I am currently doing the analysis of the frequency response of the nonlinear vibration with flexible PCB by using the module transient structural. But the problem is that I always get the linear results, I turn on the large deflection and nonlinear effects, I use the nonlinear mechanical with the element order of quadratic and the sizing function of adaptive to do the mesh. could someone give me some help, I had tried for a very long time, while I still did not get any satisfactory results.
How to do the frequency response of the nonlinear vibration of a flexible PCB?
- 1.6K Views
- Last Post 20 September 2018
- Topic Is Solved
Here is a relevant discussion on a student who wants to build a simulation of an object on a shaker table. You might find that interesting.
First observation on opening your file, looking at the Transient Structural, you have a mesh that is much finer than necessary to study frequencies up to 200 Hz. I changed the max face size from 0.1 to 1 mm and deleted the Face Meshing - Triangles. The finer mesh makes you wait longer for a solution, without giving your any benefit in higher accuracy. Not sure why you thought Triangles were better than Quad elements. They are not.
Second observation, delete Fixed Rotation 2 on the face. That is not needed. You only need the ends.
After making the above two changes, I added a Modal analysis to the Transient Structural, and found the first undamped natural frequency is 264 Hz. From your Harmonic Response analysis, you are interested in 80 - 200 Hz range of frequencies. If this is the range of interest, then there won't me much response in this range. The third change I made was to change the thickness of the sheet from 0.5 to 0.125 mm. Now there are at least a few modes that are between 80 and 200 Hz.
From your Transient, you were wanting to perform a sweep over the 80 - 200 Hz range in 10 seconds.
You can apply the displacement directly to the edges as you have done. However, you must provide a minimum of 10 and preferably 20 data points per period in the input data to faithfully reconstruct a smooth signal. Since you are going to 200 Hz, that means you should have between 2000 and 4000 data points in the last second. You have only 500 data points for the entire 10 seconds, entirely inadequate! At a constant 4,000 Hz sampling rate, you will end up with 40,000 data points for the 10 second sweep.
The very first cycle has an effect on the high frequency transients you can introduce unwittingly to the simulation. If you use a sine function on the displacement, at time zero, you create a step change in velocity, which introduces high frequency noise into your results. This will die out due to damping, but your first fraction of a second will not have the valid data you want. If instead you use a cosine function, the displacement and velocity can be zero at time zero, and the velocity can ramp up (in a sine function), and you will avoid generating high frequency noise into your results. Your displacement function has a displacement of 5 mm at time zero. That is not where you want to start. You want displacement of zero at time zero. See this post for an example.
On a shaker table, the sine sweep is usually based on acceleration, not displacement. The reason is that the acceleration required to have a 5 mm amplitude is much higher at 200 Hz than it is at 80 Hz. Where did the 5 mm amplitude come from? That is huge at these frequencies. At 80 Hz, the board will experience 129 G of acceleration, while at 200 Hz, a 10 mm peak-to-peak displacement requires 805 G of acceleration. I'm sure that is not what you want. Here is the calculator I used.
Let's say you want 5 G of acceleration applied over the range 80 - 200 Hz over a 10 second time. I have a signal generating script that runs in matlab that is part of a package called vibrationdata by Tom Irvine.
This generates an acceleration signal, which can be double integrated to displacement using another script. Notice how the displacement is reduced as the frequency increases over time.
Attached is a zip file and inside is a text file with the displacement data from the graph above.
It's not based on the sigSweep external load function. I don't know what units that function is using.
One more idea: you can use fixed supports at each end and have an acceleration load, which is the original data that was generated by matlab before I double integrated it to displacement. I can provide an acceleration file or a displacement file with different settings if you want.
If you have no nonlinear materials, then you can put a Modal analysis first and feed that solution into the setup cell on the Transient Structural, then run the linear MSUP transient solution, which may run a bit faster. The Transient Structural will take an Acceleration load, but not a non-zero Displacement if it is using the MSUP solution.
Here is a good article. It is written with examples in another product, but the lesson is the same.
My guess is that you don't have any geometric nonlinearity for normal levels of vibration. If you have extremely high levels of acceleration, then you could get to a point where a nonlinear analysis would give a different result, but is that your intent or are you more interested in fatigue life estimates?
SINE vs COSINE
If you have fixed edges and use an acceleration load, then it is better to have a sine function so the acceleration ramps up from zero at time zero If you have edges with a tabular displacement input, then it is better to have an offset cosine function so that displacement and velocity at time zero are zero and ramp up from there.
TIME HISTORY SAMPLES
Having 40,000 time history data points is not taxing on your lowly laptop. Solving the Transient Structural without the Modal Solution and the linear assumption makes a lot more work for your laptop.
SHEET BODY MODEL INCLUDING ICs
You can slice your PCB sheet body to make an interior rectangle to represent the IC chip. You can assign a thickness, and even a different material to the interior rectangle. You can adjust the density of the IC material so that the mass of the interior rectangle matches the true mass of the two IC chips. Do you know how to Slice in DesignModeler, then make a multibody part to reconnect the two bodies into one part?
How does the IC connect to the PCB? Is it a Ball Grid Array? If so, in a very detailed model, you can model all the balls and compute the stress in the corner balls that will have the highest stress due to the bending of the PCB from the corners out.
I have read one of the most cited books, "Vibration Analysis for Electronic Equipment" by Dave S. Steinberg. He has a lot to say about PCB vibration and how to estimate the fatigue failure of IC chips mounted to the PCB under various vibration conditions. You should read it.
Having read that book, I wonder if a fixed support that includes clamped edges is realistic for your model. What is clamping the edge which such force that it prevents rotation? If the edge of the PCB card slides into a spring loaded channel, under vibration, there is little to no rotation constraint. It would be more realistic to model it as fixed displacement, but leave the edge rotation free.
1. You have done in SpaceClaim what I described as a Slice operation in DesignModeler, that is to create two surfaces. The last step is to set the Share Topology to Share. That means the mesher will have shared nodes at the common edge to hold the parts together.
2. For a displacement condition, it is an offset cosine. So the displacement would be
which is zero at time equals zero. The displacement varies between 0 and -2A.
3. As the amplitude is increased, the deviation between a linear and a geometric nonlinear solution will diverge. It doesn't hurt to turn on nonlinear effects even when the amplitude is low, it just may add extra time to the solution. Where requiring nonlinear hurts when you don't need it is when it eliminates a fast solution method such as Modal Superposition.
4. You can certainly get a nonlinear geometric effect with a surface model. It only depends on how large the amplitude of vibration is for a difference to show up. The difference may shows up because of the membrane tension that stiffens the board as it deforms due to the fixed supports on opposite edges of the board. You can use a Static Structural analysis to plot the peak deformation as a function of pressure for a linear and a nonlinear (Large Deflection) analysis. That will illustrate the size of the deformation where a significant deviation occurs.
5. The mesh can be quite low density when there are only a few modes in the frequency range of interest. As long as there are at least 10 elements along a deformed wave in the part, that is plenty.
6. Okay, good.
I see in the sketch that the clamping bars, if they are fixed by bolts or screws that are torqued down tight, that may indeed constrain rotation of the edges.
1. I had the sense that the two ICs were mounted on opposite sides of the PCB and occupied about the same area. In this case, the rectangle in the center of the PCB surface represents both ICs and has a density sufficient so that the mass of that center rectangle has the mass of that part of the PCB plus both ICs. There won't be three bodies but just two bodies.
2. You can see that the solver was heading for convergence on that last step, it it had just not quit after 26 iterations. That is where you introduce a Command item into the Transient Structural branch (not the Solution branch). Click the Insert Commands button,
Then type the command: NEQIT,60
This tells the solver to keep iterating for 60 attempts instead of the default 26.
3. No problem.
4. I don't think the PCB needs any plasticity or any nonlinear property. A linear isotropic elastic material is sufficient for this model.
In your Static Structural model, add an Acceleration of 250 m/s/s in the Z direction. Change the BC on the two edges to Fixed Supports. Solve with 25 minimum substeps with Large Deflection On and Off and you will be able to create this plot. This is the geometric nonlinearity you wanted to see.
1. There are three types of structural nonlinearity: material, contact and geometric (large deflection). You can turn off geometric nonlinearity, but still have material or contact nonlinearity in the model. But if you have only linear (or no) contacts and only linear materials, then when you set Large Deflection Off, then you have a completely linear model.
I don't know what you mean by "besides, what is the meaning of turning on the nonlinear effect and thermal strain effect?"
2. Even with linear materials, there is a false stress as explained in the article above, due to large rotations in the solution that are not being properly computed. When Large Deflection is Off, the small angle assumption is used to make the computation faster. When you turn on Large Deflection, large rotations are handled properly, which takes more time to compute but then a large rotation of a sheet will not generate a false stress. In a model like yours or the skin on a drum head, even though the rotations may remain small, the deformation in the Z direction when solved with Large Deformation turned on adds tension to the drum, which reduces how far the drum head deflects under a given load. If you turn off Large Deformation, then no tension is added and the drum head deflects much more than happens in reality. That is the effect I made the plot for in my previous post.
3. You can have two ICs in the 2D model. That rectangle in the middle is assigned a different thickness and a different material than the PCB picture frame body. That rectangle in the middle represents two ICs and the PCB between them. The mass of that rectangle must equal the sum of the two ICs and the piece of PCB between them.
1. A basic structural dynamics linear material needs density, and isotropic elasticity, which is Young's Modulus and Poisson's Ratio. You can add a nonlinear property like Plasticity, or if it is already there, you can delete the nonlinear property. There is no turning it off, just either add or delete the nonlinear property.
2. Sorry that I repeated the same explanation I used previously; that wasn't helpful.
Do you know the game of checkers? There is a checkerboard and pieces occupy squares. Some squares are empty, some have one piece on it, and some squares have a stack of two pieces on one square.
Now let's build a 2D model of that checkerboard. Take a large surface and slice it into an 8x8 grid of squares. Each square is going to be assigned one of three different materials. Let's call the materials: Empty, One and Two. Each square is also going to be assigned a thickness.
Let's say the board is 2 mm thick, and the pieces are 4 mm thick. Assign a thickness of 2 mm to the empty squares, a thickness of 6 mm to the squares that had one piece on them, and assign a thickness of 10 mm to the squares that had two pieces on them.
Let's say that one empty square of checkerboard weighs 3 grams, and each piece weighs 5 grams. When you create the material called Empty, you have to adjust the density of the material until that square surface that has been set to a thickness of 2 mm shows a weight of 3 grams. Similarly, the material called One is assigned to a square surface that has been set to a thickness of 6 mm and you have to adjust the density until that surface weighs 8 grams. Finally, the material called Two is assigned to a square surface that has been set to a thickness of 10 mm and you have to adjust the density until that surface weighs 13 grams.
At the end of building this 2D model, there will be a grid of surfaces, where each surface represents either an empty square, a square with one piece on it or a square with two pieces stacked on it. The total mass of the 2D model will exactly equal the mass of the real 3D checkerboard with the pieces on it, and the distribution of mass over the 2D surface area will closely represent the true distribution of mass over that area.
This same method can be used to make a 2D model to represent the mass and stiffness of a PCB where there may be two ICs on opposite sides of the board at one location. A more complicated board that had a single IC at another location would require a third material definition. The cutout in the board is in the shape of the IC but it is the material and thickness assignment that defines whether there are zero, one or two ICs on that cutout.
I see you have two surface bodies.
- Body Thickness Material Mass
Outer 0.15 mm substrate 0.454 g
Center 2.68 mm IC chip 1.239 g
The bending stiffness of a beam depends on the factor EI, where E is Young's Modulus and I is area moment of inertia.
While both materials have the same value of E, 5000 MPa, they have very different thickness values. For a rectangular cross section of thickness t and breadth b, the formula for I is bt^3/12. So you can see that the IC is going to be much stiffer than the PCB substrate.
The thickness of 0.15 mm seems very thin for a board that has a span of 45 mm. Is it correct?
In the Static Structural model, do Fixed Supports like you did in the Modal, instead of the Displacment and Fixed Rotation you had. Then add an Acceleration load in the Z direction of 200 m/s/s. With Large Deflection turned On, you will get this plot of Deformation
In the Modal analysis, you set the stiffness behavior of the IC to rigid, but there is no need because it is already much stiffer than the PCB, and the Modal solution won't solve with a Rigid body. Set it back to Flexible. You can use a finer mesh in Modal.
After you solve the Modal, you can drag and drop a Transient Structural onto the solution cell of the Modal. Then you can apply an acceleration load to the Transient Structural to do the sine sweep for a Linear Modal Superposition Solution. No Large Deformation!
Paste the data from the attached text file, which is a 5g acceleration sweep from 20 Hz to 200 Hz sampled at 2000 Hz.
Analysis Settings, set the Time step to 5e-4 and Solve to get the Linear solution.
Duplicate the Transient Structural system and add the Fixed Supports, then you can turn on Large Deflection and perform the Full Transient solution.
You may as well add a Harmonic Analysis off the Modal to see what the frequency response is from the linear system.
Here is the Linear solution of the Transient Structural.
You will have to assume some value of damping. Since you are clamped so tightly to the PCB using a steel fixture and clamping bars, it is probably lightly damped. Try 5% damping. That means typing 0.05 in the Direct Input. There are experimental methods to measure the actual damping, like a pluck test.
1) In a Transient Structural, you are free to choose to apply a Force, Acceleration, Velocity or Displacement to the fixture. It is entirely up to you. These boundary conditions can be applied to the fixture that is bolted to the armature of the shaker, but if you use Force, then the mass of the fixture determines what the resulting acceleration is going to be. You can put the entire mass of the armature that drives the shaker table if you wish.
2) You can do a waterfall FFT and take blocks of data over the 10 second simulation and show how the frequency content shifts versus time.
You can output the displacement data of any point on the PCB or chip or fixture that you want. In a 3D model, where a chip stands above the PCB and there are lead lines coming out the side of the package and are bent down to be soldered into via in the PCB, then you can have motion of the chip separate from the motion of the PCB under the chip, but in your 2D model, that is simplified away into a single point.
3) Yes, you can have a Tabular input to the Displacement boundary condition that specifies the x, y, z coordinates of an edge or face vs. time.
4) In Transient Structural, you can run for a few seconds at a particular frequency, let a displacement amplitude develop, then change the frequency for the next few seconds. That is what we are doing in the Sine Sweep. Gradually changing the frequency from 20 to 200 Hz over 10 seconds.
When you say that displacement is "my real BC", that is only from the frame-of-reference of an observer standing on the ground next to the shaker. The fixture appears to move up and down, carrying the PCB with it.
Change your frame-of-reference and put yourself on the fixture. From that point of view, the fixture doesn't move at all, but you feel the acceleration go positive and negative, causing the PCB to flex up and down. This is just as real as the frame-of-reference of the observer standing on the ground.
I opened your archive and I looked at the system C, that has the displacements. It is showing +/- 15 mm of displacement. That is way too much. Where did you get 15 mm from? Have you computed the acceleration from that data?
I can tell that you have a sine sweep from 80 Hz to 200 Hz in the displacement data.
Because the displacement magnitude is constant over the frequency range, the acceleration must increase to meet the displacement requirement. The plot below shows the acceleration in G required to meet this 15 mm displacement.
I'm sure you don't want your PCB subjected to nearly 3000 G of acceleration.
Why don't you define the sine sweep requirements in terms of G force and let the displacement be calculated?
Sine Sweep on Shaker Table: Is it constant amplitude or constant acceleration?
If the constant displacement is 1.4 mm, then the acceleration is 36 G at 80 Hz, while it is 225 G at 200 Hz . That is a lot more reasonable than 3000 G.
If the constant acceleration is 36 G acceleration, then the displacement amplitude is 1.4 mm at 80 Hz and reduces to 0.2 mm at 200 Hz.
Find out what the shaker table settings were for the experiment. I think you will find is it a constant G force input with the start and end frequency. What three values were input into the shaker controller?
If the shaker input was a constant G force input, then use an acceleration input with fixed supports in the model.
If you find the shaker input was a constant displacement of 1.4 mm, then use a displacement input with fixed rotation in the model.
2. The exceedingly high G acceleration caused the solver to fail to converge, which may be because of the plasticity in the model. The high acceleration causes a high stress that stretched an element so far out of shape that it could no longer compute stress and strain. If you delete the Multilinear plasticity and rerun the solver, you might find it gets further in time than it did before, but as I said, the final value of 3000 G is ridiculous and the solver may not converge later in time even with a linear material.
The solver doesn't stop when the nonlinear material Total Strain exceeds the material property of Elongation at Break. It just keeps stretching the material. You have to plot the Total Strain and see if the maximum value has exceeded Elongation in order to predict failure. This is just like a linear elastic material, the solver will continue to run to values of stress far exceeding the Ultimate Strength. It is up to you to plot the von Mises equivalent stress and compare it with the Ultimate Strength to see if the part is predicted to fail.
3. I don't know what you saw in the video that was 15 mm. If the shaker was set to 1.4 mm, that is what is important.
1. When the Transient Structural model finished, the folder had 38 GB of data.
2. The solver was limited to the maximum time step and did not use the minimum time step, so the change I made was not needed and made no difference. The warning about the slow script has to do with processing 20,000 data points of output. It is a very heavy load to manipulate.
3. Do you mean clicking No at the slow script dialog?
You are doing a sine sweep from 20 to 200 Hz in 10 seconds or 18 Hz/second. Looking at the Modal results, you know the first natural frequency is at 92 Hz. Rather than spend 14 hours computing 10 seconds or 20000 points of data, why don't you instead spend 2.8 hours computing 2 seconds worth of data from 74 to 110 Hz. Then you can see the change in response as the frequency passes through the first natural frequency of 92 Hz. You will also only end up with only 4000 points of data instead of 20000 points and that will not slow the script to the point where you get warnings.
4. Looking at the attached Harmonic Response file and your comment 4 above, you do not understand what the Harmonic Response analysis is or how to use it. I Deleted the Tabular data in system D and replaced it with a 98 m/s^2 (10 G) harmonic acceleration load.
Going with the suggestion above to look around the frequency of Mode 1, I changed the analysis settings to plot 50 points between 75 and 125 Hz.
I requested the Frequency Response of the Z axis Directional Deformation of a vertex on the corner of the IC.
The solve takes 22 seconds, but it is a linear solution.
What this says is that the corner of the IC will vibrate with an amplitude of 4.6 mm when a 10 G periodic acceleration is applied at 94 Hz.
But because it is a linear model, we know that the nonlinear solution for z-displacement is much less due to stress stiffening.
I only picked 10 G, but your displacement amplitude of 1.4 mm has an acceleration of 50 G at 94 Hz. With a 50 G input, the linear frequency response says the deformation amplitude would be 23 mm, but that is an absurd value. The nonlinear effects are going to keep it from getting that large.
I suppose that is why Dr. Perkins want a nonlinear Transient Dynamics solution that can have Large Deflection turned on.
ANSYS 18.2 archive attached.
In this Transient Structural, I changed the Analysis settings to have 1 step with a 2 second end time.
I wonder is some of the slow down was because you specified 20000 steps?
I created a 1.4 mm displacement that sweeps from 74 to 110 Hz in 2 seconds, but I used 2000 samples/ second.
I'm going to run that now.
ANSYS 18.2 archive attached.
I am convinced that the very slow response of Mechanical was not due to the number of data points, but due to the number of Steps. When I ran the model with 2 seconds on a sweep from 74 to 110 Hz in 1 step, the solution only took 43 minutes. You can get 20,000 data points in 1 step by having a 10 second end time and a Maximum Time Step of 5e-4 seconds. When you do this, I don't think you will get the slow script warning.
2. I don't understand why you don't know what the input to the shaker is. It's an input. That means you set it! How do you not know what the input is???
What do you mean that 1.4 mm is the amplitude of the output? Where exactly is the output? Are you calling the motion of the fixture an output? I'm confused. Can you please clearly define what the input is and what the output is.
Yes, as I said above, a linear solution of 23 mm for a 50 G acceleration input is ridiculous. You can run the nonlinear Transient Structural with a 1.4 mm 94 Hz displacement input and see what the response of the IC will be. The problem with a displacement input of 1.4 mm is that that value is included in the displacement of the IC, so you have to subtract 1.4 mm off the maximum displacement of the IC to get the displacement of the IC relative to the fixture.
For example, say you put in a 1 Hz frequency of 1.4 mm on the fixture. The IC is going to have a 1.4 mm displacement also, but the relative displacement is zero.
I agree there is another resonance for Mode 2 at 190 Hz. That is fine, just do a sweep from 170 Hz to 210 Hz in a second analysis to complement the first mode of 93 Hz with a sweep from 74 to 110 Hz.
The rule of thumb is that a minimum of 20 samples per cycle are required to reconstruct a time history plot. So for a 100 Hz frequency, the minimum number of samples is 2000. I doubled that to get 4000 samples.
I created a 1 second input sample of 1.4 mm displacement amplitude at 94 Hz to run in the nonlinear transient model. I took the time history of one corner of the IC as the output. In the first few hundred milliseconds, higher modes are excited by the start of the vibration, but by 0.5 seconds, the transients have died down. Below is a spectrogram of the frequency content.
If I want to see what the nonlinear response is at 94 Hz, then I should throw away the first 0.5 seconds of data. This calls into question the sine sweep rate of 18 Hz/sec. The military test specs I looked at took minutes to sweep from 50 to 500 Hz.
Here is the first 100 ms of the output.
Here is the last 100 ms of the output for the 1 second simulation.
It looks like the amplitude of the IC is 2 mm, while the amplitude of the fixture is 1.4 mm so the Relative Displacement amplitude of the IC is 0.6 mm. This is the nonlinear result that matches the 23 mm from the linear harmonic analysis.
Hope this helps.
If I turn off the Large Deflection switch and run the Transient Analysis as a linear solution, the first 0.5 seconds of that 94 Hz 1.4 mm amplitude input is 64 mm!
In the long term, after the transients die out in several seconds, that would become a 23 mm amplitude.
Your sketch shows tracking of the IC displacement as an "input", but that is an "output" or Result of the Transient simulation. The input to the Transient simulation is a displacement of the edges of the PCB, that is set to 1.4 mm of amplitude at a 94 Hz frequency. Similarly, the input to the Shaker controller is either a displacement of X mm and a frequency, or it could be an acceleration input of some number of G's. That is what I want to know. What is the setting on the controller for the shaker table that creates the motion of the shaker that the fixture is attached to.
1. What is the "it" that might be helpful? While you are there, ask him what the inputs are to the shaker.
2. If you link the Modal analysis Solution to the Transient Structural, then you inherit the supports that are in the Modal, which are Fixed Supports. The only load allowed then is Acceleration on the masses.
3. ANSYS 18.1 attached.
4. You can put any file in a zip file and it is allowed to be attached if it is < 120 MB.
If you have another question, please start a New Discussion, as this topic was marked as "Is Solved" long ago. When a discussion is very long and marked as Solved, fewer people are going to look at it. There are members here beside me who have deep experience in Dynamics and it would be good to have their comments as well.
Please reply with a sketch of the part, the supports for the part and the transient load on the part.
Please describe what in this model makes it nonlinear.
It's a good idea to do a Harmonic Response analysis before you use Transient Structural. Have you done that?
If you can share the model, attach a Workbench Project Archive after you post your reply, and say what version of ANSYS you are using.
The nonlinearity of the flexible PCB is large deformation(geometrically) and material nonlinearity.
The external load function is:
sigSweep = .5*cos((startFreq*sweepTime+((stopFreq-startFreq)/stopTime/2)*sweepTime.^2));
The two rectangular beams on the sides are the fixed support, and I would like to give it a base excitation on the two beams on the sides, but I am not sure how to do it correctly. so I change the BCs into the two beams on the side fixed rotation and the displacement with only Z is non-zero. the external excitation will also be applied at the two beams and it is sine sweeping function.
I do did the harmonic response, which give me some nonlinear effects on some special situation if I give different damping and number of steps. I have no idea why it will have nonlinear effect?
Thanks for your helpful and patient reply.
Since I am also considering not including the nonlinear materials. Because only the geometric nonlinearity will also cause the system nonlinear. besides, you said that I need to use the sine function instead of the cosine function which will avoid the high-frequency noise that cause the data I do not want?
As for the boundary conditions, does it means that only the displacement is enough?
by the way, I turn on the large deflection and the nonlinear effects within the workbench, does it means that I make the model geometrically nonlinear?
That will be very great if you could provide me with the acceleration or displacement file with different settings.
As for a question concerning the damping, if I do not know the damping of the flexible PCB with the IC chips mounted on it, How could I deal with the damping? any suggestion?
one more question is that I also try with the 2D model with the thickness assigned for both the PC board and the IC chip(But I could not give two different surfaces on the 2D model, which means that I will miss one IC chip if I use the 2D model, How could I add another IC chip?), will it make the solving process faster, if it is, will the solution become less accurate?
sorry about that I have so many questions to ask, if 500 data points is inadequate, instead, I need to apply entirely 40000 data points, I do not think that my laptop could handle that large memory-required solution, could I try it with 10000 data points? will it cause a lot of errors?
Thanks very much for your help
Some other questions:
1. I have done the 2D model of the PCB with only one but not 2 IC chips mounted on it. I have no idea about how could you slice them in DesignModeler? could you please give me some help or suggestion? I will also attach the model that I have done with the SpaceClaim, After you take a look at it, you will know where my question is.
2. Like you stated, if the condition is fixed edges and the acceleration load, then you will need the sine function since at the time zero the acceleration is zero as well. while as for the condition with the fixed edges and the displacement, you would like to use the cosine function, but consin0=1, how could the input displacement be zero at time zero? did I misunderstand your points?
3. I also asked one of the professors working with vibration, he told me that the nonlinear geometry is vert important for my simulation, even I do not give any nonlinear materials, the nonlinear vibration effect will also occur. besides I have also read some papers which said that if the external load is large enough(large amplitude) then the nonlinear vibration effect will happen.while my research is only focused on the nonlinear vibratory effect(just the demonstration of the nonlinear vibration effect) still no any relation to the failure or fatigue.
4. The 3D model that simulated in the harmonic response is the real model that I would like to use, the reason why I use only the PC board is because I would like to make the problem simple and take less time to solve, then I will use both the PC board and IC chips to do the next simulation. but is it possible that I could get the nonlinear vibration effect with only the PC board?
5. Since from the modal analysis, the first mode of the PCB with the IC chips is bending, as for the meshing, I applied the nonlinear mechanical for physics preference, quad elements, curvature for sizing function, quadratic for element order and the quality-error limits-aggressive mechanical. is it good enough for the nonlinear analysis of the PCB with the IC chips?
6. The IC chips will be simplified as the rigidly connected with the PC board, there will be no any contact nonlinearity within my simulation.
Here comes some other questions
1. sorry that I did not use the DesignModeler, since I am doing it for most of the time in SpaceClaim, It seems that I do no have the option share within the share topology, besides is it the reason the at I have the ANSYS version of 18.1 but you have the higher version of 19.1?
2. if you use the A*cos(w*t)-A, the input will not change the direction from -Z to Z, which means it will only have the negative direction all the time and the magnitude of the input will also be doubled, why do not we use the sine function for the displacement input?
3. I am trying to do the static structural, as what stated before, there will be 40000 data points in total that I could cover the high frequency effect,especially the 200HZ, on the nonlinear vibration. but given that it will be taxing for my laptop, could I use only 2000 data points? but if I do it like this way, will my result get totally distorted? do you have some suggestion?
4. like what you have mentioned before: "If you have no nonlinear materials, then you can put a Modal analysis first and feed that solution into the setup cell on the Transient Structural, then run the linear MSUP transient solution, which may run a bit faster. The Transient Structural will take an Acceleration load, but not a non-zero Displacement if it is using the MSUP solution." as far as I know, you could link the engineering data, geometry, model and solution but not the setup cell, could you please show me how could I feed the solution from the modal analysis into the setup cell on the Transient Structural? After that, will the ANSYS automatically run the MSUP transient solution or maybe I have to change some settings?
5. Every time, when I use the function setting for one of the components for the displacement, the other two will be automatically locked as free, do you know why will I have such a problem?
1. In the image, do you have two bodies? If you have one body with two faces, then you don't need to Share Topology.
2. The equation I showed has an amplitude of A and a peak-to-peak range of 2A. That is the same when you have A*sin(t). If this is a displacement input to a shaker table, what do you care if it goes down to -2A and back up to zero, or if it goes up to A and down to -A. It's the same range and the velocity is both going up and down. I don't think the PCB cares what height it is at.
3. If you do a Static Structural, you don't use 40000 data points. You apply a constant acceleration of say 100 G in the Z direction. In the Analysis Settings, Auto Time Stepping is turned On. You set the Initial, Minimum and Maximum Substeps to 100 and Solve. Request the Deformation. You can now see with 100 points on the plot. Solve it with Large Deflection On and Off and see how the shape of the plot changes. That is the nonlinear geometric effect you are looking for.
Forget about the 40000 data points. They will not tax your laptop. You could cut it to 20000 if you really want do make some change, but it will not matter either way.
4. Drag out a Modal analysis and drop it on the Project page, then drag out a Transient Structural and drop it on the Solution cell of the Modal analysis. That will create links which will define this Transient Structural as a MSUP solution and will not allow large Deflection to be used as it will be a linear analysis. Note that the Fixed Support is put into Modal and cannot be added under the Transient Structural branch.
5. When you use a function setting in a BC, then the other components are free. That is normal. You can use another BC to set the free components to be zero.
Thanks for your fast and helpful reply.
1. I do have more than 1 body, in fact I will have 3 bodies in total, one is the PC board, another two will be the IC chips that are mounted on the PC board, that is why I am asking that if I give the 2 surfaces with assigned thickness, when I try to give the material properties, I could assign it to the PC board and only one IC chip not the both, that is the problem that I could not solve, But considering that the two IC chips have almost the same material properties, I think it would not influence that much.
2. I am currently meet some problems on convergence issue, when I was doing the transient structural with my flexible PCB, if I turn on the large deflection, it will have some errors, I do use small time steps, but still have no idea why it will happen. while if I turn the large deflection off, there will be no errors and I am good to get the result, do you have and suggestion? I also attached the solver output file and the workbench file.
3. Sorry about my question about using sine or cosine function, hope it does not bother you. but very grateful for your amazing reply.
4. I have also done some research on nonlinear materials for the PCB, but I feel confused which nonlinear materials should I use in ANSYS, should I use the plasticity-multilinear isotropic Hardening? I think that will be the one that match the best with the model. besides it is not that easy to get some nonlinear materials for the PC board online, is it possible you could give me some help on it?
Thanks for your helpful and patient reply
some other question still need your advice,
1. if I turn on the large deflection there will have nonlinear solution, if I turn it off, does it means that it is linear case?
besides, what is the meaning of turning on the nonlinear effect and thermal strain effect?
2. as you mentioned that even though I do not apply the nonlinear materials but with only linear isotropic material properties, I could still get the nonlinear vibration effect with only geometrical nonlinearity. is the reason that the geometrical had already included the nonlinear stress-strain relationship like the COMSOL example you sent it to me a few days ago which told me that the geometrical nonlinearity will also cause the stress-stiffening?
3. you are right, the IC chips are mounted on the opposite side of the PC board, therefore, my 2D model with assigned thickness could handle PC board with only one chip not both, that is why I could not make it perfect. besides when I was doing the mesh within the ANSYS, it shows me two IC chips, does it means that I will have 2 IC chips with the same material properties?
As I marked in the green color, There are only two surfaces that could be given the thickness, therefore it should have the PC board and only one chip, but from the view of mesh, it is 3 bodies(PC board and 2 IC chips). Do you know why?
Sorry that I have so many questions to ask
1. every time when I turn on the large deflection, there will come the warning as I posted following, will it have a big influence on my final results?
2. Thanks for telling me that I could also change the default iteration from 26 to 60. but why I did not find out that It is the issue of inadequate iterations from the solver.output file? but if I decrease the minimum time step, I find it out that there will be no convergence issue, does them means the same thing?
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback
This Weeks High Earners
- 1 Hi, I have a problem to install the license and see my problem, I am sure you can help me. Thanks
- 2 Could not connect to license server: 54529@localhost The handle is invalid. .
- 3 Problem with the Student Version
- 4 Convergence of adaptive mesh refinement tool
- 5 Structural-Thermal analysis error : element type