Transient structural analysis: busbar vibration

OROIOROI Member Posts: 7

Hi


I'm simulating short circuit force of busbar. I noticed that, busbar does not vibrate like it should, after there is no electromagnetic force applied. Busbar and steel supports bend only positive side but never go to the negative, its just dampens before it goes to negative side. How to make it busbar behave more realistic?


Here is how it should behave.


Comments

  • peteroznewmanpeteroznewman Posts: 12,827Member

    @OROI

    Total Deformation is always positive because it is the distance from the starting point.

    Plot Directional Deformation and set it to the Z axis direction. That will show positive and negative values.

  • OROIOROI Posts: 26Member

    Hi

    I plotted directional deformation and it is still only positive or it is not crossing zero point.


  • peteroznewmanpeteroznewman Posts: 12,827Member

    @OROI

    Select a single node at the center of the bar to plot Directional Deformation in Z, that should cross zero.

  • OROIOROI Posts: 26Member
    edited November 25

    Here is single node Directional Deformation, it does not cross zero point, i can also clearly see that movement stops before it goes negative side when i play the animation.


  • peteroznewmanpeteroznewman Posts: 12,827Member
    edited November 25

    @OROI

    The deformation shown is the correct simulation result for that model.

    If you want a different result, you need to change something in the model.

    Do the materials include plasticity or are the materials all linear elastic? If you have plasticity, try removing that from the material model.

    You could change the imported load.

    You could simulate for 1 extra second with no load.

    You could change the thickness of the supports.

    You could change the thickness of the bus bar.

    You could change the density of the bus bar.

    I recommend you run a Modal analysis on the structure and learn what the first modal frequency is. I think you have a mismatch between the timing of the Rejecting Force and the natural frequency of the structure.

  • OROIOROI Posts: 26Member

    I made little longer simulation and it crossed zero point little bit. Earlier i simulated with half of imported load, that change only affected the amplitude, i try even lower load next.


    Is there some property that i should add or remove for this kind of simulation?




  • peteroznewmanpeteroznewman Posts: 12,827Member
    edited November 26

    @OROI

    The materials are all linear elastic, so no plasticity.

    In Workbench, Drag and Drop a Modal Analysis onto the Model cell of the Transient Structural analysis.

    Click Solve and reply with the frequency of the first mode. You should compare this frequency with the frequency in the Imported Load.

    I can help you calculate the frequency in the imported load. In Mechanical, right click on the Mesh branch then Clear Generated Data. File Save, then File Archive which will create a .wbpz file. Attach that file to your reply and I can open your model.

  • OROIOROI Posts: 26Member

    ok, here you have it, i hope it went right.


  • peteroznewmanpeteroznewman Posts: 12,827Member
    edited November 26

    @OROI

    I can't open your archive file because you have Ansys.Ansoft.CoreAddin.Addin and I don't have that installed so it won't let me open the archive.

    I'm not sure how to fix that but you can go to Workbench and click on Extension, Manage Extensions...

    If you see Ansoft in your list, uncheck that and try saving the archive file again.

    Or you can put the imported load into a spreadsheet and attach that to your reply.

  • OROIOROI Posts: 26Member

    I did not have Ansoft extension, but only difference was "Speos" extension, so i unchecked that, maybe it now works. Here is also imported load.


  • peteroznewmanpeteroznewman Posts: 12,827Member
    edited November 26

    @OROI

    I get the same error trying to open this archive. I don't know how to fix this problem. I opened my own question to get advice.

    How many other systems are in that project? Is it just a single Transient Structural system? If not, it is the other systems causing the problem. In that case, you can right click on the Transient Structural and just Export that one system.

    Unfortunately, the BodyForceDensity file had force components for all elements in the model at a single point in time, not a time history of the load.

    Can you plot a time history of the sum of the Z component of forces along the bus bar?

  • OROIOROI Posts: 26Member

    Project includes is also Maxwell 3d blocks, here is attached only transient structural system block.


    If you can't open the model, can you use these probe force values, if not, can you tell how to plot that sum of the Z component of forces along the bus bar.


  • peteroznewmanpeteroznewman Posts: 12,827Member

    @OROI

    I was able to open the archive with only the Transient Structural included.

    Below are three plots. The first plot is the force on the middle joint that you provided in Probe2.txt. The second plot is a filtered version of that and the third plot is your transient displacement results.

    It's clear that the motion of the center of the bar is following the input force, filtered by the mass and stiffness of the structure. Notice that the force is always positive, so it is not surprising that the displacement is always positive.

    If you want to see the busbar oscillate back and forth, you need to simulate for 3 seconds, where the first 1.5 seconds has the applied load while the last 1.5 seconds has no load.

  • OROIOROI Posts: 26Member

    ok, here is the report of that real world test what i'm trying to simulate. Do you think that my model in structural way is like in this report or should i change something, to make it behave like in report results (does not have to be exactly same, but close)?


  • peteroznewmanpeteroznewman Posts: 12,827Member
    edited November 28

    @OROI

    Attached is a beam element model of one busbar (the other is suppressed and incomplete). The first mode of this busbar is 2.89 Hz which has a period of 0.346 s. You can see that I have 3 joints. The fixed joint represents the clamp at point B while the two spherical joints represent a hinged connection at points A and C. I adjusted the density of aluminum to get the weight of the busbar correct.

    Look at the first cycle on the graphs you show. It has a period of approximately 0.34 s so the model above is a reasonable close representation of the structure.

    It seems to me that in this experiment, the power is turned on from t=0 to t=0.135 s then turned off. This pulse kicks the busbar to the side and begins the oscillation. Then from t=0.580 to t=-0.885 s the power is turned on then off to kick the oscillation to a larger positive value and a smaller negative value while the power remains on.

  • OROIOROI Posts: 26Member

    ok, i tried import that beam model what you made, but it seems that Maxwell tool does not understand that beam geometry correctly. Not sure but maybe geometry needs to be solid model. I think it would be take less time to simulate if i use beam model. I try to adjust that solid model.


  • OROIOROI Posts: 26Member

    I made adjustment for those support pillars and changed end joints from fixed to spherical. Now one cycle time period seems to be close, but still it does not oscillate from positive side to negative like in that report results.


    Here is results with high and very low load. It seems to me that the model permanently bends and it gets new zero reference from positive side where it continues oscillation. What i should change to prevent that "bending"happening, if that is the reason for that kind of behavior?


    High load, node point middle of busbar.


    Low load, node point middle of busbar.


Sign In or Register to comment.