numerical parameters - Modal analysis (Ansys Workbench) - eigenfrequencies too High! what to do?

[Matej_H]

My CAD geometry is defined as a circular thin plate in a 1:1 scale (so the same size as as the actual disk with D=300mm, thickness = 1,8mm). I tried both solid and shell elements.

The „inner“ part of the disk (up to D=100m) is clamped (for this purpose i tried various options, such as: fixed support, frictional support, compression only support, …). Material properties (temperature dependent) are set for Steel – meaning E (at 20C) =200GPa, Density= 8750kg/m3.

For the step No.1 – at normal „room temperature“ conditions - the calculated eigenfrequencies (e.g. modes 1 to 6) are about 40% higher than the measured ones. Why is there such a big difference?

Playing around with values for density and E (reducing both) resulted with slight decrease of frequencies, but, they are still about 30% to high.

For step No.2 (separate simulation model with the same CAD geometry) – I performed the transient thermal analysis (heat-loading only over a certain area of the disk), follwed by the static structural analysis (to calculate the structural response i.e residual stresses – at 750Mpa). In the last phase the Modal analysis was performed to evaluate changes in Eigenfrequencies (compared to results from a step No.1) due thermal effects.

Results of step No.2 show that modes 1 and 2 increased (slightly in addition to allready 30% too high values compared to No.1) due to the influence of residual stresses, whereas, higher modes (3, 4…) decreased due to same effects. Unfortunatelly, in reality or as meassured, it is the other way around – modes 1 and 2 tend to decrease, whereas, higher modes – 3 and 4- tend to increase.

The solution to my problem might be hiding in my material model - as I mentioned I have defined E (T), density is considered as constant,...flow curves are defined for elevated temperatures, etc

Thank you in advance! with best regards. Matej

Does anyone have any ideas of why this is happening? Any suggestion, help, a push in the right direction is more than welcome.
Best regards,

 

[NRP99]

Matej_H

You need to run nonlinear static structural analysis first with contact and material non-inearity and then modal called as pre-stressed modal analysis. But be careful to correctly set the contact settings. During modal analysis ANSYS will treat all non-linear contacts as linear one. Friction less is considered as no separation and frictional is considered as bonded contact. Contact stiffness setting will also have effect on natural frequencies meaning high stiffness settings can give high frequencies due to high contact stiffness in the overall stiffness matrix of system.

For more information check this link and this link.

 

[scheah]

Hi Matej,

It's worth giving Simply Supported a try. Fixed support is very difficult to enforce in real life.


Kind regards,
Jason

 

[NRP99]

Matej_H

Please ignore my earlier response. I misread your question. This response is valid for modal analysis after nonlinear contact structural analysis.

As Jason said, you can use simply supported condition for your analysis. But that is applicable only to line and surface bodies. Also the frequency results vary for surface and solid body approach since later is somewhat stiffer.

What do you say Jason?

If the 100mm diameter is clamped, you may consider 100 mm portion to be constrained in the vertical direction and circular edge at 100 mm diameter can be restrained at lateral directions. There will be variation in the frequencies as you change your support conditions which changes the stiffness of disk. So try different displacement constraint scenarios like above until you get the results matching with experimental values.

 

[scheah]

Simply supported first came to mind because it is significantly "softer". If these approximate boundary condition is not reasonable, modeling the details of the clamps may be the way forward.


Kind regards,
Jason

 

[Matej_H]

Thank you very much for your comments. To both of you! Also the comment about contacts will be very useful in the next few weeks.

Yes! "Simply supported" constraint proved to be a much better option for this problem. Eigenfreq. have reduced significantly! Values are however still a bit too high - but much closer to reality than before. I will also try to model the "clamps" as NRP99 described.

I still have the problem described as step No.2 in my initial question post. if a prestressed condition is applied to the disk - via structural analysis (following the transient thermal) resulting with residual stresses and plastic strains over a certain region of the disk, then results of Modal analysis show that Eigenfr. increase for the first few modes (compared to non-formed disk) and decrease for the higher modes. In reality it is the other way around. This may have to do something with material properties which are assigned to the model ( I guess :/ )

Thank you again.
best regards
M

 

[NRP99]

Matej_H

Difference may relate to correctly capturing the actual residual stresses and permanent strains which affects the stiffness and ultimately the frequency of disk.