🎉Community Raffle - Win $25

An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.
Join and Win

Base Motion in Modal Based Frequency Response.

User: "IRA_EM_21281"
Altair Community Member
Updated by IRA_EM_21281

Find more posts tagged with

Sort by:
31 - 60 of 892
    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    I assumed that bottom of the honeycomb is clamped I'm not sure if this is true or not.

    how to model this

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    it it is clamped, just add a SPC to it.

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    yes I have some results for this test

    I can only share results private message

    If you want to see I will send

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    for clamping you should just use SPCs at the base of your honeycomb.

     

    For all the connections between honeycomb and Jigs you could use TIE/FREEZE contact to bound parts together, and reduce computational cost, as you wouldn't need so finer mesh for the Jig.

     

    Dynamic problems, are affeted by mass and stiffness. If your masses are ok, then probably your stiffness and connections are not so good, or material properties are not correct.

    You need to compare first expected frequencies against numeric ones.

     

    That's all I can say to you. Maybe others can help you better.

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    for clamping you should just use SPCs at the base of your honeycomb.

    it is ok, I did what you said

    Dynamic problems, are affeted by mass and stiffness. If your masses are ok, then probably your stiffness and connections are not so good, or material properties are not correct.

    masses are ok, material tensile simuation were performed and compared tensile results are agreet to each other however when I use contact I could obtain close resuls and model with rbe elements is closer.

     

     

    Unable to find an attachment - read this blog

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    For all the connections between honeycomb and Jigs you could use TIE/FREEZE contact to bound parts together, and reduce computational cost, as you wouldn't need so finer mesh for the Jig.

    @Adriano A. Koga

    I should take into account thickness both rigid plate and honeycomb, should not I?

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    yes. Thickness needs to be there so that mass is also considered.

    While for contacts, usually you can define the Search Distance to guarantee that your contact is fully working. But the defaults usually work as well as they take into account your master plate thickness.

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    ok, I will share a new model

    @Adriano A. Koga I cannot define contact pls help

    Unable to find an attachment - read this blog

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    As you already have a rigid body in the lower plate, there's no need to use a material with so high Young's modulus.

    This could take to numerical singularities.

     

    Your constraints look strange to me, as your model is only constrained in X direction in the upper plate.

    As you use EIGRL V1 - 1.0, you will not see any rigid body modes, but they're there, meaning your model is not constrained.

     

    I've changed a little bit your contact definition and some material properties.

     

    But you should investigate further your boundary conditions. They should reflect what you have in your test. I assume the lower plate is the concrete base, and if so, it should be grounded. (create a SPC at the reference node of the rigid body)

    <?xml version="1.0" encoding="UTF-8"?>mode1.gif

    Unable to find an attachment - read this blog

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    thank you for all your all support but these numerical results no agreed to my experiments

    I obtained lower modal frequencies from the experiments

    Unable to find an attachment - read this blog

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    10% maximum difference for lower modes?

    it is not good, but not so bad, i would say.

     

    Your FEA model shows stiffer behavior, with frequencies consistently above the experimental results.

    If mass is correct, then, stiffness might be a little off.

    Sometimes material data is not 100%, or mabe the contact has induced a little more stiffness than desired.

     

    Another point, did you perform a mesh sensitivity analysis? probably refining your mesh would make it more flexible, thus frequencies would be closer.

     

     

     

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    Sometimes material data is not 100%, or mabe the contact has induced a little more stiffness than desired.

    I compared tensile simulation and tests and good agreed no problem.

    10% maximum difference for lower modes?

    the model you shared, is too different and never agreed with experimental results I would like to say that contact increase stiffness of the model

    I'm doing with rbe what you're doing with your contact algorithm I have shared experimental results and numerical results for you at ppt

     

    Whatever, thank you for all support

     

    I want to ask another question;

    in frf analysis, Can we see the behavior of the structure, for example displacement, at any frequency as a contour plot or how do we do it?

     

     

     

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    I don't get it. The model you shared is different from the PPT?? i'm confused here.

     

    your last model seems to miss the proper boundary conditions. You are running a normal modes but have not constrained the base. This is already a big issue, in my point of view, as you can see in the GIF i've sent before.

    I've only sent you a base contact configuration so that you adjust your BCs, specially a the base.

     

    Concerning FRF, yes, you will be able to evaluate displacements over your entire frequnecy range (requested), just like the graphs that you've sent in the PPT.

    There are a few tutorials in OS Help that shows the process.

     

     

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    actually, i've noticed that i was looking it upside down.

     

    Anyway, your upper plate has what total mass?

    I see a mass of 0.74Kg in your rigid body + the plate mass. What should it be?

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    I think a mistake was happened everyting was mixed I'm sorry,

    there are so many model files that they are all mixed up

    don't get it. The model you shared is different from the PPT?? i'm confused here.

    I the file I mentioned is attached its results are closer to experimental results

     

    see a mass of 0.74Kg in your rigid body + the plate mass. What should it be?

    I shared above but rigid mass dont 0.74 but 0.745

    Unable to find an attachment - read this blog

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    Concerning FRF, yes, you will be able to evaluate displacements over your entire frequnecy range (requested), just like the graphs that you've sent in the PPT.

     

    how to do it? which tutorials

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    lunch help, go to OptiStruct section, then you will find OptiStruct tutorials, and you will find them under Advanced Small Displacement Finite Element Analysis

    <?xml version="1.0" encoding="UTF-8"?>image.thumb.png.dc6f737eeb55edaaf169b053ee0ed7b8.png

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    did you looked at the results

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    I've changed your solid model to shell with contacts. Results are similar.

     

     Subcase  Mode    Frequency      Eigenvalue        Stiffness        Mass   
           1      1   3.965253E+01   6.207284E+04     6.207284E+04   1.000000E+00
           1      2   4.720448E+01   8.796828E+04     8.796828E+04   1.000000E+00
           1      3   6.231411E+01   1.532966E+05     1.532966E+05   1.000000E+00
           1      4   6.477586E+01   1.656480E+05     1.656480E+05   1.000000E+00
           1      5   1.310828E+02   6.783461E+05     6.783461E+05   1.000000E+00
           1      6   1.429535E+02   8.067697E+05     8.067697E+05   1.000000E+00
           1      7   1.267066E+03   6.338083E+07     6.338083E+07   1.000000E+00
           1      8   1.433586E+03   8.113483E+07     8.113483E+07   1.000000E+00

    Unable to find an attachment - read this blog

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    thank you for all my friend

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    /profile/97129-adriano-a-koga/?do=hovercard' data-mentionid='97129' href='<___base_url___>/profile/97129-adriano-a-koga/' rel=''>@Adriano A. Koga

    you have done what you suggested contact instead of utilizing of rbe greetings
    (Much obliged!)
    but I modelled rigid mass as four solid elements (CHEXA)
    numerical results agreed with experimental results.
    I want to conduct an optimization study to optimize the thickness of the specimen
    when a contact algorithm was installed between rigid mass and the specimen, and I leave a gap by 0.5 mm ( this value is half of the specimen thickness). My problem begins here. Since I purpose to optimize the thickness, I want to define the gap value as a function of the thickness (for example, t/2)
    how to solve this problem

    best regards and thank you for replies

     

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    hi /profile/32816-durukanbdilek/?do=hovercard' data-mentionid='32816' href='<___base_url___>/profile/32816-durukanbdilek/' rel=''>@durukanbdilek 

     

    The t/2 correction is mostly valid for full NL contact analysis.

    In your case, if I recall correctly, you're using FREEZE/TIE contact, so this small difference won't be so important in your model.

     

    For optimization use the gauge optimization, and take care on defining well your optimization problem so that you get what you expect. (just like any other analysis, in optiization if you don't define it correctly, garbage results will be generated).

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    The t/2 correction is mostly valid for full NL contact analysis.

    In your case, if I recall correctly, you're using FREEZE/TIE contact, so this small difference won't be so important in your model.

    no problem in this part, numerical and experimental results were agreed with each other.

    Look, I want to realize an optimization study and I want to use thickness (t) as a design variable do you understand me

    I would like to define the gap, between mass and specimen as a function of the specimen thickness (gap=t/2).

    how to define this parameter and this function or has hypermesh such as possibility ?

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    But your specimen is tied to your piece? If it is tied, like I said, the difference is expected to be low.

     

    Anyway, of you want to be 100% accurate, yes, you can combine both things.

    You will have 2 design variables:

    - size/gauge desvar for T

    - shape desvar translating your specimen (let's say unit translation in thickness direction)

     

    Coupling of the 2 desvars can be acomplished by desvar link (dlink).

    You can link the 2 desvars by a simple linear expression, by using translation_shape = 0+ 0.5*thick_desvar

     

     

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

     

    But your specimen is tied to your piece? If it is tied, like I said, the difference is expected to be low.

    yes, I made tie contact. experimental and numerical results agreed

     

    Anyway, of you want to be 100% accurate, yes, you can combine both things.

    I got what I want..

     

    - size/gauge desvar for T

    the problem is optimization I have only one variable is thickness of specimen  because I want to define the gap as a function as thickness

     

    I have a model file but its size is very large how to send to you

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    I will say again..if you're using tie contact, the gap shouldn't be that important in your analysis.

     

    If you really want to go further with this, i've already described what you need to do:

    But your specimen is tied to your piece? If it is tied, like I said, the difference is expected to be low.

     

    Anyway, of you want to be 100% accurate, yes, you can combine both things.

    You will have 2 design variables:

    - size/gauge desvar for T

    - shape desvar translating your specimen (let's say unit translation in thickness direction)

     

    Coupling of the 2 desvars can be acomplished by desvar link (dlink).

    You can link the 2 desvars by a simple linear expression, by using translation_shape = 0+ 0.5*thick_desvar

     

     

     

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    If you really want to go further with this, i've already described what you need to do:

     I intent to optimize the thickness (t) for transmissibilty(a(out)/ain) where a is acceleration or displacement.

     

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

    You can create your desvars as described before, and for responses tou can create 'frf acceleration'.

    Just take care when using a frf responses as you need to think well if this would be an objective or design constraint.

    As you will have a vector (amp x freq) you need to correctly define this, if you want a specific frequency, or a maximum value, etc..

    User: "durukanbdilek"
    Altair Community Member
    Updated by durukanbdilek

    You can create your desvars as described before, and for responses tou can create 'frf acceleration'.

    that is ok. I need conduct the FRF analysis. I agreed.

    as objective function, I want to optimizie the transmissibility curve which can be obtained from frf analysis of the model

    a curve can be obtained as figure

    resim.png.13abb62e4d760ebcc0accb868e56e541.png

     

    In the analysis, I run a range of 10-100 Hz. For example, I aim to access 0.1 at 90 Hz by altering of t (thickness) or other parameters (in necessary)

    Is this possible?

    also I want to sent to you my model file, whose size is  90 Mb  how to sent it

     

     

    User: "Adriano_Koga"
    Altair Employee
    Updated by Adriano_Koga

     

     

    You could calculate your transmissibility by using advanced dresp2 or dresp3 with Compose.

    Dresp2 allows you to create an equation and use this as objective or constraints. 

    Take a look at OptiStruct help for more details.

     

    As for the model you can zip the fem file. It would get smaller.

     But i don't have access to my computer now. Sorry.

31 - 60 of 892