much appreciated your help, own you a bottle of scotch for your time
Unfortunately these tests been done for a while and I was asked to simulate them.
I was not involved in the load profile set up and the ‘whys’.
I do understand these bending tests do not represent the fatigue properties of the pipes, I guess they wanted to have some more fancy method (and more data) rather than just simple bending until it fails ( or the standard low cycle fatigue load method)
Your Pipe 05 model - Run 4-100 sec looks promising to the final solution, but I think it will not lead to the real deformation because the contact surfaces are much bigger than just those small ‘dots’.
It looks to me -after your hard tries-, that Simscale does not like this 90 deg pipe-pipe contact,
it works nicely for non linear material and displacement boundary condition, could this be a bug?
(also noticed, that the sin function I used has to be +4000 for the initial offset as it starts form 4kN not 4N)
The small indentations are needed to stabilize the initial solution, of course, the contact area will spread as the load increases. The simulation is already set up a allow for this.
You’re right about the load profile equation. I missed the units on the plot in your post. Taking the ‘kN’ into account the load profile should be:
-1000 * SIN(2 * 3.14 / 100 * t) - 10 * t - 4000
The 90-degree pipe contact arrangement is a type of Hertzian Contact. This type of problem is more difficult to solve because of the point contact between the two parts. This is not a bug, it is just the nature of the physics involved.
I have updated my project with another example.
[!!!THIS LINK IS NO LONGER AVAILABLE!!!]
This time I took the deformation to 10 mm. For reference, the pipe outside diameter is about 28 mm.
This has been done with a linearly increasing displacement load. I expect the same thing is possible with the sinusoidal load profile provided above. You just need to decide whether the extra computation time is worth it, given it will make no difference to the final result.
The 4 kN initial load is too abrupt for the simulation to get started. You can modify your load profile equation to ease the load in at the start. For example, the equation below works for me (with auto time stepping enabled).
I managed to run the simulation (with the same set up as yours) with a table load till 60 sec and it took 800mins
what would you do to speed up this process? coarser mesh, bigger convergence (like 0.001), or what options do I have?
Your simulation will run much faster (and be more stable) with a first-order mesh but the results will not be very accurate. Sometimes it is beneficial to start with a first-order mesh to get some preliminary results. Then you can do a final pass with a second-order mesh. Please see this post for more details.
Note that the plastic transition zone (circled in the image below) will take much longer to solve than the bits either side.
Using a coarse mesh will reduce the computation time. You could drop back to one element through the thickness of the pipe but only with a second-order mesh. And even then I don’t expect you will save much, your mesh is already pretty efficient.
I took a quick look at your simulation setup and I can see you are not using the center roller contact (only the support roller). Therefore your non-convergence issue (and possibly long computation time) is probably coming from this contact. You could try to improve this region to make it more stable. For example:
Provide a larger contact surface area to reduce the local plasticity.
Change the bottom of the pipe to have a small flat face. This may allow the pipe to slide over the roller more freely.
You could increase the residual (by a factor of 10 or 100) but that would be a last resort. Non-convergence is usually a sign that there is something else wrong and increasing the residual usually won’t help. The default value is generally pretty good for most situations.
Hi @tenshinshoden,
in addition to what @BenLewis said the biggest time waster seems like the extremely high number of iterations per time step (up to 600 and more than 100 in average) - certainly one reason is that you are using penalty method for both contact nonlinearities - which is more stable, but also slower than newton.
I guess you already tried to at least use Newton for the “Contact nonlinearity resolution” and it failed (since 2nd order mesh) - if not I would do that.
Additionally, as the exact resolution of the contact should not be one of your major concerns and as you don’t have large relative sliding on your contact surfaces, I would try to “force the contact convergence”, by specifying a fixed number of fix point iterations (under “Nonlinearity resolution” you find “Geometry reactualization”, set that to manual and specify some low number for that, maybe 2-3).
This will certainly speed up the solution time and should in your case also be acceptable from a error point of view.
I used your very set up for my simulation hence I do not get this:
I took a quick look at your simulation setup and I can see you are not using the center roller contact (only the support roller). Therefore your non-convergence issue (and possibly long computation time) is probably coming from this contact. You could try to improve this region to make it more stable. For example:
Provide a larger contact surface area to reduce the local plasticity.
Change the bottom of the pipe to have a small flat face. This may allow the pipe to slide over the roller more freely.
with shaving down the surface of the contact surfaces the simulation runs in a reasonably time.
many thanks for all the help and time that @BenLewis and @rszoeke helped me to get the best set up.
I still have many things to learn and to understand about this platform.
I did not have this issue with diff packages for the same set up (FEMAP, NX Nastran in CAD, seen comsol too)
would the development team have a look at this weakness of this amazing package, cos everything else is superb ?
…or do I have to find a workaround for this to satisfy my simulation needs?
hope my voice can be heard!
How are the other packages handling things like that? I have only experience in Abaqus and Ansys but even there you have to be very careful not to apply a high force on a single node let’s say in a Hertzian contact model causing singularities. I mean that’s nothing very dramatic - you can fix your geometry in Onshape and use the import tool to directly upload your updated model which is a pretty good workflow I would say. Any opinions from your side?
But was this in parallel? Usually Code_Aster scales better than Nastran using MUMPS afaik. If you like let’s do a study together and see if Nastran and FEMAP really are that much better also taking into account the cost for licensing etc.
With regards to Nastran, were you using a first or second order mesh? A first order mesh will solve much quicker. In your SimScale project you are using a second order mesh, this will produce much better results than a first order mesh but there is a big trade off with computation time. If you want to compare the two systems you will need to use comparable meshes.
(with the same set up as yours) with a table load till 60 sec and it took 800mins 
Usually Code_Aster scales better than Nastran using MUMPS afaik. If you like let’s do a study together and see if Nastran and FEMAP really are that much better also taking into account the cost for licensing etc.