How to perform two step dynamic analysis in Ansys Mechanical
-
-
Also I want the disp vs time graph of the response, that is of the isolated object for different frequency ratio and damping ratio. So how do I input those values for it?
Here are their results:
Top means a surface on the isolated object and bottom is where the input of Z sine wave is given.
Alright I will check it out, but as for this problem with hyperelastic material, what should I do to simulate this type of analysis.
I tried Modal+transient and did not get the correct results.
Here my step 2 was given base excitation of 5mm amplitude and the output is pretty much having the same amplitude, but in reality, it should dampen out those vibrations and have a small amplitude as the other graph shown previously of disp vs time.
So what should I be doing for it? I will check out the harmonic response tutorials and the course from here as of today and try to understand it.
I have started to look at your 2D model. First observation: you must have at least 2 quadratic or 4 linear elements across the width of any member that will see bending deformation. This mesh has only 1 element, which is insufficient. I will continue to investigate over the next 3 days and post new information as I find it.
Is this fine? Used quadratic this time
I have other related doubts with static analysis too which I will ask later. Basically I tried static analysis to get F vs D graph while base is fixed and the top surface is displaced in steps.
I tried it for both the whole metastructure as well as unit cell, I should get a non linear curve with a little flat region in the middle, which I got correctly for the metastructure but not for the unit cell.
This was my graph for the metastructure
And this is for unit cell, which is wrong. I used the same procedure for both during the analysis.
The two graphs in your last post are not plotted on the same axes, one is F vs D, the other is U2 vs what? Please label axes and include units. Also, the metastructure has 3 layers of unit cells so if you displace that 30 mm, you should compare that with a unit cell displaced 10 mm.
I have a post that lists recommendations for models that use hyperelastic materials. You need to follow that advice if you continue to use 2D Plate elements. This is not necessary if you use 3D Shell elements.
I tried 2 quadratic elements through the thickness and it did not perform well. I had to do some slicing of the domain in order to get pieces what would be easily meshed. The image below has 6 linear elements through the thickness.
Another approach to this model is to abandon the 2D meshing of a surface and replace the entire model with beam elements on line bodies. That would eliminate any concern about how many elements are through the thickness and it would reduce the node count to a very low number which would make the transient solution compute much more quickly. I built the mesh shown below, then learned that Beam188 elements do not support hyperelastic material models. So if you can use linear elastic materials, you could use this approach.
Next I extruded the line bodies into sheet bodies 10 mm wide. Shell elements increase the node count by 4 times over the line bodies above, but is still a lot fewer nodes than the 2D Plate elements.
I ran the top surface down using a Displacement BC, without gravity, in order to plot the force-displacement graph.
It looks like you adjusted the mass of the supported object and the frame itself in order to put this mass on the flat portion of the force-displacement graph.
The deflection due to gravity is working as it should.
Here is the input to the Transient Dynamics model. I stopped the solution at 2.4 seconds to check the progress.
Here is the output at the top mass:
What we see here is a mistake in the model. I forgot to turn off Time Integration in Step 1 so we see the bouncing up and down for 2 seconds. It looks like the natural frequency is about 2 Hz. So at t=3 when the shaking starts, the mass is not at rest. I will rerun that with the proper setting for Step 1. I also forgot to enter some damping. In the attached model, I have entered 0.05 damping ratio at 2 Hz and turned off Time Integration in Step 1.
ANSYS 2021 R1 Archive.
The above archive didn't converge. I made two changes to allow the spring to settle in the deformed state at the end of step 1. I changed from Standard Earth Gravity to an Acceleration load that I could ramp on from 0 to 9.8 m/s^2. Here is the motion of the top mass:
The second archive failed to converge during the transient step 3.
The corrective action is to put 6 linear elements across the thin beam in the 2D Plane Stress model OR switch from 2D Plane Stress to a 3D shell model.
I managed to get 6 linear elements across the 2D beam just using the Proximity Mesh control.
That model is running now.
I showed you how to make a 3D shell. That may have less convergence problems, but it will surely solve faster.
Even with such fine mesh for the 2D analysis and then having at least a 100 substeps in the analysis settings, why do I still not get the right results for F vs D? Also it gave no errors for convergence.
The link above is to the 2D structural analysis I tried. Please let me know as to why this type of model will not give the desired output. Is it because of the meshing?
The last model I attached, Transient 2Hz made it 83% of the way to the end of the simulation before an element started turning inside-out. One advantage of the 3D Shell model is elements won't start turning inside-out.
Here is the input base motion:
Here is the output motion of the top mass:
Plotting these on the same chart looks like this:
It doesn't look like the top mass is being isolated.
Would the model look something like this?
Something like this:
I used a Beam element to go between the layers. It may be possible to change the cross-section from rectangular to a tapered beam. Not sure about that. It could have been a sheet, but then the thickness would be constant, but it is a little easier to do if you haven't created beams before.
Fixed Joints (Behavior = Rigid) is used to tie together the pieces at each intersection and jump the gaps.
I was able to connect the single column and add enough extra constraints, such as Fixed Rotation, and Displacement of X and Z = 0 on a few nodes to limit the spring to motion along the Y axis without having to make more columns. To simplify as much as possible, I used a linear material, Stainless Steel, which is a lot stiffer than the TPU, but I put a lot more mass on the top to get the deformation to the flat part of the Force Deflection curve. It is not quite flat because there is a mistake I found later that I haven't fixed yet.
The good news is that when I turned on Gravity, the solver pulled the top down to the same deflection. I ran a Modal analysis, and found the first mode was at 12 Hz. I made a three step transient, step 1 gravity in 0.1 s, step 2, no change till 0.2 s, step 3 a 12 Hz 4 mm sinusoidal base motion will 1.2 s. I got a result similar to what the paper shows, excellent isolation. Because there were so few nodes, the Transient solution finished in 9 minutes! Before I was waiting hours.
I checked the Connection Elements created by the fixed joints and see I made one mistake and have one extra edge that I will remove and rerun the analysis to get final results.
I think you can get to this point (without the mistake) by Monday.
With the mistake fixed, the F vs D curve flattened out.
The response also looks cleaner and I forgot to include any damping in the model, so the result is impressive.
To be effective in your internship, you need to develop geometry creation and editing skills, model building skills, and simulation debugging skills. I gave you the 3D surface model of the two springs of a half cell in the attachment (Geometry Options for Spring) in my August 7 reply on P2 of this discussion. I have attached just the geometry here for you in a 7z file below.
Use the Mirror button to reflect surfaces about the center of the unit cell then use the Move tool, holding the Ctrl key to make a copy to stack up 3 layers. Instead of the Move tool you can also use the Linear Pattern tool to copy them down. You will have to sketch out some lines for the Frame and extrude those out into surfaces. I'll check in later to see how it's going.
Is this alright for the 3 row model?
Is this alright?
Is this correct for the 3x4 arrangement?
Okay, I tried doing it a little differently, so that giving fixed joints would be easier.
Can that red marking be ignored? I selected multiple edges for it and joined it to another single edge
My Meshed model
How do I restrain its motion in y and x axis, even the rotations?
Since it is a shell elements, I am not able to select the front and back faces in frictionless support as they are seen as lines and not surface
This time I tried making it look exactly like the one from the research paper
But it did not work and the F vs D graph is bad
I will try meshing it finer and see if that changes anything
Wow, a lot of progress!
Below is the split in the face that is needed to make the Fixed Joint. Go to SpaceClaim. Use the Split button and Ctrl-click all the horizontal faces in one column then click the Cut button and select of of the vertical faces at the center to split the faces. Repeat for the other 3 columns. Then go and repair each fixed joint and change it from using a face to using only edges. The reason for this edit is that the Fixed Joint with behavior Rigid makes the whole horizontal frame rigid instead of flexible.
Below is the Rigid Elements that cover your structure, you can see it covers way too much compared with the example I provided in one of my previous comments. This is why your F vs D is not correct. Look carefully at which edges are included in each joint. This plot can only be seen after the solver has run on the model. Click on the Solution Information folder where you see the Force Convergence Plot, except the main graphics window automatically switches to Worksheet. Click the Geometry tab at the bottom left of the main window to see this plot.
I will send this now and keep looking at the rest of the model. What time zone are you in? I am in the Eastern US Time Zone. I posted this at 7:08 AM. What time does it show for you?
Okay, you are 9 hours ahead, so we have a few hours before it gets late for you today.
Here is what the Rigid Connection Elements look like after splitting the faces and repairing the Fixed Joints.
Below is the F vs D graph for TPU without Earth Gravity, there is a glitch at 0.5 seconds.
Below is the F vs D graph for TPU with Earth Gravity, which seems to smooth out the glitch.
Below is the F vs D graph for Stainless Steel, a linear material, without Earth gravity. The linear material is more stable over the flat part of the curve.
The nonlinear properties and the low stiffness contribute to the lack of flatness.
Below is a Transient Structural run with a 0.126 kg point mass added based on the 1.24 N force at the top of one of those smooth waves of TPU with gravity as the only input. Z = Free at the top.
If you perform an FFT on the data from 1 to 2 seconds, the frequency is 4.688 Hz. That is the natural frequency of this system.
How do I join this part? It is separate, the horizontal base on the right and the left.
Its split this way, the blue lines are a single unit and the yellow marked is seperate
How do I fix this? That part isn't acting as a fixed joint, though I have combined the bodies in spaceclaim
Got it finallyyyyyyy
This is my model. I found a mistake in the Connection Elements in one of the Fixed Joints. This kind of mistake can hurt the convergence.
This is caused by having the Fixed Joint Coordinate system out in space. Not sure how that happened, but glad I checked it. Make sure you have checked this plot of the Connection Elements.
Here is a completed transient with TPU and a 5 mm amplitude input motion. It would be interesting to simulate another few seconds. This took 53 minutes to simulate.
I fit a straight line to the Uniaxial TPU data and came up with a modulus of 41.4 MPa. I'm going to convert this model to a Linear Material and see what it looks like.
I am looking at your model now. I see the version of ANSYS you used in the last iteration was 2020 R2, but I understand you have access to both versions, since I have been working in 2021 R1.
It may turn out to have a smoother motion if Earth Gravity was on in Step 1 then the motion began in Step 2.
Looking through the Solution Output, these warnings were issued:
*WARNING*: 24 MPC equations were released for the rigid constraint surface identified by real constant set 249 due to overconstraint detection logic.
*WARNING*: 24 MPC equations were released for the rigid constraintsurface identified by real constant set 265 due to overconstraintdetection logic.
*WARNING*: 6 MPC equations were released for the rigid constraintsurface identified by real constant set 269 due to overconstraintdetection logic.
I got those warnings too, and they mean that the solver has to ignore some of the things you asked it to do because it can't do two things at once: (1) Use a node in a joint and (2) use a node in a boundary condition. I eliminated those warnings by creating boundary conditions using nodes near the point when the joint was, while not using any nodes that were in the joint (on the edges). Not sure if it will make a difference in the output though.
For example, since there is an edge in the center that is part of a Fixed Joint, I picked 8 nodes on the base to use in the Displacement 3.
In order to apply an X = 0 constraint to the vertical sides of the frame (frictionless support) without touching the nodes along the top edge that were involved in a Fixed Joint to the spring, I picked a row of nodes just below that and also a row along the bottom corner. I held both X and Y = 0 to keep the cells in the XZ plane.
The TPU output had 5% damping at 5 Hz
Here is the same model, but with a Linear Material E = 41 MPa instead of a Hyperelastic Material.
Increased E to 90 MPa and now the flat part of the curve is about 1.22 N which is where the TPU was.
This requires about the same 0.125 kg mass, but when the Modal solution is run, the natural frequency is 11.6 Hz.
Here is the linear material, which has an 11.6 Hz natural frequency, delivering the expected isolation:
Looking at the plot in the paper shown below, I don't think the authors in that paper are starting the base excitation after gravity has dropped down the mass. I think the mass is falling to the equilibrium height at the same time that the base is vibrating. This makes the simulation easier, since I had to create a 3 step simulation to first let the mass settle to the equilibrium height, then start the base motion. But experimentally, that is an odd setup. It means the mass must be supported so that the springs are not compressed and the mass is released at the same time that the base motion begins. Don't you think that is an odd way to run an experiment?
Also, how do i check these connections? I am not able to find the option or tool to do so.
Okay, so I was trying to do this static analysis with having point mass over each column and then turning on gravity.
But it turned out to be this way. How do I make it translate only in Z?
I tried your method to restrict the nodes from displacing in X and Y but I cannot apply that boundary condition. If I select the node and press apply in the geometry, it doesn't work.
Like I am selecting the nodes this way and then press apply, but nothing happens. What am I doing wrong?
This plot can only be seen after the solver has run on the model. Click on the Solution Information folder where you see the Force Convergence Plot, except the main graphics window automatically switches to Worksheet. Click the Geometry tab at the bottom left of the main window to see this plot.
Returning to the question of starting the simulation with the spring uncompressed and the mass out of equilibrium with gravity as implied by this graph.
In the current simulation, I changed the sign of the motion to agree with the sign convention above. As you can see below, the mass starts falling, but the spring seems much too weak and the mass falls a large distance. Perhaps instead of a stronger spring, a larger base motion would help?
Here are the analysis settings for Transient Structural.
This looks pretty neat
Now I will start off with the transient analysis
In the plot shown in the paper, I feel like they have done what you had done first, that is compressed and give base excitation. The output of it then is adjusted to make it look like it started off from 0 displacement. So I feel like that shouldn't really matter as long as we can get the same kinda damping effect in our simulation.
This graph looks pretty good
But what is the reason for us getting a pattern in the output and them getting a regular sine wave instead?
Am i doing something wrong here? I am not getting those named selections in the option though they are created
When you click in the pull down, there are no named selections?
The wiggles in the model are a combination of a low frequency oscillation overlaid with the driving frequency of the base. I'm not sure why we don't get the same wiggles as in the paper. I did a few one-step simulations but the top mass had much larger amplitudes than the base.
Anything else Ive to add to the boundary conditions?
I will run this and see, same conditions as in the link I had sent last.
Don't forget to add the 5% damping.
You have two joints holding onto the same blue edge on the frame. Use a single joint to hold all 4 edges. Delete all duplicates and repair remaining joints to eliminate this condition.
Below is the repaired joint with the duplicate suppressed.
Yes, you can use an online tool to generate a sine wave tabular data. Just make sure you get 500 points per second.
You have matlab, so you should download the free Vibrationdata Signal Analysis Package from Wordpress from the link below.
It is a zip file. Unzip to a folder. In matlab, add that folder to your Path. Type vibrationdata at the command line.
Click Begin Analysis. Fill out the entries, then click Calculate. Then type in a file name and click Save.
That variable sine116 is now in the matlab environment. It has Time and Displacement columns. Highlight the rows and copy, the paste into Excel for adding 0.2 to the Time column, then add a row for time = 0, 0.1 and 0.2 with Displacement = 0.
After you make a new time column, copy those 2 columns and 503 rows so you can paste them into Mechanical.
Step 1 converges easily.
You can try to reduce the Minimum Substeps to 10 instead of 100, but leave the Initial Substeps at 100 since it needed that to get started.
Step 2 converges easily.
You can try to reduce the Minimum Substeps to 3 instead of 10, and set the Initial Substeps at 3 also.
I did it directly in excel using the formula
I am getting an error
Add a Modal analysis.
Drag and Drop the Fixed Support, the side displacements.
Make a Nodal selection called Top. Use that in a Displacement that prevents motion in X and Y.
Mode 2 is at 12 Hz and is the vertical motion.
Unfortunately, Mode 1 is at 9.9 Hz and is the top beam pitching.
How to fix the error.
Suppress both Frictionless Supports, You have Nodal Displacements to replace them.
The Displacement 3 on the bottom faces includes nodes used in the Fixed Joint to the bottom rail.
Create a Nodal Selection of nodes on the bottom rail that avoids the nodes used in the Fixed Joint.
These are the frequency values that I got
First mode shape looking like this
Some of the nodes on the face are used in the Fixed Joint, so you can't use them in a Boundary Condition as well.
I solved the transient analysis, but my response isn't dampened. What could be the reason?
I tried the static analysis, It shows a correct reaction force
But the deformation should be 14mm instead it only shows 1.58mm
What is the exact meaning of this frequency in the damping control?
Hi, I really tried different things with the transient analysis but couldn't get the correct output for disp vs time.
Please check this file
It is the last two systems in which I have tried the latest analysis.
Here are a few frames showing Step 2, the transient portion where there are no changes in the Boundary Conditions.
At the end of Step 1, the structure is compressed. The contour is the X displacement.
As I said before, if you extrude a deeper structure, 10 or 15 mm instead of only 5 mm deep, that may help to stabilize the structure. You could also increase the thickness of the horizontal springs to reduce the chance of buckling. This is an actual physics result, not an artifact of the simulation.
I increased the horizontal spring by 5% to 0.84 mm and that seems to have fixed the problem. I could get through step 2 with only 100 initial substeps.
Probably would have been a better idea to do the F vs D graph after changing the stiffness of the horizontal spring before spending nearly 5 hours computing the transient.
Here is the F vs D plot where step 1 up to 0.1 s is gravity ramping up while the top rail is held fixed, then step 2 is the bottom rail moving up 30 mm. You can see that about 3 N is perfect force to be in the middle of the flat region.
Checking the mass, it is at the sweet spot of 0.30 kg.
Adjusting the mass up just slightly causes a gravity powered Static Structural solution to shoot well past the middle and end up on the far end of the flat. It is very difficult to adjust the mass to put it on the flat, especially with the wavyness.
To answer your question on Damping, you should watch the videos in this course: /courses/index.php/courses/damping-effects/
Viewing 176 reply threads- The topic ‘How to perform two step dynamic analysis in Ansys Mechanical’ is closed to new replies.
-
You are navigating away from the AIS Discovery experience