Pipe bending simulation


#41

Hi Richard (@tenshinshoden),

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).

-1000*sin(2*3.14/100*t)-10*t-4000*(t*(t<1)+(t>=1))

Note, this equation will ramp in the 4 kN load over the first 1 second.


#42

Dear Ben (@BenLewis)

I managed to run the simulation :sparkler: (with the same set up as yours) with a table load till 60 sec and it took 800mins :smiley:
what would you do to speed up this process? coarser mesh, bigger convergence (like 0.001), or what options do I have?

Best Regards,

Richard


#43

Hi Richard (@tenshinshoden),

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.


#44

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.

Best,
Richard


#45

hi Richard (@rszoeke)

yes, I tried Newtron and it failed.

I cannot see anywhere the Geometry reactualization

thanks
regards,
Richard


#46

Hi @tenshinshoden,
there it is:
number_iter

Please also try @BenLewis’s suggestions.

Best,
Richard


#47

Dear Ben (@BenLewis)

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.

Regards,

Richard


#48

Richard,
thanks!
Regards


#49

Hi Richard (@tenshinshoden),

You have a lot of copies of the pipe bending project. It would help if you shared a link to the project related to your post.

As far as I can tell the project you are working on is this one.

https://www.simscale.com/projects/tenshinshoden/ben_help_30-07-2018/

And the simulation you are referring to is Copy of Pipe_06 - working diplacement - Run 1.

In this configuration, you have made a number of significant changes from my original project. Including:

  • Removal of the physical contact between the center roller and the pipe.
  • Addition of Boundary Condition 5 to fix the center roller in place.
  • Addition of Boundary Condition 1 to load the pipe directly (instead of via the center roller).

#50

hi all,

I tried to make my geometry much simpler, but still getting some contact errors,
although it is much quicker now!

https://www.simscale.com/projects/tenshinshoden/ben_help_30-07-2018_1/


#51

Dear All,

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 :slight_smile: ?

…or do I have to find a workaround for this to satisfy my simulation needs?
hope my voice can be heard!


#52

Hi @tenshinshoden!

Can you elaborate what “issue” you mean in particular? We are trying to help wherever we can.

Best,

Jousef


#53

dear Jousef,

in order to achieve a 1-2h simulation run I had to shave off the diameters, to have small flat contact surfaces at the beginning.

thanks,

Richard


#54

Got it @tenshinshoden!

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?

Best,

Jousef


#55

hi Jousefm,

I used Nastran in CAD for a while and it solves the hertzian contact much quicker.
also seen FEMAP (Nastran too) doing the same thing.

Best,

Richard


#56

Hi @tenshinshoden!

But was this in parallel? :wink: 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.

Cheers!

Jousef


#57

Hi Richard (@tenshinshoden),

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.