# Free Modal Anaylsis

Member

I am trying to perform a free modal analysis on a 3U CubeSat. In this model, no fixed supports were introduced. For the attachment of the side panels to the rails (4 long slender components), I used a bonded contact with the formulation MPC as shown in the second screenshot. I used pinball radius at the holes of the side panels. In this first model there is a top plate shown in the 4th screenshot but no bottom plate as shown in the 3rd screenshot. The results I got for the eigenfrequencies make somehow sense as it is expected that the eigenfrequencies for the first 6 modes are 0. BUTTT!!

After introducing a bottom plate, PCB with 2 connectors, connector at side panels in Pic 3, using bonded contact with same formulation as above & point mass, the eigenfrequencies I got are 0 for all 9 modes and this phenomenon starts occurring, the PCB is detached from the connectors which does not make any sense as is it supposed to be intact because of the bonded contacts as shown in the second last picture. Last picture shows properties of point mass defined. The reason for using point mass is because the PCB contains other electrical components in itself.

Could anyone explain why this is happening. Cant seem to figure out. Thank you in advance!

• Member
edited October 2020

@purichmunlow Thank you for writing up a detailed question, it makes it easier to answer.

Under 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.

If it is shown as Closed, Suppress the Point Mass and solve, the PCB/Connector should stay attached. Is that true?

In that case, with Point Mass Unsuppressed , you should find a message in the Solution Output about a conflict.

The 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.

• Member
edited October 2020

@peteroznewman Thank 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?

• Member

@peteroznewman The above figure shows the electrical components on the PCB, which I modelled them as a point mass. Should the point mass not be distributed throughout the whole PCB like how I did earlier?

• Member
edited October 2020

A 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.

Thank 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.

Do 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.

• Member
edited October 2020

@peteroznewman Thank 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.

Warning message concerning the conflicting conditions.

After 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?

• Member
edited October 2020

@purichmunlow

If 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.

If 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.

I 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.

• Member

@peteroznewman 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. :)

• Member

@peteroznewman Hi Peter. Did you perhaps make any progress? :)

• Member
edited October 2020

Here is the way I used to add "non structural mass" to a structure.

Create 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.

If you have three boards, you will need a unique material for each board, assuming they have different populated masses.

This 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.

=== Modal Results ===

Here 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.

Modes 1-6 are all rigid body modes as you can see from the deformation animation.

I 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.

• Member

peteroznewman 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?

• Member
edited October 2020

I'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.