Modal Analysis on PCB

  • Last Post 18 June 2019
Arvind posted this 09 May 2019

Hi. I would like to perform modal analysis on the attached PCB in order to find the natural frequencies and determine the mode shapes at those frequencies. With regards to the design of the board, there are 4 holes through which they are secured on to a fixture on the base plate and the board is excited by means of an electrodynamic shaker. I designed the board in SolidWorks and imported to ANSYS. I edited the Engineering Data by adding the material:FR-4 and selected the linear elastic option - Anisotropic elasticity. I exported the model to Mechanical Analysis. I fiddled around the geometric mesh spacing, fixed supports option under Modal (A5) but I got nowhere closer to the results from experimental technique. Please advise. Your help in this regard is highly appreciated.PCB design

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 09 May 2019

1) What was tested, a bare PCB board or one with components on it?

2) What is the exact mass of the PCB board when you weigh it?

3) What is the mass of the model reported by ANSYS in the Details window when you click the body?

4) What does the fixture look like that fastened the PCB to the shaker table?

5) Make an ANSYS Modal model of the fixture without the PCB, what is its first natural frequency?

6) Show the material properties for FR-4 and say which component is through the thickness and which is in-plane.

7) Why anisotropic and not orthotropic material?

7) How was the first natural frequency experimentally determined on the shaker?

8) The geometry of the PCB should be a surface that is assigned a thickness in Mechanical, not a solid.

9) When you use shell elements with orthotropic materials, you need to override the element coordinate system.

This post is without the override, the next post shows how to override. You don't need this with solid elements.

10) If you used a solid model, please show the mesh. There should be at least 2 elements through the thickness.


  • Liked by
  • jj77
Arvind posted this 10 May 2019

Thanks for your response. Please find my reply as follows:

1. Both, bare board and assembled board were tested but I would like to start with a bare board. Hence, in this case I'm using a bare board.

2. 97.3 g.

3. 88.09 g.

4. Please find attached image. The board is normally rigidly fastened on the vibration platform. (Image only for reference)

 Board mounted on fixture

5. Previous studies have considered only the board for modal analysis, and not the fixture. Should I still go ahead and analyze the fixture?

6. Please find attached.

FR4 Material Properties

7. By performing a random sweep.

8. I have used a Solid model here.

9. Okay.

10. Please find attached.

Hope, my response satisfies your queries. Please let me know if you need additional information.

peteroznewman posted this 10 May 2019

2) If the model mass is 88 g but the part mass is 97.3 g you should multiply the density of the material by 97.3/88 to get the model mass to match the physical part.  What is the mass of the accelerometer?  You can add a point mass at the center if you slice your model with two planes to make an edge through the thickness to attach the point mass to the center of the board. 

6) Do the material axes correctly correspond with the orientation of the sheet in the global coordinate system?

7) Do you mean a sine sweep?  Please show the frequency response plot from the accelerometer mounted at the center of the board.  Can you estimate the damping from that plot?  Does the software output the Q value or the damping ratio?  What is the measured first resonance frequency?

11) I forgot to mention that you should measure the thickness of the PCB on four edges using a micrometer and adjust the thickness of the solid to the measured value. You will have to tweak the density to get the mass to match if you had to change thickness.

Once you have adjusted the density, added the point mass and rerun the Modal, what is the undamped natural frequency from ANSYS for Mode 1?  If you enable Damping in Modal and enter the measured damping ratio, what is the damped natural frequency from ANSYS Mode 1?


Arvind posted this 13 May 2019

2) After your comments, I multiplied the density by approximately 1.2. I didn't notice a significant change in the results. For this test, accelerometer was mounted on the base plate and not on the PCB.

6) Yes

7) We used a laser vibrometer to measure the response signals and the first 4 natural frequencies were at 118 Hz, 326 Hz, 491 Hz and 627 Hz whereas with FEA, the first natural frequencies are at 110 Hz, 160 Hz, 299Hz, 369 Hz, 394 Hz and 399 Hz. The displacement at 118 Hz from experimental technique was at 0.103 mm whereas the displacement at 110 Hz from FEA technique is 6.41 m which is extremely high. I'm not sure the software gives a Q value but we did a search and dwell test to find the natural frequency with a Q factor of 10.

I wasn't able to compute the data with Num Cells Across Gap = 2, instead I used a value of 1. With the former value, I was receiving an error message due to long time duration taken to process the data.

Thanks again for your response.

sk_cheah posted this 13 May 2019

Hi Arvind,

I would approach this problem a bit differently. 

First get the natural frequency and mode shapes of a free-free boundary condition (rubber bands). This boundary condition can be more accurately replicated in your model (unconstrained). You can then tweak your stiffness and mass parameters of your PCB to properly replicate your model. 

Armed with your updated model, add the boundary conditions of your shaker. If fixed boundary conditions at the holes doesn't work, you may need to include the model of your fixture. 

Also... make sure you are able to measure and plot mode shapes from your experimental data. This would help you associate the test modes to analytical modes that are computed. 

Finally, 6.41m FEA results indicates something is wrong in your model. Best to spend some time troubleshooting by solving a known problem to check your answers. 

Kind regards,

  • Liked by
  • peteroznewman
Arvind posted this 14 June 2019

Hi Folks,


I have a query regarding the analysis results (please refer attachment – analysis results). The first 4 natural frequencies obtained on FEA technique was 112, 162, 305 and 374 Hz, whereas the experimental technique produced 118, 326, 491, 627 Hz as the first few natural frequencies. All the properties considered – material properties, analysis settings, fixed support, mesh sizing have been attached for your reference. In order to get the values closer to the experimental technique, what properties do you reckon I can try modifying?

Analysis resultsAnalysis settingsFoxed support constraintMaterial propertiesMesh sizingPart properties in modal analysis tool


peteroznewman posted this 15 June 2019


The first mode has good agreement, but the second mode does not.  The reason may be because the second mode has a vibration node at the center of the board where the accelerometer is mounted, so that cannot see the second mode.  The third mode has some displacement at the center so the modal result of 305 Hz is compared with the experimental 326 Hz.

The modal frequencies are a little low, so you could increase the thickness of the board in the model slightly to increase the stiffness and raise the modal frequencies. Another way to add some stiffness to raise the modal frequencies is to increase the size of the circle where the fixed supports connect the PCB to the shaker table. If the PCB geometry has the hole the fastener passes through as the fixed support, increase the hole diameter to equal the standoff or the washer or screw head on the top.

Arvind posted this 17 June 2019

Thanks for your input, Peter. It was helpful!

Per your suggestion, I increased the hole diameter to match the screw head along with slight increase in the thickness of the board. During this process, density of the board was modified accordingly to match the mass of the PCB. Results obtained are attached:

Also, to obtain the Frequency Response Function, an accelerometer wasn't used in the test, instead a laser vibrometer was used. Hence, I am able to comprehend why there would be difference starting second mode of the structure. Is there any other factor that is required to be incorporated?

peteroznewman posted this 18 June 2019

It looks like you have fairly close agreement between the experimental and modal frequencies now.

If you are doing an analysis such as Harmonic Response, you will need to enter some data for damping. What will you use for damping ratio?