October 10, 2020 at 9:29 ampurichmunlowSubscriberOctober 10, 2020 at 12:52 pmpeteroznewmanSubscriberThank you for writing up a detailed question, it makes it easier to answer.nUnder the Connections folder, insert a Contact Tool and Generate Initial Contact Status. You expect to see all the contacts Closed. Is the contact between the PCB/Connector shown as Far Open? If so, then you need to increase the Pinball Radius on that contact. nIf it is shown as Closed, Suppress the Point Mass and solve, the PCB/Connector should stay attached. Is that true?nIn that case, with Point Mass Unsuppressed , you should find a message in the Solution Output about a conflict.nThe corrective action is to separate the faces needed for bonding the PCB to the Connectors from the face needed to attach the Point Mass. You could imprint the shape of the Connectors onto the PCB, then imprint a square in the center of the PCB to connect the point mass, that way you will have four faces and none of them touch each other. You will end up with two contacts, one for each connector. Then you should get what you expect.nnOctober 11, 2020 at 1:44 pmpurichmunlowSubscriberThank you for the answer, Peter. Your predictions were right. The PCB/Connects stayed attached when I suppressed the Point Mass and when it is unsuppressed, a warning message about a conflict popped up. Why is that. An explanation would be appreciated. Regarding the imprint of a square in the center of the PCB for the point mass, I did not quite fully understand. Is it like what is shown in the screenshot below? How big should be the imprint of the square? The four faces you mentioned, are 2 imprints of connectors, square imprint in the center, remaining face of the PCB. Am I right? Could you perhaps explain why the phenomenon I described earlier happened with the method I at the beginning? nnOctober 11, 2020 at 3:00 pmOctober 11, 2020 at 5:50 pmpeteroznewmanSubscribernA more accurate model would be to imprint the two large chip outlines onto the pcb surface. Then you can add a point mass of each chip. There are two choices when adding point mass. If you choose Behavior = Rigid, you will also insert an area of rigidity into the surface. This will increase the natural frequency. If you choose Behavior = Flexible, that will add no additional stiffness and decrease the natural frequency. I recommend you run this model twice and report the range on the natural frequencies.nThank you for the photo of the pcb populated with components. Find out exactly how much that populated board weighs. Subtract from the mass of the populated board the mass of the two chips that you will add as point masses, call that mass Mp. In the model, you have defined a density for the pcb material, call that Db. Mechanical shows the mass of the pcb body, call that Mb. You want the pcb body in Mechanical to show up with a mass of Mp. Therefore, multiply the density of pcb in Engineering Data by the ratio of the masses and type in a new value for the density of the pcb material. The new density for the pcb material is Db*Mp/Mb. After you do that, Mechanical will report the mass of the pcb body as Mp. When the two point masses are added in, the total mass will equal the mass of the real populated part.nDo a Google search using the exact text of the warning about conflicting conditions in the model and you will find some information. If you provide the exact text, I can help some more.nOctober 11, 2020 at 7:15 pmpurichmunlowSubscriberThank you for the detailed reply and insights on how to model the above figure. I have thought of this and consulted this with my supervisor. He mentioned that it is not necessary to model the PCB in detailed as the mass of each component on the PCB is very small. Moreover, we do not have the information of mass and location of each component on the PCB. So the proposed approach to model this is to add a point mass that represents the total mass of the components at the C.G. of the PCB. But you mentioned earlier to create a square imprint in the middle of the PCB. My question is how big should this imprint be? Since as shown in the above figure of the PCB. Should the point mass not be distributed throughout the whole PCB's surface as shown in the below figure? The setting of the point mass is shown in the above screenshot. nWarning message concerning the conflicting conditions.nAfter implementing the changes except the imprint for point mass according to your advice, the phenomenon that I described earlier (Connectors detached from PCB) is gone now. But I still don't understand why the eigenfrequencies for mode 4, 5, 6 are not 0. It should be isn't it? Since it is a free modal analysis? Is there an explanation behind this?nnOctober 11, 2020 at 11:55 pmpeteroznewmanSubscribernIf you adjust the density of the pcb material to account for the components, you don't need a point mass at all. One advantage of adjusting the density is that it spreads the mass of the components over the full area of the pcb board. Another advantage is there are no conflicts. One newer feature in Mechanical is Distributed Mass, where you pick a face and it distributes the mass over the area of the face. I don't think that creates any conflicts, but I haven't used this feature yet, so if you use it, you can see if the conflict goes away.nIf you insist on a point mass, then you have the right idea on the face in the center. Just make sure to use Behavior = Flexible. Any size face is acceptable.nI don't know why the Free-Free modes are not zero for all six modes. Perhaps the model has an unintended connection to ground. I would be happy to check the model out if you attach a zip file containing the Ansys Project Archive .wbpz file and say what version of Ansys you are using.nOctober 12, 2020 at 2:20 pmpurichmunlowSubscriberArray Thank you for the explanation Peter. Here is the link to the Ansys Project Archive. https://drive.google.com/file/d/17OawW-uG_8_a7jy1SvsLijDf2EQ27cF0/view?usp=sharing. The version I am using is 19.2. I have create two seperation models. One is with distributed mass and the other one is with point mass. If you have the time, could you create another model with the methods you mentioned with adjusting the density in the file as an e.g.? I did not fully grasp it. Thank you in advance for your help. nOctober 14, 2020 at 10:09 pmpurichmunlowSubscriberArray Hi Peter. Did you perhaps make any progress? nOctober 15, 2020 at 12:25 pmpeteroznewmanSubscriberArraynHere is the way I used to add non structural mass to a structure.nCreate a copy of the material called pcb and call it populated pcb. Where the density was 2.364 g/cm^3, type in a new value of 3.873 g/cm^3.nIf you have three boards, you will need a unique material for each board, assuming they have different populated masses.nThis is the old school way of adding distributed mass. Now they have a the distributed mass in the Workbench interface, it probably isn't necessary anymore.n=== Modal Results===nHere is mode 7, the first bending mode. Are those panels supposed to be free to bend like that or is a contact missing in the model? Try fastening this panel and rerunning Modal.nModes 1-6 are all rigid body modes as you can see from the deformation animation.nI don't know why the frequency ratio between mode 6 and 7 is not larger. The ratio should be greater than 100. It is only 4. Maybe someone else has a comment.nOctober 19, 2020 at 4:47 pmpurichmunlowSubscriberpeteroznewman Thank you for the clarification. I still do not understand why the eigenfrequency for mode 1 to 6 is not 0. I thought they should be 0 since the model is not constrained? Another question is what is the reason behind the frequency ratio greater than 100 between mode 6 & 7?nOctober 19, 2020 at 5:23 pmpeteroznewmanSubscriberI'm not sure where the check that ratio of frequencies of rigid body modes and the first bending mode at mode 7 had to be larger than 100 came from, but in most models, it is very easily achieved.nViewing 11 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.