in the software.

In reality we ended up applying 320 tons of force still there was no breakage. We reached the maximum capacity of cylinders, but nothing could break that part.

[JDMather]

---

@Anonymous wrote:
 

1. Inventor (even some other FEA softwares, not specifically inventor) results and actual results don't relate each other.

Using more finer mesh, more stress is developed, meaning it will fail but thats not the case in reality.

---

1. No.  Higher calculated stress does not mean failure of the part.

You will want to get your digital model to correlate to your physical testing - but I do not see any strain gauges in the images you attached.  The dial indicators should be located closer to the ends and you have not indicated their readings (at particular loads).

Inventor does not calculate fracture.  It returns S(y)/S(calc).  A part can be bent beyond S(y) intentionally to strengthed the part (work harden).

For example, this bracket is bent beyond S(y) with the intention that it remain in its deformed shape rather than return to original shape.

Same for this sheet metal hitch part.

The metal has been deformed very significantly beyond S(y) yet has not fractured (failed).

and

Inventor analysis is limited to anisotropic materials, where the material properties of these parts would now be isotropic.

[JDMather]

---

manish wrote:

2. Adding ribs or supports must reduce stress and increase safety factor but the stress increases. For customer, high stress and low S.F means it will break faster or something in that part will crack faster at lower force.

---

No.  In the first simple part you posted you added a rib that reduced Displacement, not stress. You added a relatively "weak" feature at a location that does in fact reduce displacement but now if the part does fail - that is where it will fail first.  It makes logical sense that the stress is higher on this feature.

If you did failure testing on this part you would see that in fact, that is were it would fail (but remember - Inventor does not do francture analysis anyhow).

The thin rib you added to your second part doesn't really make sense to me IF your goal was to reduce Displacement in that long rectangular feature that you welded onto the original part.

It is difficult to expect the customer to interpret an advanced topic like FEA analysis if the person who is doing the analysis doesn't understand how to interpret the results. 

You could have a localized stress riser or singularity that is simply a result of the meshing method but is of no practical concern.

You could have a localized high stress area that will in fact result in permanent deformation on the real world part, but again, is of no practical concern in the functional use of the part.

[JDMather]

---

@Anonymous wrote:

3. Adding fillets and stress reducers increase the stress in software(very strange)

---

3. No.  Not strange if you have studied how digital analysis is done.
For a general discussion, I like the book Building Better Products with Finite Element Analysis by Vince Adams.

For Inventor specific FEA get the book by Wasim Younis.

But neither of these books really substitute for logic an practical experience.

The Younis book should show you how you can set up the analysis results such that unimportant (to the function of the part) areas can be handled such that the analysis results can be properly presented to the customer.  But again, you should have a clear understanding of exactly what you are doing with the digital model so that you are not simply creating pretty pictures that say what you want them to say.

[Anonymous]

Safety factor is measured with Yield strength/stress. No one is interested in what will happend after yield strength. No one designs or sells anything based on tensite strength. At least not in our branch (heavy structures/shipbuilding/mining)

From our hand calculations and from our extensive testing that we did over and over again we are getting much higher results than simulated by Inventor.

Also field test results prove the safety factor is much higher than expeted with Inventor.

Why do we have Inventor? or any other FEA analysis if SF of the simulation is much lower than tested and hand calculated.

HOW TO CALCULATE THE SAFETY FACTOR? (of course based on YIELD only)  

[Anonymous]

---

@Anonymous wrote:

---

@Anonymous wrote:

3. Adding fillets and stress reducers increase the stress in software(very strange)

---

3. No.  Not strange if you have studied how digital analysis is done.
For a general discussion, I like the book Building Better Products with Finite Element Analysis by Vince Adams.

For Inventor specific FEA get the book by Wasim Younis.

But neither of these books really substitute for logic an practical experience.

The Younis book should show you how you can set up the analysis results such that unimportant (to the function of the part) areas can be handled such that the analysis results can be properly presented to the customer.  But again, you should have a clear understanding of exactly what you are doing with the digital model so that you are not simply creating pretty pictures that say what you want them to say.

---

What are your simulation results?

Please interpret the results about the modal?

---

[Anonymous]

---

@Anonymous wrote:

What are your simulation results?

---

---

As I am not using Inventor 2014, I couldn't open your .ipt files; however, I did my best to recreate your part using the drawing/sketch you provided -- I must say that it left much to be desired as it was missing many dimensions.

Using the 880,000 N load and the fixed conical surfaces, my results were similar to yours; a resultant stress of approximately 317.7 MPa and a deflection of 0.446mm (for reference your values were 322.1 MPa stress and 0.411mm displacement).

However since the stress exceeds the yield of the steel material (~206.8 MPa), the FEA model does not reflect what would happen with the actual part under similar loading conditions.  I am curious how your FEA model indicates a Safety Factor of 0.97 Min when the material yield strength is 207MPa; did you accidentally use 307MPa in your original model as 207/322 = 0.64 not 0.97.

- - - - -

As for the differences observed when using different mesh sizes for the FEA model, they are expected ... a coarse mesh allows for a faster computation of the stresses and deflections; however, it also means that the values aren't necessarily as accurate since each node in the FEA model influences the other nodes around it.  What the coarse mesh provides is a first order approximation of the magnitude of the stresses and deflections and approximately where the critical zones are.  With this information, the critical zones of the part could be redesigned to reduce the induced stress and deflection.

Once the design is finalized, finer meshes can be utilized in the FEA model to obtain a more accurate stress and deflection -- for your design, I used four different mesh sizes from 40mm (coarse) down to 5mm (fine) and while the stress value increased from 297MPa to 334MPa that only represents a 11% increase; the deflection on the other hand increased on 1.5%.  Note that with each reduction of mesh size the 'error' between it and the finest mesh model was significantly reduced.

Unless it is critical to have the highest accuracy for these stresses and deflections due to minimal design margins, a 10% difference in stress is generally acceptable as the material properties themselves will fluctuate.

HTH

[Anonymous]

---

@Anonymous wrote:

---

---

However since the stress exceeds the yield of the steel material (~206.8 MPa), the FEA model does not reflect what would happen with the actual part under similar loading conditions.  I am curious how your FEA model indicates a Safety Factor of 0.97 Min when the material yield strength is 207MPa; did you accidentally use 307MPa in your original model as 207/322 = 0.64 not 0.97.

---

As already mentioned in message no. 25, I changed the yield strenth to 330 MPa

and tensile strength: 520 MPa. I didn't use Inventor steel.

I got safety factor around 1.04 as far as I remember at that time. 

And I totally agree with you for the mesh settings. But still it doesn't solve the issue.

[Anonymous]

manish wrote:

As already mentioned in message no. 25, I changed the yield strenth to 330 MPa and tensile strength: 520 MPa. I didn't use Inventor steel.

Was that change made before you did the pictures of your analysis that you provided in message 19 or did you use a different yield strength for that analysis for the Safety Factor image seems inconsistent with either a material with 207MPa or 330MPa yield strength.  Regardless of that inconsistency, my analysis using SolidWorks provides a similar stress and displacement to yours using Inventor; the minor differences between them can be attributed to both the different modeling method of the parts and mesh size used in the analysis.

As for translating the FEA model results into a prediction of real world performance, you have to first verify that all the assumptions and parameters are valid.

1. Stresses remain within the Elastic/Linear deformation zone (i.e. below the Yield Strength of the material)

2. Material properties (i.e. Elastic Modulus and Yield Strength) used in the FEA model match the actual material

3. Loading conditions and magnitudes`

4. Part geometry

- - - - -

Remember that FEA is a design tool which can highlight critical regions of stress and/or deflection; this allows the engineer to optimize the part for the particular loading conditions.  However, it cannot predict how the part will perform outside of the elastic/linear stress region nor how much additional load is required for ultimate failure.  An excellent example of this would be subjecting a uniform shape under pure tension (i.e. a tensile test), we know that, in the real world, the part will critically fail once the loading exceeds the ultimate tensile strength of the material but an FEA model would only indicate that the stress exceeds the yield strength for the majority of the component’s length.

Trying to extrapolate results beyond the limitations of the analysis technique is meaningless.  If you require knowing exactly how much load can be applied before the part critically fails (i.e. breaks), then your only alternative may be to subject a series of parts to total destruction.

HTH

[rmerlob]

Manish,

I think the explanation in layman's terms that you need about the first model you posted is: you placed a rib in a location where it is in the position to "soak up" most of the force produced by that loading condition (center of the beam-like structure), that coupled with the fact that it is very thin, causes it to have a stress greater that what the sides have. As you can see, the sides did get a relief from this added support, problem is the added support cant handle what you are asking of it, therefore has higher stress.

EDIT: be aware inventor returns maximum stress and safety factor for the worst location on the part not for an average. talking in purely theoretical terms, the average stress did get lower by adding the reinforcement, is just that the stress that was relieved from the sides is now adding up in the center reinforcement.

I think those results have to do with the geometrical nature of the part, loading and reinforcement you have presented.

This behavior seems pretty logical to me.

As for the most complex part, Inventor Simulations arent in the position to predict part breakage as they are only valid for the elastic portion of the stress and strain curve, I've also done these kinds of real life tests and have concluded that you have to at least use Autodesk Simulation with a bilinear material model to come close to real life after yielding has occurred.

Regards,

RM