Strange results with Modal analysis/MES

[Anonymous]

Hi,

I'm looking to use Algor to model a wind turbine blade being fatigue tested. As part of this process I am benchmarking it against some other software I have available, namely ADAMS, Ansys, and Inventor simulation.

I am doing this by using MES, but I have tried to benchmark by using modal analysis as well. The benchmark model is just an aluminium beam, cantilevered and allowed to fall under gravity so that it vibrates in its first mode. Neither the modal analysis, or the MES with brick (even at very fine mesh size) or beam elements predict the behaviour. The other software packages all agree very closely that the natural frequency is 25Hz in the direction with the high stiffness and 14Hz in the direction with the lower stiffness, but Algor is way out. I followed the piston MES tutorial but it seems I am definitely doing something wrong somewhere... I don't want to discount highly regarded software because I'm not doing something right!

Thanks,

Pete

[PipePakPat]

Pete,

I reviewed your model and noted the mesh was too coarse. It appears that your model is a thin-walled square tube. Unfortunately, only the *.fem file was sent, which does not contain all of the model information. I did create a finer mesh, and defined as T6 aluminum. Because the model was thin relative to the mesh size, I activated the mid-side nodes option in the Element Definition screen. Mid-side nodes, or higher order elements, alleviate tetrahedral element "shear locking". I ran a linear modal analysis which produced 14.3654 Hz for the first mode and 24.935 Hz for the second mode. I have attached an archive of the newly configured model, which can be opened by changing the "Files of type" field to read Algor archive files (*.ach).

Pat Tessaro, P.E.
Autodesk Inc.

[Anonymous]

Thanks Pat,

Looks like midside nodes has solved the problem with the modal analysis frequency and the reason MES wasn't working was because the gravity load was defined with a ramping load curve rather than constant.

I do have one more question, is it possible to probe a nodes velocity, position etc. in MES and use that value to update a force value for the next time step by using a formula?

I'm sure I'll be back with more questions before too long!

Edited by: n1210933 on Mar 23, 2010 2:57 PM Edited by: n1210933 on Mar 23, 2010 3:08 PM

[PipePakPat]

Pete,

Access the "HELP|Search" pull-down menu in Algor and type "lookup". Choose the first topic to learn about Result-Based Load Curves.

Pat Tessaro, P.E.
Autodesk, Inc.

[Anonymous]

As I predicted I'm back with another question. I'm analysing a wind turbine blade (composite structure with difficult geometry) as a series of beam elements. I have, or can approximate, the following info at various different lengths along the blade: Torsional stiffness, EI value in both directions, Mass per unit length etc. I've got this information into a format that Algor can read, and filled out the section properties by using estimated values for the Young's modulus and density. However, it won't let me proceed because it says that it needs more information about the profile shape. It only needs this for nonlinear effects and stress analysis which I'm not concerned with (I just want the bending moments along the length of the blade). Is there any way to trick it, or make a new library? At the moment all i can think of is making it into parts that have the correct I values in each direction and fudging the material properties in order to get the results right for the other properties.

[John_Holtz]

If you want to use the MES software (Mechanical Event Simulation), then set the "Material Model" under the Element Definition to "Linear". This will ignore all of the secondary effects needed for nonlinear displacement, so you will then be able to use cross-sectional properties such as area (A), moment of inertia (I2 and I3), and so on. Note that you cannot enter these properties directly in the "Sectional Properties" spreadsheet. You need to select the row in the spreadsheet that you want to change, click the "Cross-Section Libraries" button, and set the drop-down boxes to "User Defined". You can then enter the properties directly.

The other option is to use linear stress (either static or transient stress depending on what you are calculating).

John Holtz
Product Design
Autodesk

[Anonymous]

Hi Jon,

I've attached the model. I seem to have lost something by making the material model linear, it's not moving now when the simulation is run. Does it need an isotopic material in order to react to the gravity forces?

Thanks

[John_Holtz]

It is not moving because the analysis did not run: it stops with an error message before performing any calculations! The error message from the processor is trying to tell you that you cannot perform a large displacement calculation when using the linear material model. By changing the Element Definition setting of "Analysis Type" to "Small Displacement", the analysis will run to completion.

P.S. I assume that you have the "Tools > Options > Analysis > Automate Analysis" option checked, and this is why you didn't notice the error. (If I remember correctly, checked is the default for this option. When checked, the analysis window is automatically closed after the processor finishes.) In this scenario, you can go to "Report" environment (tab at bottom of browser tree) and look at the branch "Processor Log Files > Analysis Logs" to see what happened during the analysis and why you have no results. (It's not that the displacements are 0; there are no results.)

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[Anonymous]

thanks very much Jon, believe it or not I thought I might be able to glean something from the log but I couldn't find it. Your help is much appreciated.

[Anonymous]

Another question on this subject; I have created a model of a cantilevered beam using beam elements. It starts off in a horizontal position and falls under its own weight setting up a vibration The analysis is linear and small displacement (I've run a comparison to see if this affects the results and it's OK) and I am applying no damping, either material (I can't be because it's beam not brick elements) or Rayleigh damping in the advanced tab of the Analysis type menu. I know that there are no energy losses in the system and yet the amplitude of the oscillations decay away as if I'd applied damping. Any idea why this might be? I know that there will be damping once I model the final system but I want to be able to control it.

[John_Holtz]

Very observant, Pete. The "damping" comes from numerical damping to help improve the convergence. These settings are located under the "Analysis: Parameters: Advanced: Integration" tab. If my memory is correct, the default integration method is "General: MES, NLS" with a parameter of 1. Changing the parameter to 0 should eliminate all of this numerical damping.

The next thing to check is whether the calculation time step is small enough (capture rate large enough) to capture the behavior of the vibrations. If you think of a sine wave and imagine calculating the results at only 3 or 5 points along one cycle, then the results will be "rough". If you capture 10 or 20 steps, then the approximation is better. Let's say you want 20 steps per vibration cycle. Based on this, you can calculate the MES Capture rate as (20 steps/cycle) * (F cylces/sec), where F is the highest frequency that you want to capture. (Normally only the first few frequencies are important.)

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[Anonymous]

Hi. Thanks again for your previous help, I'm almost there with this. I have two more questions... As I mentioned earlier I'm analysing a beam that is being excited by a device that moves a mass at the resonant frequency of the system in order to fatigue test it. This means that the device is started when the beam is in an equilibrium position. I can do this by starting the loads after the free vibrations have been damped away and just wait for them to finish every time, or I believe I can do a restart analysis? I've found the .asd file for the analysis (and checked it's for the right analysis by making a new design scenario and running that) but I get an error right at the start of the run. Is there a way of making sure that the asd file is correct for the analysis?

The second thing, which is a bit more important, is that I need to get an output of the bending moment in the 2 and 3 directions as a time history at each node. I haven't found an option for graphing this, would I maybe need to write some VBA code or something?

Thanks,

Pete

[John_Holtz]

Pete,

The restart idea is a good one. Like you said, no need to run every simulation and wait for the "pre-stress" condition to be obtained. In some situations, a way to reduce the amount of time it takes for the vibrations to die out, is to use prescribe displacements (PD) to pull/move the model closer to the expected equilibrium position, and use the death time to "remove" the PD from the analysis. [So instead of applying the loads, which may be gravity and forces, and watching the thing vibrate for X number of cycles, apply the loads and PDs. A simple linear stress analysis should be efficient to get the equilibrium position when it is not known ahead of time.]

You didn't mention what the error was. If you have not reviewed this page in the documentation ("Help > Contents"), then it might provide some answers to your problem. There are different restrictions and procedures depending on what type of restart analysis is being performed. [Autodesk Algor Simulation > Setting Up and Performing the Analysis > Setting Up Part 2 > Nonlinear > Analysis Parameters > Advanced Settings > Performing a Restart Analysis]

For the second item, you can graph any result that you have shown in the contour plot. So in your case, you would go to "Results > Forces and Moments > Moment 2" to display the first results, then select the nodes (Ctrl+A if you literally want all of the nodes), then right-click and choose "Edit Graph". By default, the graph shows the sum of the results, but there is a drop-down so that you can get one curve for each node.

After the graph is created, you can either change the result type while viewing the graph, or go back to the contour presentation, change the result there, and create a second graph or add the moment 3 results to the existing graph. Also, right-clicking on the graph window gives an option to output the data to a text file if you want that.

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[Anonymous]

Hello again...

Thanks for your previous help, I've got a really good model coming along. I have another question though... Is there a way of creating a representative surface when using beam elements? It is a little hard to visualise what is going on with the model at the moment, as all I have is a line that is slightly thicker in one direction than the other. I've seen that you can get various section shapes but as I'm using user defined section properties I don't get to use them. I can attach a model if that helps.

[John_Holtz]

Hi Pete,

I looked at the previous model you posted, so I have a good idea of what you are doing. Currently, there is no means of visualizing a beam that has user defined properties. Do you have a suggestion on how we might be able to implement it?

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[Anonymous]

Hi John,

The only reason I asked was that I'd heard you could do something similar in ANSYS, but it could well be that that function is the same as the general beam element in Algor. The only way I could think to do it is to define a cross section (by using a series of y,z coordinates with 0 as the centre of the element, see this page http://www.ae.illinois.edu/m-selig/ads/coord_database.html for what I mean by this) for each end of each beam element and do a loft between the two, or just have some pre defined sections for visualisation purposes only... in my case it would be useful just to be able to show the beam as a rectangle so the major axis was instantly identifiable. I have now discovered the ability to show and hide the beam orientation markers so my problem is solved anyway.

With regards to the prescribed displacement thing you mentioned earlier, I tried this and the simulation wouldn't run. I am performing a small displacement linear analysis in MES, and I let the model run until the damping had removed all movement. I then inquired the displacement at each node and applied this to the model with a death time of 1s after the simulation begins. A strange thing that I noticed with this was that the x displacement was zero even though the y displacement wasn't (because the beam was bending). Is there a reason for this? The error code was "non linear formulation used in linear analysis" I think. I'll attach the model on monday if that's not enough info for you to help.

[John_Holtz]

Thanks for the suggestion on visualizing the beams. I'll have to see how feasible that would be. (It sounds easy in theory, but gets difficult in the details depending on the cross-section shape.)

Regarding the prescribed displacements (PD), it was a good idea on my part, but unfortunately I was not aware of a restriction. The PDs make the model nonlinear, but the beam elements force it to be linear! Thus, the analysis will not run due to this conflict. Hopefully you can accomplish the same final goal without needing the PDs.

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[Anonymous]

More on this... I'm trying to simulate air resistance in a MES.

The test article is again a cantilevered beam, with a force which excites it near it's resonant frequency in order to fatigue it.  I have calculated material damping using physical tests but the results still aren't matching up to reality, so I now want to incorporate damping from air resistance.  I want to do this by applying probes to various nodes along the beams length measuring their speed and then using the Z velocity of the probe in the formula below.

F=-0.5*air density*Area around node*abs(velocity)*velocity* drag coefficient

The minus at the start and the abs() mean that the force should always oppose the motion and thus cause it to die down, however in practice the model quickly gets into a feedback loop and goes crazy.  I've been through the help files and I can't find anything similar (I contemplated using if statements and multiple columns in the look up table for when the beam is moving in different directions but I don't see how it will help).  The load curve that is relevant is number 3.  Does anyone have any idea how to solve this problem?  I've attached the archive.

[S.LI]

The "huge" displacement value looks like a display problem in post-processor.

Mouse right click and do "undo zoom", your displacement shows in the right way.

Another way is 1.) close the current displacement windows, 2.) open a new one. The number looks right, since I can see reduced amplitude over there.

[Anonymous]

I'm getting displacements of something like 1*10^113m, has anything changed between algor 2010 and 2011 that could cause it to work for you and not me?  I'm expecting an amplitude of about 0.025m that decays gradually in a sine wave.