Spectrum Analysis - Off Resonance Results

[roseda]

I have ran both a Modal and Spectrum analysis on a Mechanical System.

The Spectrum results shows high stresses in a mode that is slightly above the excitation frequency range.

Question: Is it possible to find the stresses at another frequency other than the modal frequency to determine how fast the stresses reduce?

I have tried Harmonic analyses but for some reason these give different stress values and mode shapes at the modal frequency.

 

[Stringmaker]

Is it possible that in your harmonic analysis you are not exciting it in a direction which has a high mass participation factor? Take the example of a flat plate for instance. Typically they are not a very stiff structure but when the direction of excitation is inplane it takes a very high amount of energy to excite it whereas out of plane excitation occurs very easily.

 

[SANOSAN]

First: I apologize for my english....hope that you will understand me.

My opinion about your problem:

As far as I know, the principal steps for spectrum analysis are the followings:

input:
- frequency range for modal analysis (from fmin1 to fmax1)
- spectrum data from frequence fmin2 to fmax2

Output:
Modes shape, participation factors and combined response from those later.

If fmax1 > to fmax2 I think that last acceleration from spectrum input (at fmax2) is applied to each mode shape which is calculated after fmax2....

In clear, if fmax1 superior to fmax2, it is possible that you analyse your structural response for natural frequencies uppon your excitation frequency range (if modes exist between fmax1 to fmax2). Your fmax1 is probably not exactly equal to fmax2?...if fmax1 and fmax2 are equal, you can't obtain response which consider mode shape superior to fmax2. So, the case that you desdcribe in your thread is not possible I think.

In addition, your second remarks about differences between spectrum and harmonic analysis is quit normal. Spectrum and harmonic are to different things. Spectrum is a simply way (not very realistik sometimes) to calculate dynamique response of a structure by combinaison of determined mode shapes. In this case, user decide which mode shapes must be considered (by the frequency range for modal analysis) and the way to combine them (cqc srss etc.). This method is, in general well adapted to strcutures exited on a their base (ex: buildings under seismic loading)

Contrary to spectrum analysis, harmonic analysis consists to solve the general motion equations with forced load (gamma x masse + velocity x damping + displacment x stifness = forced load ).

Harmonic analysis is the real theorical dynamique response of a structure (asuming that the later is compute from the full modal base) under several kind of unconsant loadings (forces, displacement, pessure etc.) which can be applied anywhere on the structure.

I dont't know about your kind of study but the harmonic analysis can be applied with minimum of restrictions and asumptions. In general, results are satisfying and don't need to much justifications and checkings.
You must be very aware about your results and your asumptions when you decide to use spectrum analysis.

Cordialement.

 

[roseda]

Thanks for the replies.

Stringmaker, I am exciting my system at the nodes where it is attached to the exciter and applying the same acceleration in the x, y and z directions as three seperate load steps. I then combine these with load cases using SQRT(x^2+y^2+z^2). This is the same way that the loads are applied in the spectrum analysis.

Sanosan, a small misunderstanding - my input range fmin2-fmax2 is a lot greater than fmin1-fmax1 - I was trying to say that the item that my system is attached to has a running range of say 0-100Hz - we then add a margin of safety to this of 25% and so try to design our systems to fall above 125Hz. The system that I am working on as a modal frequency of 120Hz and I need to determine the stresses at 100Hz and 110Hz. My system is similar to a building in that it consists of a range of brackets attached to an exciting structure.

I have performed a simple comparison on a rectangular plate with two mounting holes and the analyses both show different mode shapes.

Sanosan, from what you say, I think that the stresses will never match, but the mode shapes surely should?

 

[roseda]

I have found an error.

I have attached my system to the exciter by the following method (at each bolt hole):

Node1 has fixed DOF

Node2 is coincident with Node1 and connected to it by a MATRIX27 element to represent the stiffness of the exciter.

Node2 is connected to the system bracket bolt hole using beam elements.

My error: I was accidentally applying my exciting forces to Node1.

With the forces applied to Node2, the mode shape is now correct.

However, I have checked the stresses at the modal frequency and 10Hz either side and found that instead of peaking at the modal frequency, they are increasing with frequency!

Compared to the Spectrum analysis, the stress is approximately double at the modal frequency.

I am new to harmonic analysis - does anyone know what I am doing wrong?

My Procedure:
1. Run Modal Analysis
2. Set up an Harmonic Analysis - leave settings at default
3. Apply a Structural Force to the attachment nodes in the X direction.
4. Write Load Step
5. Repeat for the Y and Z directions
6. Load Step Opts >> Time/Freq >> Damping >> DMPRAT=0.02
7. Load Step Opts >> Time/Freq >> Freq >> Ramped >> 3 substeps
8. Solve >> From LS Files
9. Create Loadcases for all substeps
10. For each frequency, read Loadcase FX, Square it, add Loadcase FY^2, add Loadcase FZ^2, Squareroot
11. Check Results

 

[SANOSAN]

Sorry for the misunderstanding...it's not very easy sometimes to figure out the nature of our problems...never mind...

About your last post:

My Procedure:
1. Run Modal Analysis
---> It is not necessary for harmonic analysis (motion equation is directly solved...)

2. Set up an Harmonic Analysis - leave settings at default
---> ok

3. Apply a Structural Force to the attachment nodes in the X direction.
---> Why only in one direction? Solution must be the same when you apply Fx, Fy and Fz simultaneously.

4. Write Load Step
---> not necessary if Fx, Fy and Fz applied simultaneously in the same load step.

5. Repeat for the Y and Z directions

6. Load Step Opts >> Time/Freq >> Damping >> DMPRAT=0.02
--->OK

7. Load Step Opts >> Time/Freq >> Freq >> Ramped >> 3 substeps
--->So, You want to analyse 3 frequence responses? If you want to analyse a 1 single frequence response (to identify your problem precisely) you may set Load Step Opts >> Time/Freq >> Freq >> Stepped and set one step between 0 and the specific frequence from wich you need to compare other results.

8. Solve >> From LS Files

9. Create Loadcases for all substeps

10. For each frequency, read Loadcase FX, Square it, add Loadcase FY^2, add Loadcase FZ^2, Squareroot
---> Are your output Items summable (see 5.5.5.3 of ANSYS V9 online manual)? If yes, do you combine both Real and Imaginary part? Could you be more precise. Normaly, harmonic results contain one real part and one imaginary part (to be combined in order to view amplitude result. See next point).

11. Check Results
--->If you are checking results remember to set your phase angle to a value > to 360° to chek amplitude result(HRCPLX,load step, sub step,400) but you are probably aware about this.

If your are aware about all this points, we should probably search another origin problem. Example: When 2 modal frequencies are close enough, they can lead to a one single peak response (instead of 2 distincts)...to see...

Just one more thing about : "Sanosan, from what you say, I think that the stresses will never match, but the mode shapes surely should?"

When you analyse a single frequence response, your deformed shape don't match necesseraly the mode shape of the correponding modal analysis. It depends on the configuration of your loading. Does your load excite the researched mode shape (as stringmaker said it in his last post). Moreover, even if your load excites the strcuture at the mode frequencies requiered, other modes can participate to the response. Your load can excite multiple modes so that the result mode shape is a combination of multiple modes which are excited too (in general with lower participation). In this case mode shape don't match.

I wish my discussions will be helpfull for your analyse.

Good work !

 

[roseda]

Thanks for all your help.

Modal Analysis is required:
Ansys10>>Help>>Contents>>Structural Analysis Guide>>Harmonic Response Analysis>>Performing a Harmonic Response>>4.4.3>>Note)

My outputs (elastic stress) are summable.

I did not know about the HRCPLX command (there isn't much mention of it in the online help!)

My test analysis of a plate has a 35.3Hz mode (flapping). The next mode is at 221.4Hz which is far enough away to be disregarded.

I have had another go and put the 3 load components on simultaneosly which avoids having to do any summing. I have also set the input to Stepped. Using the HRCPLX command, I now see a stress peak at the modal frequency.

The only thing left now is the size of the stress. My spectrum run gave a stress of 52098 at 35.3Hz.

Harmonic Results:
25.3Hz = 151976
30.3Hz = 164750
35.3Hz = 698878!
40.3Hz = 193099

so the stress at the modal frequency (35.3Hz) is 13.4 times larger than the spectrum analysis.

One thing that I'm not sure about is the loading. The spectrum analysis is run with a macro that was written by a person who is no longer at the company. It applies seismic loading seperately in the x,y and z directions, solves and then SRSS's the results. The input loading is 8.3g which is multiplied by 386.4 to convert to in/s^2 - it is then also multiplied by 25 (the Q value) - should this be included in the load for the harmonic analysis or is it taken care of by the 0.02 damping (which is equivalent to Q=25)? [Q=1/2z]

If I leave the 25 multiple out of the load, I get the following results:

Harmonic Results:
25.3Hz = 7443
30.3Hz = 7529
35.3Hz = 29616
40.3Hz = 7775

which are a lot closer but still a factor of 1.75 out.

Does it matter which direction I apply the loads in the Harmonic?

The spectrum analysis input is a curve that happens to have a flat section of 8.3g within the frequency range that I am interested in. Perhaps the accelerations at the other frequencies are providing some of the excitation. Can I use the table function in the F command to apply the full spectrum curve to the harmonic analysis? or is there another method?

 

[SANOSAN]

So, I understand that you are analysing your structure response with a mode superposition methode (not the full methode)...In this case I'm agree with you, you need to generate the mode shape before. I thought that when you've said :"2. Set up an Harmonic Analysis - leave settings at default" it meant that you use Full resolution methode.

The HRCPLX is well documented in the online help of ANSYS. I am very surprise that you can't find this command.

I think your spectrum analysis can be wrong...
When you set up a damping in ANSYS, it has no dimension. It is why it generaly in express in %.

Does the macro that you use run the spectrum procedure of ANSYS?

If yes be carefull about your SVTYPE and SV command. Damping is a value <= to 1.
Be carefull about units in your SV input (defining your spectrum curves). The units must be coherent. For me, I use Tonnes - mm - mm/s^2 to get MPa stress unit.
Be carefull about the FACT parameter in the SVTYPE command. It can be modified to get coherent your inuput data defining the spectrum curves.

The spectrum analysis must be lead with a lot of attention. Errors can appear easier than with a harmonic analysis.

But, I repeat : About your precise case, i think that you can't match harmonic and spectrum analysis results. You probably take the problem in the wrong way.

 

[SANOSAN]

With SVTYPE,2 (acceleration versus freq.) you may be match the results...Be carefull of units, damping and your acceleration direction. You need the SVTYPE (to define the kind of excitation), SV (to define acceleration value, becarefull, the first value is the damping ration of your spectrum), FREQ (to define frequences), and SED (to define acceleration direction) commands to define your analyse and your spectrum curves.

Matching results is also depending on the way to combine modes....you must match the combination method from your macro with the option that is activated in the harmonic calculation parameters (you can choose CQC, SRSS, DSUM etc. combination procedure..).

Run the ansys spectrum analysis with superposition methode.
In this case, I think you may match the results....

Good work !