Thanks for taking a look at this simulation. You have done some really great work here!
Also, your tip on switching from relative to absolute residual is very useful.
I had disabled geometric non-linearity as a troubleshooting measure and had forgotten to enable it again. I should have recognized this from the linear force-displacement curve. Rookie mistake. Well done on picking this up.
Because there has been a lot of options discussed here I thought it was worth summarizing where we are at. As I see it there are now three workable solutions, each with advantages and disadvantages.
Remote Displacement, Second Order Mesh - Fast and accurate but cannot use friction.
Physical Contacts, Fine First Order Mesh - Fast but too stiff, friction possible.
Physical Contacts, Second Oder Mesh - Slow but most accurate, friction possible.
The images below show a comparison of the results obtained from the three different methods.
Peter (@pborgens), depending on what you want to achieve you should be able to get it done with one of these methods. I suggest starting with the first order mesh. You may be able to improve the accuracy by making the mesh even finer.
Great work @BenLewis! Very nice to see how the results from remote displacement matches the physical contact one. If I have to do the analysis without considering friction, I would for sure go for the former option
first of all I’d really like to express my gratitude for your great help/support. I’ve rarely found such an active, friendly and helpful community in a rather technical support forum. I’ve been studying your contributions to the topic over the past few days and learned a lot. Today I also talked to the engineer who actually constructed our setup (which is, being in a UHV cryostat, not easily accessible) and we found out that the real situation is a bit different from the problem we’ve been looking at in our simulations so far.
The most “critical” difference is the fact that the free/sliding end of the spring does not contact the steel support plate in the initial state. Instead, there is 1mm of free space when no force/displacement is applied to the center of the spring.
I’d like to understand how that influences my model (also in the light of Ben’s idea of the stress being too high). As I’m still quite new to FEA, my question is: is it still possible to use a static analysis for this situation, or do I have to use a “true” dynamic simulation now? My idea would be to just create a more accurate 3d model of the setup, then re-run the analysis with second order (nonlinear) physical contacts. Any suggestions how to do this transition would be highly appreciated.
Regards,
Peter
Sure you can do also this transition phase. All you have to do is to upload this time a model with a 1 mm gap between the steel plate and spring. Furthermore, I think you only need to perform a nonlinear static analysis here since your applied loading is not fast that it may produce vibrations in spring. If in real life the movement of lower steel plate is fast then you may have to consider dynamic analysis.
Hi,
so here’s a successful run with the new spring model with a gap. I’ve been using a 2nd order mesh (in fact, most of the settings are the same as @ahmedhussain18 's since I copied his project. Now trying to introduce friction… which might be difficult for a physical contact which is a 1mm gap, initially. By the way, how do you make those animated gifs of the simulation results? Looks like I missed an export feature…
I’m confused about the results you shared in your previous post. Here are my observations:
The pressing plate moves vertically a distance of 2 mm, but your plot shows a maximum travel of just over 2.5 mm.
There is a 1 mm gap between the free end of the spring and the fixed sliding surface. From geometry, the pressing plate will move approximately 0.5 mm vertically before the free end of the spring engages with the fixed sliding surface. Your plot shows this engagement occurring at around 2 mm.
Your spring rate (once engaged) is very high compared to the results obtained with no gap. I would not expect such a large change.
Maybe I have misunderstood your application. If so, please let me know.
I’m not sure what the friction coefficient for beryllium copper on steel is. As such I have run your simulation with three levels of friction. The results are shown in the plot below. This plot shows the sensitivity of the system to the level of friction.
These simulations take quite some time to solve (anywhere from 6 to 10 hours depending on the level of friction). However, I have found the current setup to be quite robust so I would stick with using a second order mesh with physical contacts.
I have to apologize, just now found out that the gap in my new spring model is actually 2.5mm wide, not 1mm. My engineer got that info from the manufacturer but didn’t tell me, just gave me the new CAD model (the spring is also shaped slightly different to the first one, to reflect the true shape better). So to me it appears that both results were correct, just for different situations… However, if there is some obvious mistake in my simulation setup I’d be really glad to know since i don’t know many of the details of the process yet…
Thanks again for your help,
best regards,
Peter
Your setup looks pretty good. If you have trouble with convergence or you want to reduce the solution time you could try some of these changes.
Reduce your penalty coefficient from 1e14 to 1e13. This will result in slightly more penetration between physical contacts but will solve quicker. I found the penetration with a penalty coefficient of 1e13 to be quite acceptable. You may want to try reducing this even further to solve quicker. It’s a bit of a balancing act.
Increase the maximum number of fixed point friction iterations from 10 to at least 20. This will help with convergence. You will find this setting under Domain > Physical Contacts > Friction > Coulomb > Friction nonlinearity resolution > Fixed Point > Maximum number of iterations.
Increase your mesh size so that there is only one element through the thickness of the spring. This is not recommended for first order meshes but I generally get good results with second order meshes. The settings I used were - Maximum element edge length [m] = 0.0002, Minimum element edge length [m] = 0.0001.
Reduce the size of your slave surfaces as far as possible. The less slave nodes the quicker your simulation will run. To do this you will need to split your slave surfaces in your CAD tool.
Reduce the number of computing cores from 32/16 to 2/1. This simulation does not require much memory. This will save you core hours.
Change your time step definition from auto to manual. When your settings are correct you will not need auto time stepping.
I hope this helps. Please let us know how it goes.
Not sure here though. With second order this machine combination could be small. 1 core will work way slower. If the memory distribution is not a big problem considering there are less DOFs, I would recommend to use MUMPS on 8/4 if the mesh size is bigger than 60K nodes otherwise 8/2. This will decrease the computation time at least two times if not 4.
i’ve done a couple of runs and run into a problem: there’s a warning about my mesh (orphan nodes), which makes some runs fail, while others complete without problems. Looking at the solver log, I don’t really understand what the problem is (apart from the fact that I should try a different mesh). Could anyone please explain to me why my simulation runs failed?
One more question: I’m now using different different CAD models for simulations which differ only by the position of one plate (the slider fixation plate, i. e. the plate where the free end of the spring slides). Would it be possible to get different situations by simply using the displacement mechanism for that plate? Like, a fixed (in time) displacement of this plate in Y direction for each run?
best regards,
Peter
The error occurred since the solver exceeds the fixed point iterations and not due to existing orphan nodes which is just a warning in this case. The error says:
!-----------------------------------------------------------------------------! ! <BoucleContactError> <MECANONLINE9_11> ! ! ! ! Stop by failure in the loop of point fixes on the statute of contact. ! ! The total base is saved. It contains the pitches archived before the stop. ! !-----------------------------------------------------------------------------!
The reason of termination after this divergence is the use of ‘Manual’ timestepping scheme. In the case of Manual, solver will not try to cut down the timestep in order to get convergence. You can switch it to ‘Auto’ in order to make the simulation running even after this divergence. Please note that simulation will take a long time as it already did in order to reach the final time and it may fail also after that.
Furthermore, looking at one of your results your stresses looks odd. The main reason is that your mesh is quite coarse. You may need to reconsider mesh refinement here.
For an easy convergence, you can consider increasing the iteration criteria to 0.05.
@ahmedhussain18
Thank you for your quick reply. I agree that the mesh is rather coarse, my idea was to start with something less demanding in processor time and then move to finer meshes… What do you think about my second question?
Yes you can do that. All you have to do is to initially move the plate along y-axis via function definition and make it constant afterwards. And then start moving the lower plate. For example, giving 0.0012t*(t<=0.5)+0.001*(t>0.5) under y-direction formulation will move the upper plate to 1 mm until 0.5 sec. and then it will remain there afterwards.
Then your lower plate formulation would look something like this: 0.002*(t-0.5)*(t>0.5) when you run the simulation until total time period of 1.5 sec..
That sounds like a bit of a complicated solution to me… isn’t it possible to just set the displacement of that plate to 1mm (with no time dependancy)? I’d prefer to have only one displacement of that kind per simulation, and keep the time dependancy for the pressing plate.
please see the following simulation in my public project [!!!THIS LINK IS NO LONGER AVAILABLE!!!] :
Spring12 - REM - Run 8 - DY 430e-5 T1 0.24
This simulation is set up to do what you are asking for. This approach is very quick but you cannot use friction. You also have to tune the vertical translation rate of the fixed silder so that there is no force applied to it in the first (non contact) stage of the simulation (see plot below).
@pborgens, yes you can do that in the very first timestep by giving the displacement value directly 0.001 which will actually perform something like this 0.00110t*(t<=0.1)+0.001*(t>0.1). Make sure then you ramp the moving plate as 0.002*(t-0.1)*(t>0.1) otherwise it may diverge or may not even following the older method. This case is easily doable while in absolute error convergence criteria whereas the solution initially diverges a lot in case of relative convergence criteria. Reason? no forces in the system. Also make sure to switch to auto timestepping before doing this.
I got confused about what you were asking for. Now that I understand I can see my answer does not make sense. The approach suggested by @ahmedhussain18 is the right one. Sorry about the confusion.
Hi again,
I decided to revive this old project after taking a long break from simulation problems in general due to being very busy with experiments. This time i want to move the “pressing plate” horizontally, sliding against the spring, in contrast to pressing the spring from the top (see the last simulation, “Type 2 gap 2.5mm no fric”). After making a new CAD model and mesh, i tried to set up the simulation, first without any friction. However, i run into a “singular matrix” error, and would be thankful if anybody could give me a hint how to fix it (and maybe additional optimization hints/ideas). Any help would be much appreciated!
