June 21, 2023 at 9:59 amBALASubscriber
As from the ansys innovation course i found the answer for this as below
- 1.5 times to highest frequency it is exposed to
- Ratio of effective mass to total mass should be equal to 90% or more
I have followed this guidelines but in my case in one of the direction the ratio of effective mass to total mass is not getting even 50% , for other two direction i am getting almost 80%. Now my question is how many modes i should extract bcz even if i am increasing it will just increase resut file size. I searched for the method like residual vector but this only works in transient not in random vibration, Please help
June 21, 2023 at 3:54 pmAkshay ManiyarAnsys Employee
I guess you have checked the below video from AIC courses which talks about how many modes need to be included.
Do you know the frequency range for the assembly in which it will be operated? Also, what is the direction of excitation?
June 22, 2023 at 9:26 amBALASubscriber
Yess i have checked the same video. My frequency range which is Random vibration profile is betweeen 20 to 2000 Hz and direction is all three directions applying individually in X,Y and Z.
June 21, 2023 at 4:09 pmBALASubscriber
Dear Sir, Thank you for reply. As i already mentioned about these perticular video in my question itself that i did follow guidelines given. As per the video we have extract the modes till we the ratio of effective mass to total mass equals to 90%. But in my even if i am extracting more number of modes my ratio is not going more than 50% for one perticular direction . As in video it is suggested to use residual vector or missing mass method (this method is not explained how to do in video) but this is applicable for Response Spectrum or Transient dynamic but i am performing MSUP Random Vibration analysis so that is why I am asking what i can do for this situation.
June 22, 2023 at 12:14 ampeteroznewmanSubscriber
Please post an image of your structure and make sure the Global Csys triad is visible so we know which direction is which. Show the mesh. This may help us understand why there is only 50% participation in one direction. Also say which direction that is.
June 22, 2023 at 9:49 amBALASubscriber
Dear Sir, Thank you for reply. Sir due to some confidentiality issue i cant post on it, but i can tell that my structure is electronics enclosure assembly which has pcb and other components in it. As my modal was getting so big with quad elements i have to reduced it by using linear element , as i have used Multizone (hexa core) method for some part it has created the lower order pyramid elements. i have used quad element for those part which is meshed using tetrahydron patch conforming method. the max aspect ratio i am getting is almost 220 and avg is 2.8.
June 22, 2023 at 9:15 pmpeteroznewmanSubscriber
PCBs and enclosures are thin-walled parts. The best practice for modeling those are to reduce the parts to midsurface models that are meshed with shell elements. You can imprint the outline of the larger, heavier components onto the PCB and create a remote point on each outline to attach a Point Mass to represent each of those components. You can use a Distributed Mass on the remaining area of the PCB to smear the mass of the smaller, lighter components over the PCB to get that up to the correct total mass.
The enclosure should also be a midsurface and meshed with shell elements. Is the enclosure a box shape? Are the seams welded or screwed together. If welded, then those surfaces should meet at a clean corner. If screwed, then you need to use a Fixed Joint to hold the edges of the two holes. You could use Remote Points to define one side of the Fixed Joint and add a Point Mass to represent the mass of the screw.
One component that is convienient to leave as solid are the stand-offs that hold the PCB above one face of the enclosure. It is best if some features of the stand-offs, such as holes and chamfers are deleted from the geometry so that the part becomes a sweepable body. The cleaner geometry will allow better solid element shapes to fill the volume. I doubt you need to impose a Patch Conforming mesh control, you will get better element shapes if you don’t impose that and probably don’t need to maintain the details of each and every face on the solid body. Bonded Contact can be made between each end of the stand-off and the enclosure or PCB, even though there is a 1/2 wall thickness gap at each end, by turning on the Thickness Effect in the contact. Set the behavior to MPC so you can see the spider of elements holding the parts together after the model is solved.
Once you have done all this geometry clean-up, you will get much better element qualities and by replacing solid meshed components with shell elements and Point or Distributed Masses, you will have a much smaller model.
Solid elements must be Quadratic and not Linear unless you have a pure Hex mesh. Linear Tet or Pyramid elements are overly stiff and do not give accurate modal results, especially if there is only one or two elements through the thickness of a thin walled part.
I can’t imagine the geometry of a PCB and its enclosure to be an issue for confidentiality, but that is entirely up to you.
June 23, 2023 at 2:40 pmBALASubscriber
Thank you very much sir for your detailed response, this is very helpfull for me.
Seams are screwed together in my assembly, if i am using shell bodies which one option i should use fixed joint or Beam connection to hold these parts. I tried both( on just two plate connected by bolt) but result are very different in both cases, for beam connection i have referred your youtube video which was for solid parts (thanks for this also). With beam joint, two plates are rotating about beam in one of the mode shape. More important point here when using beam joint the plate are rotating in apposite directions which they should not. Also if i need use solid bolt (for accuracy) then using this with shell enclosure means there will be actual a edge -surface contact for bolt shank and enclosure. What we can do this for situation.
fig. Beam Connection
Fig. Mode shape result with beam connection
Mode shape for fixed joint
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.