Dynamic Analysis at Constant Frequency 2

[aphilic]

Hi guys,

I have some questions about dynamic analysis in Ansys. Im kinda new at this program so every help is so precious for me.

Well, for a project, i prepared a 3d structure and applied static displacement. Now i need to apply the same displacement as a sinusoidal function for 5 secs at constant frequency to the same model. I did the static analysis with the help of tutorials but for this analysis i cannot find anything that helps me.

Anyway, i think if i set the Analysis Type to Harmonic Analysis all the applied displacements will be in sinusoidal function. Is that true? All i need to do is to submit the amplitude of the applied displacement.

My analysis should be performed at a fixed frequency but all the tutorials mentioned to the determining frequency range and no of substeps and if is it ramped or stepped. Well i need one frequency but i dont know how to set it into the program.

My other problem is that, i want to apply this displacement for a few secs which is hundreds of cycles. I could not found anything for this option.

Thanks in advance.

Can

 

[Lirock]

Hi, Can
I think you can do a transient dynamic analysis and apply the load with function loader.There are great express in the help document about how to do a transient dynamic analysis and how to use the function loader.

Regards!

Rock Li

 

[aphilic]

Thank you very much Rock li! I ll give a shot.

Regards,

Can

 

[cbrn]

Hi,
as regards computational effort, Harmonic Response is the best way, unless there are some non-linearities in the model which must be taken into account.
Don't be scared if you find "frequency ranges" when all you need is a single frequency: the explanations in the help file must be as general as possible, and in your case a single frequency will be the exact same as a frequency range with only ONE loadstep (i.e. start freq = end freq, the freq range collapses into a single freq !).
See help file in Chapter 4.4.3.

Regards

 

[aphilic]

Hi,

Thank you cbrn. Well as much as i know i should use Harmonic response however i have faced some problems that i could not solve yet.

Well, as much as i have learnt so far, if i enter the same frequency as begining and ending frequencies, the analysis will be only at one desired frequency which is exactly what i want. Then i leave the number of substeps part blank and stepped or ramped preference as ramped. I think this is what i should do so far.

At this point, if i enter a constant displacement value (when the analyze is harmonic), it will be applied as a sinusoidal wave with the amplitude of the value that i enter in "displacement on nodes" place and with a frequency that i specified.

But again, as much as i know, this will be applied only for one cycle. However, i want it to be applied like 500 cycle. Or for 4-5 secs. Do you have any idea how i can do this?

Thank you very much in advance and sorry for sending this long post but i mentioned, im kinda new at this and i could not understand the program yet

Can

 

[cbrn]

Hi,
yes, I understand that the initial problem, with all the programs which handle multiple loadsteps in sequence, is understanding what a loadstep is.
You can think about it as a "set" or "configuration" of loads and boundary conditions.
Inside a loadstep, there is the concept of "substep": it's a sort of "instant of calculation", that's why the analogy with time is so strong; given an analysis "duration", there will be a certain number of substeps placed at a certain "time pitch". You can generalize the concept and remove the link with time; let's reformulate my previous sentence: "given a certain ratio of loadstep advancement, say for example 1 = 100% for simplicity, there will be a certain number of substeps placed at given advancement fractions, i.e. with 10 substeps the substep 1 at t=0.1 will have 1/10 of the loads, the substep 2 at t=0.2 will have 1/5 of the loads, and so on".
How do we shift from one loadstep to another? By using the "restart", which is seen as a continuation of the analysis where the program knows that you want to vary something in the boundary conditions. There are cases in which the loadsteps are created automatically, others in which the user creates them explicitely.

To return to your problem: in each loadstep, the harmonic response calculates the steady-state response for a well-determined excitation frequency. Therefore, there are no such concepts as "time step", "delta-time", "time duration", because for example the time duration could be infinite, or 2 secs, or 0.00001 sec, it doesn't matter; of course, nothing will be known about the duration of the transient phase of the response: if THIS is what you need, then you MUST do a transient analysis (the name says everything, huh?).
My advice is to very carefully read all the Chapter 4 "Harmonic Response Analysis" of the Structural Analysis Guide.
Hope this helps...

Regards

 

[aphilic]

Hi,

First I want to thank you for your reply here. I have read about Harmonic Response Analysis and Transient Analysis. I decided to use transient analysis for two reasons. In harmonic response analysis I am not allowed to add any nonlinearity into account but the material that I am modeling have viscoelasticity effects. Thats why time is important for me and in harmonic response analysis its not important at all. The other reason is obvious i guess.

Anyway, in transient analysis I think I have to build up a function then need to find a number of points within a desired time interval. After that, i have to save the point data and define it as a table of dataset to use as displacement values. At this point I need some suggestions. In my problem, the frequency i desire is 250 Hz and i want it to be applied within 0-5 secs. Thus, i need to define 1250 cycles in total. I thought that for each cycle if i define 20 points (substeps) the results will be accurate enough and the shape of loading will be like a real sinusoidal one (or it is sinusoidal enough). But then, the program has to solve 25000 substeps. However, in Ansys it is not possible to solve more than 1000 substeps (or at least as much as i know). Is there any way for Ansys to solve 25000 substeps in a row in one solve command? Or should i decrease number of points for each cycle from 20 to let's say 8 (which does not solve my problem completely)? Or should i do the solve command for every 0.1 secs (which is 500 substeps) and restart it for 50 times?

Moreover, i tried to solve for 1000 substeps (0.2 secs) and it took like 1,5 hours and like 20 GB HDD capasity for each substep data and .rst file in total. If i do it like 50 times more it takes enormous capacity of HDD (time is not my primary problem at this step). Is it normal? Is there anything that i can do to reduce the size of the file?

My last question is about results. When I did the 1000 substep solution I wanted to see the displacement of a node within the time interval (for 0.2 secs).I went to TimeHist Pros then pressed add data button. Then I specified the node I want to see the displacement in time. However, when I did everything and press OK button nothing happened. The program did not add the node to the list so I could not plot the time history graph of the node. It does not add any node to the list in Time Hist Proc. Why do you think it is?

Thank you in advance.

Regards,

Can

 

[cbrn]

Hi,
1- you have several possible ways to solve as many substeps as you need: either run several restarts in blocks of 1000 substeps, or force Ansys to increase the max number of substeps with /CONFIG,NRES,25000 for example.
2- Be careful to generate results files compatible with the readability in the operating system you use.
3- Try to generate as little data as possible. For example, 10 subs per period are sufficient to characterize a sine wave. Instead of saving "all results", select only those you are interested in.
4- However, transient = VERY huge files and solve times; this can't be avoided. Be careful: if you know that the static analysis of your model takes 1.5 hour, then it will be ABSOLUTELY IMPOSSIBLE to do a full-transient over 25000 substeps (more than 30000 hours ??!!??)
5- Not seeing any result over time is generally a consequence of not having saved the data FOR EVERY SUBSTEP. However, due to the dimensions of your results file it seems you have correctly done so. At this point I'd try running the analysis with much less substeps (say 10 or 20) in order to generate a res file smaller than 4 GB (it's not an absolute limit: I myself generated and read a res file of 12 GB without problems).

Hope this helps.

Regards