December 27, 2018 at 4:57 amRavikishanSubscriber
December 27, 2018 at 5:50 ampeteroznewmanSubscriber
Please reply with an image of the mesh, especially zoom in on a thin section and show how many elements are across the thickness. You should have at least two elements across the thickness.
Is the mesh setting to Keep or Drop Midside Nodes? It is better to Keep Midside nodes.
December 28, 2018 at 6:19 am
December 28, 2018 at 7:02 amRavikishanSubscriber
please check the attached archive file.
December 28, 2018 at 9:27 pmpeteroznewmanSubscriber
I'm looking at your model now and had a few questions and comments.
I don't know why you get an "Invalid Geometry" message. There is no error shown in Solve.out, but the simulation runs.
Do you know about Modal Superposition (MSUP) solution method for linear analysis?
That is shown below.
I assume that you don't want MSUP because you want a full nonlinear solution.
Why are some of the parts meshed with linear elements (midside nodes dropped)?
Better results are usually obtained from quadratic elements (midside nodes kept).
Some of your parts seem to have only one element through the thickness, which can be a problem.
In the Transient Structural, the End Time for analysis is the same as the end of the ramp on the acceleration. I would have expected that the sawtooth would have occurred and then there would be a much longer simulation time to observe the response in the system to that "shock", like 100 ms.
Where did the 20,000 G level at 11 ms come from? That sounds way too high. This webpage talks about a 20 G shock level at 11 ms. If you convert 20 G to mm/s^2, you get close to 20,000 mm/s^2. Is that what you meant?
If you want the shock to end and the response to be calculated beyond, you can't use the formula that you have used, but you can break it up into a 3 step simulation, Step 1 ramps acceleration up to 20 G in 11 ms, Step 2 ramps down to zero acceleration in 0.1 ms and Step 3 keeps zero acceleration till the end time of 100 ms.
It is better to use these settings under Analysis Settings.
I'm running the model with these changes now. It converges on the first increment, then I stopped it to attach the ANSYS 17.0 archive. I will let it run out to 100 ms and reply if anything interesting happens. It might have a problem at the beginning of step 2.
December 29, 2018 at 5:01 amRavikishanSubscriber
December 30, 2018 at 12:15 ampeteroznewmanSubscriber
My doubt remains about ramping up to an acceleration of 20,000 G in 11 ms.
Double integrate the 11 ms acceleration ramp; the device displacement is 3.95 meters!
Do you have a 4 meter (13 foot) long sled?
What happens once you reach 20,000 G in 11 ms? What is the profile after that?
The sled carrying the device is traveling at about 1000 m/s at that time.
With zero acceleration it will travel another 10 meters in next 10 ms.
The device has a mass of 3.385 kg, so to create the 20,000 G acceleration requires a force of 664 kN or 149,300 lbf.
I expect this is an explosive method (pyro) to create that much force on this device.
You say you are using linear elements to keep the node count down. I recommend you take all the thin bodies like PCBs and cover plates and make them midsurface models in the geometry editor and mesh them with shell elements. They will have more accurate bending response and take fewer nodes than the solid elements currently in the model.
In the model I left you above, I mistakenly used the Y-axis for the acceleration instead of the Z-axis. I also only used 20 G for 11 ms. Below is the simulation result from that run, which took about 20 hours on a 4-core computer to compute out to 15 ms. I hid a few of the outer parts to show the body with the largest deformation. It looks like a part of the PCB is missing. When you add the extra piece back in, it might stiffen this up to the point where it doesn't penetrate the other body, especially when you switch from Y to Z axis acceleration.
December 30, 2018 at 5:48 pmpeteroznewmanSubscriber
The solver fails after 1.7 ms having ramped up to 3,090 G on the way to 20,000 G at 11 ms.
December 31, 2018 at 4:27 amRavikishanSubscriber
i've changed the midside node to kept. and trying for a complete solve of 100 ms, it is solving from saturday
June 22, 2019 at 12:04 pmRavikishanSubscriber
i have difficulty in understanding your reply (bold-underlined below) regarding the double integration, sled velocity, displacement on sled, force transferred on the object. can you share any references for understanding the above topics. also will MSUP solve faster than this non-linear solution for a simplified view of the problem under study.
Do you know about Modal Superposition (MSUP) solution method for linear analysis? - i referred it from ansys help that modal super position will yeild a better solution
June 22, 2019 at 3:30 pmpeteroznewmanSubscriber
1) MSUP does not yield a better solution, it yields a solution in less time than a Full transient analysis if the model is completely linear. If the model is not linear due to a nonlinear material, frictional contact or large deflections, then you will not be able to run a MSUP transient analysis, you will have to run a Full transient analysis.
2) In your first post you said, "I tried to run the saw tooth shock with 20000g for 11ms." I just took a second look at the image you posted below that statement and I see it has 2.1582e+6 mm/s^2 of acceleration. If I convert the number in the image, that is equal to 220g not 20,000g that you wrote.
In either case, the equations of motion are simple. Below are the Mathcad formulas I used, first with the value you wrote.
Second with the value from the image.
After 11 ms, the acceleration is zero, so the velocity at 11 ms is the constant velocity from then on. If you want to know how far it travels in the next 10 ms, in the first case you multiply 0.010 * 1,000 m/s to get a 10 m distance traveled.
- 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.
- How to calculate the residual stress on a coating by Vickers indentation?
- Errors – Reinforced Concrete Beam
- Solver Pivot Warning in Beam Element Model
- An Unknown error occurred during solution. Check the Solver Output…..
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Large deflection
- Colors and Mesh Display