Does anyone have any experience with scaling modal results to get meaningful stress values for fatigue analysis? Right now, for vibration analysis I simply apply a static g-load and assume the load is fully reversed if no other pre-loads are present. I would like to add a little more fidelity to this process, but would like to avoid a full blown harmonic analysis. With the products I work with dampening is a big unknown, therefore IMO, if I'm guessing at the dampening, I'm guessing at the response. It seems like I should be able to scale the modal results using the reaction forces at the fixed support and a know g-load and mass.
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Scaled modal analysis? 3
- Thread starter Adubeng
- Start date
Pretty sure the answer is that you can't "scale" modal results. Modal results are frequencies and mode shapes. Stresses and reaction loads are meaningless, unless I'm misunderstanding your question.
As for damping, depending on the material with which you are working, there are some "rule of thumb" numbers for Rayleigh damping, if that applies.
What software are you using and can you give us a general idea of your application?
As for damping, depending on the material with which you are working, there are some "rule of thumb" numbers for Rayleigh damping, if that applies.
What software are you using and can you give us a general idea of your application?
- Thread starter
- #3
I realize that the stress and reaction load values are meaningless, but my thought is that these can be scaled to some meaningful value. It seems like you could scale displacement and then apply that scale factor to other values.
I am using ANSYS and the application is typically for small glass filled nylon pressure vessels for automotive applications.
I am using ANSYS and the application is typically for small glass filled nylon pressure vessels for automotive applications.
I think the main purpose of modal analysis is to get natural frequencies of structures. And then compare with the frequencies of dynamic loads to avoid resonance.
And the stress and displacement appear only if the frequencies of dynamic loads are close to the results of modal analysis, So it might be meaningless to scale the displacement or stress in most cases.
And the stress and displacement appear only if the frequencies of dynamic loads are close to the results of modal analysis, So it might be meaningless to scale the displacement or stress in most cases.
Boeing has a method for developing static-g loads from natural frequency calculations, but it is proprietary. Some of the process, however, is based on their many years of experience in the field...more empriacle than analytical. I wouldn't think the method would apply if the industry changed, but it does suggest that what you are asking is possible.
The application of the Boeing document does require a single degree of freedom system, or at least one where a majority of the mass participates in single mode.
The application of the Boeing document does require a single degree of freedom system, or at least one where a majority of the mass participates in single mode.
-
1
- #6
Hi,
the "displacement" values obtained after a MODAL analysis are the expression of the eigensolution normalized to a certain criterion (can be unity, or mass, or whatsoever, but the most meaningful are the first two, in general).
The "stress" values output by a FE program for a MODAL analysis have NO meaning at all, they are simply the mathematical computation of an "equilibrated force field" compatible with the "displacement field".
If you want to determine the stresses induced by a vibration, you have to "characterize" the causes which will induce this vibration, i.e. for example an alternating force, an unbalance, pulsations in a pressure field, etc etc, and then perform a response analysis. If the exciters are all sinusoidal or cosinusoidal, then you perform an "harmonic response" analysis. Otherwise you do a spectrum response analysis or a transient analysis.
Regards
the "displacement" values obtained after a MODAL analysis are the expression of the eigensolution normalized to a certain criterion (can be unity, or mass, or whatsoever, but the most meaningful are the first two, in general).
The "stress" values output by a FE program for a MODAL analysis have NO meaning at all, they are simply the mathematical computation of an "equilibrated force field" compatible with the "displacement field".
If you want to determine the stresses induced by a vibration, you have to "characterize" the causes which will induce this vibration, i.e. for example an alternating force, an unbalance, pulsations in a pressure field, etc etc, and then perform a response analysis. If the exciters are all sinusoidal or cosinusoidal, then you perform an "harmonic response" analysis. Otherwise you do a spectrum response analysis or a transient analysis.
Regards
cbrn,
"The "stress" values output by a FE program for a MODAL analysis have NO meaning at all, they are simply the mathematical computation of an "equilibrated force field" compatible with the "displacement field"."
Totally agree with you, well said.
But you can get some pretty pictures!
"The "stress" values output by a FE program for a MODAL analysis have NO meaning at all, they are simply the mathematical computation of an "equilibrated force field" compatible with the "displacement field"."
Totally agree with you, well said.
But you can get some pretty pictures!
I think we're all singing the same song. Even the Boeing document to which I referred is really a single degree of freedom frequency response analysis with some history applied in areas to simplify the math and add some other loads to account for other stress inducements. You may want to check with the Vibrations Forum, but I camp out over there a good bit, too, and am pretty sure you will get the same reaction...only perhaps a little more emphatically from the people that consider this sacred ![[smile]](/data/assets/smilies/smile.gif "[smile] [smile]")
-
2
- #10
fetraining
Aerospace
- Jul 29, 2008
- 17
All,
The stresses from a normal modes analysis are in general meaningless in their own right, but there are some ways they can be interpreted and used after some manipulation. One of these is via the Modal Effective Mass (MEM) concept. This is the basis for shock response methods and an outline follows. I wouldn’t recommend a hand calculation in practice, but it is useful to experiment with. If anybody is interested in the analysis file and spreadsheet calculations I can post them.
If the excitation is through a rigid base of a structure (and the structure is not connected to anything else), then the MEM can be derived for a unit input acceleration at the base. I won’t go into the maths here, but essentially the MEM of a mode is the inertia contribution each mode makes to a rigid body base acceleration. For a single DOF system the MEM is the mass of the system. For multi DOF systems the summation of the MEM from each mode will theoretically reach 100%. However in practice it is tough to get above 80% for real structures. Most FE solvers will output the MEM with the natural frequencies in a table. Note that MEM is not the same as ‘generalized mass’ or’ modal mass’, which is an arbitrary value.
Most FE solvers also output the Participation Factor (PF), this is actually the fundamental term used, but is not so easily visualized as the MEM. However the PF can be used to answer the original question.
"It seems like I should be able to scale the modal results using the reaction forces at the fixed support and a known g-load and mass."
Armed with the PF you can now use the equation for response of each mode in turn:
Response = FEresult*PF*Acceleration/(w*w)
Where FEresult is any nodal quantity (displacement, stress, reaction force) for each mode in a particular direction
Acceleration is the shock response acceleration ( more on that below)
W is the modal frequency in radians/sec (Hz value*2pi)
This also assumes the eigen vectors are mass normalized which is the default for most FE solvers.
As an illustration I have run a cantilever beam , with response only in the vertical plane. The MEM for the vertical direction is Mode 1: 61.08%, Mode 2: 18.88%, Mode 3: 6.48% - etc. The total for 10 modes is 94.9%.
This means we are able to represent 86.44% of the inertia response with the first 3 modes. I will stick to these for the moment.
If I take the vertical reaction at the end of the cantilever then apply the ‘response’ equation, but use unit shock Acceleration, then I get reactions forces in the same ratio as the MEM. For the first 3 modes I get 86.44% of the base reaction to a unit acceleration of the cantilever. If I could get 100% modal effective mass the total base reaction would equal the mass*unit acceleration.
However to turn this into a real shock calculation I need to consider a few things:
What is the shock Acceleration? For a unit shock acceleration input, what response will I get – I assumed 1 which is just to show the principal. In practice we use 1/G * input where G is the structural damping. That is a whole other discussion, but for now assume 5% structural damping (2.5% critical) across all frequencies, then the dynamic magnification factor is 20. In practice the shock environment would be defined by a shock curve of g versus frequency. So knowing your modal frequency you can just do a look up. The effect of damping is already assumed in the curve, so check what that assumption is.
How are modes combined? I could take all three modes and add the results which would give 20*.8644 peak base reaction. However it is very conservative as it assumes all the modes were in phase at some time in the time history response to the input shock. With multiple modes you have no idea how they will respond in terms of phasing. We are trying to take a snapshot of an event that happens through time. In practice the modes will move in phase and out of phase . The best we can do is to take the peak responses and then make assumptions. Most conservative is to take all modes and assume peak occurs together at some time in the response. A good compromise is to assume the modes within 10% of the biggest response occur at the same time and Square Root Sum of the Squares (SRSS) of the others. So assume phasing between close modes and add the 'noise' of the others. There are many, many variations.
In practice the first bending mode will give a dominant base reaction with 61.08% base reaction. The other modes may or may not come into phase. Using the other two modes in an SRSS gives 81% of base reaction. Using all 10 modes gives 81%. What this means is that we never see a full 100% of the structure mass * shock response acceleration, as the modes are never in phase as ‘one lump’. Some industries assume this is non-conservative and will deal with the ‘missing mass’ in various ways such as adding a pseudo static body acceleration.
Mode 6 gives an extensional response, so for a longitudinal shock this mode would be excited. The single mode gives 80.7% of longitudinal base reaction.
The same approach can be taken for displacements, stresses etc. on a mode by mode and nodal DOF by nodal DOF basis.
regards
Tony Abbey
The stresses from a normal modes analysis are in general meaningless in their own right, but there are some ways they can be interpreted and used after some manipulation. One of these is via the Modal Effective Mass (MEM) concept. This is the basis for shock response methods and an outline follows. I wouldn’t recommend a hand calculation in practice, but it is useful to experiment with. If anybody is interested in the analysis file and spreadsheet calculations I can post them.
If the excitation is through a rigid base of a structure (and the structure is not connected to anything else), then the MEM can be derived for a unit input acceleration at the base. I won’t go into the maths here, but essentially the MEM of a mode is the inertia contribution each mode makes to a rigid body base acceleration. For a single DOF system the MEM is the mass of the system. For multi DOF systems the summation of the MEM from each mode will theoretically reach 100%. However in practice it is tough to get above 80% for real structures. Most FE solvers will output the MEM with the natural frequencies in a table. Note that MEM is not the same as ‘generalized mass’ or’ modal mass’, which is an arbitrary value.
Most FE solvers also output the Participation Factor (PF), this is actually the fundamental term used, but is not so easily visualized as the MEM. However the PF can be used to answer the original question.
"It seems like I should be able to scale the modal results using the reaction forces at the fixed support and a known g-load and mass."
Armed with the PF you can now use the equation for response of each mode in turn:
Response = FEresult*PF*Acceleration/(w*w)
Where FEresult is any nodal quantity (displacement, stress, reaction force) for each mode in a particular direction
Acceleration is the shock response acceleration ( more on that below)
W is the modal frequency in radians/sec (Hz value*2pi)
This also assumes the eigen vectors are mass normalized which is the default for most FE solvers.
As an illustration I have run a cantilever beam , with response only in the vertical plane. The MEM for the vertical direction is Mode 1: 61.08%, Mode 2: 18.88%, Mode 3: 6.48% - etc. The total for 10 modes is 94.9%.
This means we are able to represent 86.44% of the inertia response with the first 3 modes. I will stick to these for the moment.
If I take the vertical reaction at the end of the cantilever then apply the ‘response’ equation, but use unit shock Acceleration, then I get reactions forces in the same ratio as the MEM. For the first 3 modes I get 86.44% of the base reaction to a unit acceleration of the cantilever. If I could get 100% modal effective mass the total base reaction would equal the mass*unit acceleration.
However to turn this into a real shock calculation I need to consider a few things:
What is the shock Acceleration? For a unit shock acceleration input, what response will I get – I assumed 1 which is just to show the principal. In practice we use 1/G * input where G is the structural damping. That is a whole other discussion, but for now assume 5% structural damping (2.5% critical) across all frequencies, then the dynamic magnification factor is 20. In practice the shock environment would be defined by a shock curve of g versus frequency. So knowing your modal frequency you can just do a look up. The effect of damping is already assumed in the curve, so check what that assumption is.
How are modes combined? I could take all three modes and add the results which would give 20*.8644 peak base reaction. However it is very conservative as it assumes all the modes were in phase at some time in the time history response to the input shock. With multiple modes you have no idea how they will respond in terms of phasing. We are trying to take a snapshot of an event that happens through time. In practice the modes will move in phase and out of phase . The best we can do is to take the peak responses and then make assumptions. Most conservative is to take all modes and assume peak occurs together at some time in the response. A good compromise is to assume the modes within 10% of the biggest response occur at the same time and Square Root Sum of the Squares (SRSS) of the others. So assume phasing between close modes and add the 'noise' of the others. There are many, many variations.
In practice the first bending mode will give a dominant base reaction with 61.08% base reaction. The other modes may or may not come into phase. Using the other two modes in an SRSS gives 81% of base reaction. Using all 10 modes gives 81%. What this means is that we never see a full 100% of the structure mass * shock response acceleration, as the modes are never in phase as ‘one lump’. Some industries assume this is non-conservative and will deal with the ‘missing mass’ in various ways such as adding a pseudo static body acceleration.
Mode 6 gives an extensional response, so for a longitudinal shock this mode would be excited. The single mode gives 80.7% of longitudinal base reaction.
The same approach can be taken for displacements, stresses etc. on a mode by mode and nodal DOF by nodal DOF basis.
regards
Tony Abbey
- Thread starter
- #11
fetraining
Aerospace
- Jul 29, 2008
- 17
Adubeng,
thinking about this some more:
The usual way to do a fatigue analysis using a real vibration environment is to use a random vibration analysis. That is a 'full blown harmonic' analysis as you describe it, followed by a PSD factorization to get an output PSD and then RMS stress levels. You also get the 'apparent frequency' associated with each RMS stress. Thus you have the cycle count and the alternating stress and can do Miner's damage calcs.
The deterministic equivalent of this for a known input would be to break down the loading into the frequency content based on the main structural modes. If the loads are steady state, then the shock spectra approach I described could work as the individual peak is the same, but you would have to define some type of 'loading' curve of g versus frequency, which would be a steady state condition.
In that case, you wouldn't combine the results using the SRSS method, you would do a damage calc for each individual mode - ie stress level and frequency (cycle count), then add the damage up.
A huge caveat here is that it has to be base driven loading. If your pressure vessel is sitting on a mounting and you can charterize its input motion by a peak g versus frequency through the base then you can do it. If you are cycling the internal pressure in the vessel then it is not base driven and you can only do a frequency response analysis.
There may well be processes to do this in commercial Fatigue software - I have only worked with Vibration fatigue (Random) or Psuedo static fatigue loadings where the dynamic effects are ignored.
Another issue is that in fatigue analysis, relative phase changes in loading input components make things very complex. a conservative, robust simplified appraoch could be useful.
regards
Tony Abbey
thinking about this some more:
The usual way to do a fatigue analysis using a real vibration environment is to use a random vibration analysis. That is a 'full blown harmonic' analysis as you describe it, followed by a PSD factorization to get an output PSD and then RMS stress levels. You also get the 'apparent frequency' associated with each RMS stress. Thus you have the cycle count and the alternating stress and can do Miner's damage calcs.
The deterministic equivalent of this for a known input would be to break down the loading into the frequency content based on the main structural modes. If the loads are steady state, then the shock spectra approach I described could work as the individual peak is the same, but you would have to define some type of 'loading' curve of g versus frequency, which would be a steady state condition.
In that case, you wouldn't combine the results using the SRSS method, you would do a damage calc for each individual mode - ie stress level and frequency (cycle count), then add the damage up.
A huge caveat here is that it has to be base driven loading. If your pressure vessel is sitting on a mounting and you can charterize its input motion by a peak g versus frequency through the base then you can do it. If you are cycling the internal pressure in the vessel then it is not base driven and you can only do a frequency response analysis.
There may well be processes to do this in commercial Fatigue software - I have only worked with Vibration fatigue (Random) or Psuedo static fatigue loadings where the dynamic effects are ignored.
Another issue is that in fatigue analysis, relative phase changes in loading input components make things very complex. a conservative, robust simplified appraoch could be useful.
regards
Tony Abbey
GregLocock
Automotive
In experimental modal analysis we extract the modes as idealised normal modes, but can resynthesise the original FRFs of the entire model (and hence the vibration spectra at each coordinate form a know set of excitations).
But in order to do that we need estimates of the damping of each mode and the modal mass of each mode, at the reference coordinate.
The modal mass effectively scales the amplitude of each mode.
Presumably this is just a restatement of Tony's post, from another perspective.
Cheers
Greg Locock
SIG
lease see FAQ731-376 for tips on how to make the best use of Eng-Tips.
But in order to do that we need estimates of the damping of each mode and the modal mass of each mode, at the reference coordinate.
The modal mass effectively scales the amplitude of each mode.
Presumably this is just a restatement of Tony's post, from another perspective.
Cheers
Greg Locock
SIG
lease see FAQ731-376 for tips on how to make the best use of Eng-Tips.Hi,
in fact, I see that sooner or later we fall back to the "harmonic response" concept.
The posts from Fetraining seem very close to an explanation of how the "harmonic response by modal superposition" works.
As the original question seemed to deal with stresses, there may be even a more trivial solution:
As an eigenshape depicts the "shape" that the freely-vibrating system would assume after it has been "pulled" out-of-equilibrium and released, if you are interested on the stresses induced by an exciter acting only on the first mode (for example), trivially "pull" the system with an applied distribution of prescribed displacements which corresponds to the eigenshape, then get the reactions, then compare them with the magnitude of the exciter, then scale accordingly.
I sincerely strongly suggest not to proceed like that, as you will have big troubles in superimposing the modes.
Once again, due to the fact that nowadays' FE programs are efficient in doing that, and the computer power is not an issue any more, I REALLY don't see why you would not do an harmonic response analysis or a spectrum response analysis depending on what kind of input you have.
Regards
in fact, I see that sooner or later we fall back to the "harmonic response" concept.
The posts from Fetraining seem very close to an explanation of how the "harmonic response by modal superposition" works.
As the original question seemed to deal with stresses, there may be even a more trivial solution:
As an eigenshape depicts the "shape" that the freely-vibrating system would assume after it has been "pulled" out-of-equilibrium and released, if you are interested on the stresses induced by an exciter acting only on the first mode (for example), trivially "pull" the system with an applied distribution of prescribed displacements which corresponds to the eigenshape, then get the reactions, then compare them with the magnitude of the exciter, then scale accordingly.
I sincerely strongly suggest not to proceed like that, as you will have big troubles in superimposing the modes.
Once again, due to the fact that nowadays' FE programs are efficient in doing that, and the computer power is not an issue any more, I REALLY don't see why you would not do an harmonic response analysis or a spectrum response analysis depending on what kind of input you have.
Regards
020100
Mechanical
- Aug 30, 2008
- 11
Hi, everyone,
Even though it is "NO" in theory, I used quite often for the following reasons.
(1). Quite a lot of frequency contents make very time- consuming to do harmonic anlaysis.
(2). Modal analysis hard to predict very broad spectrum over 5Hz to 2000Hz due to complicated structure. It makes harmonic analysis very unreliable.
But I did do a couple of things in order to ensure the simple static analysis makes sense.
I measured the vibration/displacement on the structure to see whether the static analysis generates reasonable results. In general, it is off by a factor ~2.
Hope it helps.
Even though it is "NO" in theory, I used quite often for the following reasons.
(1). Quite a lot of frequency contents make very time- consuming to do harmonic anlaysis.
(2). Modal analysis hard to predict very broad spectrum over 5Hz to 2000Hz due to complicated structure. It makes harmonic analysis very unreliable.
But I did do a couple of things in order to ensure the simple static analysis makes sense.
I measured the vibration/displacement on the structure to see whether the static analysis generates reasonable results. In general, it is off by a factor ~2.
Hope it helps.
- Status
Similar threads
- Question
- Question