Transient Shock Analysis in Creo Simulate vs Ansys

[jameslamb]

I am looking at a transient shock analysis of an assembly which contains 3 components each connected by springs of various stiffnesses, I am moving the base of the model and measuring the response of the structure using acceleration measures. I am finding that my Ansys and Creo Simulate results do not marry up very well unless I use a damping factor of 5% in Creo and 15% in Ansys (changing this in ansys has little/no affect to the first response as you might expect), can anyone explain this to me. The other interesting thing I have found is that increasing the damping in Creo increases the acceleration magnitude of the response. Is the damping factor increasing the spring stiffness?

Thanks in advance

James

 

[shaun8567]

What level of convergence did you get on the modal analysis for both Simulate and ANSYS? How many modes did you ask the solver to calculate for both? What results combination method did you use for Creo and for ANSYS? Creo has Absolute Sum and Square Root Sum of the Squares, where as ANSYS has these plus CQC, ROSE, and some others.

Regarding the increase in the acceleration magnitude as you increase you damping, that depends on you input. If the majority of your input is past the cross-over frequency, then increasing the damping will increase the magnitude of the response.

 

[jameslamb]

Hi Shaun,

Thanks for the reply.

For the Simulate analysis I asked for 10 modes (the first two achieve 100% mass participation according to Simulate) and achieved the following convergence;
Mode Frequency (Hz) Convergence
---- -------------- -----------
1 9.600748e+00 0.0%
2 1.841376e+01 0.0%
3 2.058550e+02 0.5%
4 4.762221e+02 4.3%
5 4.775110e+02 5.1%
6 1.355810e+03 0.3%
7 2.523667e+03 0.7%
8 3.995857e+03 0.4%
9 5.032525e+03 0.7%
10 6.649013e+03 0.7%
I am not sure what solver I used in Simulate and cannot seem to find this information, I have looked in the solver output and the analysis setup.

With Ansys I cannot run a modal superposition analysis due to the fact that I am using a displacement constraint (I was informed by an Ansys representative that this is the case) so ran a full transient analysis with the direct solver.

I used acceleration probes in each simulation and plotted the acceleration of each body using excel.

Excuse my ignorance but is the cross over frequency when the frequency of the input equals that of a natural frequency? I still don't really understand why increasing the damping will increase the magnitude of the response. It sounds counter intuitive from a real world view point, how do you know which damping coefficient provides you with the most accurate answer?

Thanks again for your help.

James

 

[shaun8567]

That should be enough modes. Regarding the mode combination method you used, look in the analysis definition under the, "Response Spectrum" tab.

Wait, you were told that you can't use modal superposition because you're using a displacement constraint? Do you mean you're applying a prescribed translation constraint on some entity of the model (for example, this surface moves 1e-6 inches in the x-direction)? I'll need more information on the system to say for sure, but I see no reason why you can't do this as a pre-stressed modal analysis. Now, all that being said, you're comparing a linear superposition analysis to a non-linear transient analysis, so the first question to ask yourself is: are the assumptions of linear superposition appropriate for you system? Furthermore, non-linear transient analyses (i.e. explicit dynamics) can be difficult to perform correctly, so you're ANSYS solution may not be valid.

The cross-over frequency happens when the frequency ratio is equal to sqrt(2). If you look at a plot of the magnification factor vs. the frequency ratio (omega/omega_n) for different values of the damping ratio (zeta), you'll see the plots cross-over at a value of sqrt(2). Increasing the damping ratio only results in a decrease in the magnification factor if the frequency ratio is below sqrt(2); after sqrt(2) it results in a higher magnification factor.

 

[shaun8567]

Regarding your question, "how do you know which damping coefficient provides you with the most accurate answer?", what do you mean by, "accurate answer"? Are you asking what damping ratio you should use on a (for example) welded steel structure?

 

[jameslamb]

Hi Shaun,

Really the accuracy question was coming from my Mechanica analysis, by changing the damping (something I had anticipated to not affect the first maximum response of the system greatly) I was getting vastly different answers. If analysis has been done in the past with say a 15% damping factor applied but a 20% damping factor produces a different result, how do I know which is more accurate in real world terms without physical testing? Currently in Ansys I am calculating the Rayleigh damping coefficient from the natural frequancy with the highest mass participation factor (applying only the stiffness coefficient) to acheive a zeta of 0.15.

For my analysis I am moving the base of an assembly in one direction to achieve a certain acceleration pulse input. The base is connected to the main structure using a bushing to simulate the spring shock mount. The shock pulse will then move up the assembly through a number of bushings until it reaches the last component. I expect the shock profile (accel time) to reduce in amplitude and widen as it moves through the structure and springs. I am finding however that the attenuation of shock through the assembly is not as expected and that in some structures the acceleration value increases as if energy is being added. One other interesting thing is that where I would expect to see a time lag between the response of two components I see no lag at all, both structures react at the same time (my time steps are small enough at 0.1ms), this may be due to the fact that there is a very stiff spring between these but I still expected some attenuation.

Thanks again for your time.

 

[shaun8567]

Something just occurred to me that I should have caught at the start. You said you were doing a shock analysis, so I assumed you were using the Dynamic Shock in Creo. However, you said you were adjusting the damping ratio value in Creo, which is something you can't do in a Dynamic Shock (since a Dynamic Shock uses the Response Spectrum Method, which has the damping accounted for in the curve). I assume that you're doing a Dynamic Time analysis in Creo, correct? That being said, if you are doing a Dynamic Time analysis in Creo, then what did you define as your input? Creo's Dynamic Time can only take an acceleration curve/table as an input for base excitation, but in ANSYS you're essentially using a displacement curve/table with your displacement constraint. However, assuming you've set up both analyses correctly and that your mesh for each is such that you have accurate results, the difference between the two might be because your system is very nonlinear. It might be worth your time to make a simple model (say a SDOF system) that you know linear superposition is valid for, and solve it using the same methodology in each package and compare the results.

[highlight #FCE94F]"I expect the shock profile (accel time) to reduce in amplitude and widen as it moves through the structure and springs. I am finding however that the attenuation of shock through the assembly is not as expected and that in some structures the acceleration value increases as if energy is being added."[/highlight]

Hmmm, wouldn't that depend on the nature of the structure? The wave speed through a structure depends on the local stiffness and mass, so the wave speed could increase or decrease depending on the specific characteristics of the structure. For example, image you have three springs of the same length and mass, but different stiffness, where the first spring has a lower stiffness compared to the second spring, and the third spring has a lower stiffness compared to the first spring. If you gave an impulse to the free end of the first spring, you'd see a wave travel through the first spring at some speed v₁. However, once the wave reaches the end of the first spring and passes into the second (stiffer) spring, you'd see the wave speed up and travel at some velocity v₂. Finally, when the wave reach the end of the second spring and passes into the third spring, you'd see the wave slow down and travel at some velocity v₃. You'd have the relation: v² > v₁ > v₃.

[highlight #FCE94F]"One other interesting thing is that where I would expect to see a time lag between the response of two components I see no lag at all, both structures react at the same time (my time steps are small enough at 0.1ms), this may be due to the fact that there is a very stiff spring between these but I still expected some attenuation."
[/highlight]

Is this in your ANSYS or Creo analysis? If it's in the Creo analysis, and you're doing a Dynamic Time analysis, what are your setting under the "Output" tab? Can you post a screen shot? If it's your ANSYS analysis, have you made sure to construct a proper mesh? I don't have much experience with explicit dynamics, but I do know that mesh is much more important in explicit integration compared to implicit. Furthermore, you critical time step is very important as well, and having a critical time step that is either too larger or too small can result in a poor simulation.