Non-linear analysis of a masonry arch bridge

AndreaC91

Hello,

I'm trying to analyze a masonry arch bridge by using a plane model. As of now, I have modelled all the components with linear elastic materials but I'd like to use a compression only model at least for the masonry arch.
Is this possible in Mecway?

Secondly, is any constitutive model for concrete available in Mecway?

Thanks,

p.s. I attach for reference the file I'm working on.

disla

Hi AndreaC91,

Mmartin has a nice example with only compression and very similar to yours in the forum.

Clay arch simulation
https://mecway.com/forum/discussion/1089/clay-arch-simulation

Be careful , I have seen some nodes disconnected on the lower corners. You can use the tool Open cracks in the View menu to find them.

AndreaC91

Thanks for your reply. I will correct that flaw as soon as possible.

I saw the clay arch simulation file but it is a 3d model. I was wondering whether it is possible to model compression only materials also in 2d models.

Regards,

mmartin

Dear Andrea:
I am experienced on simulating 3d archs using compression only material.
Maybe soon, I expect to get a new mfront compilation linked to MW with mazars material model ready to use. Then we will be able to reproduce cracks on brittle materials.
Manuel

disla

I think it is possible with custom model definition, calculix and nonlinear.
Line load doesn't work .
Find example with random material properties for a compression only arch.
You need to erase the material on the main tree to avoid conflict.
Check it carefully. I never try this.

AndreaC91

Thanks disla.
I've tried to modify the model as suggested but it doesn't run the analysis. I'm still testing the free edition and the model has less than 1000 nodes. However, when I try to save the file, I get an error message due to the number of nodes.

Please find here attached my modified file. Doesn't it run just because I'm using the free edition or for some other reason?

Victor

It's not because of the free version.

The error "element set ARCH has not yet been defined." is because Mecway didn't generate an ELSET for ARCH which is because it doesn't generate duplicate ELSETs and already has Element_Selection which is the same. So modify or remove the Element_Selection named selection.

It's also lacking Z displacement constraints but that's a subsequent issue.

AndreaC91

Thanks Victor for your feedback. However, even removing the Element_Selection named selection, the analysis doesn't run. For sure I'm missing somethig. I get this message error:

*ERROR: too many cutbacks best solution and residuals are in the frd file

In addition, after running the analysis, I can't save the file anymore and I get this message:

Cannot save.
Free edition: Cannot solve, save or run sripts on models with more than 1000 nodes.

The last version of the file is here attached. Thanks for your support.
Andrea

disla

It works for me adding the named selection call "Arch."
By your description seems your analysis is running but not converging. That's a different problem.
Check the time settings in Nonlinear.

Regarding the number of nodes, I would try symmetry if you are just playing. Loads may not be symmetric but... just for testing could be enough.

Line load do not work. Try pressure or traction. Expand the geometry to see the thickness of the shell and you can select the area.

File attached.

AndreaC91

The strange thing is that if I work on the file you sent before (just by adjusting the mesh and modifieg material parameters), the analysis runs smoothly and converges.
On the other hand, if I try to set a new file with the same features you provided in the one you sent, the new analysis doesn't converge.

AndreaC91

I worked out the issue: it was due to lacking of Z displacement constraints. Now the analysis converges properly.

I still get the error message when I try to save and I don't understand why since the model has less than 1000 nodes, but this is a second order issue at the moment.

Since I'm novice with Mecway, is there any reference to help me through the Custom Model Definition?

disla

The custom model definition, custom Step, Custom element,.... are used to include in the .inp file that MECWAY prepares and send to the solver (Calculix), commands and functions that are still not available directly in the MECWAY GUI. They do not work if you are running the internal solver.

To be able to use those new capabilities that Calculix offer, you need to learn how to set up an analysis for Calculix (or at least have some general idea)
COMPRESSION_ONLY set up can be found in the ccx Manual v 2.19 page 245

https://www.dhondt.de/ccx_2.19.pdf

prop_design

as far as the issue with not saving. check in solution view how many nodes there are. the calculix solver expands shells to solids. so you end up with a lot more nodes than what you start with. it good be that in model view you are below 1000 nodes and in solution view you are way over that.

AndreaC91

Thanks everybody for your reply.

Regarding the number of nodes, in the log file produced after the analysis I can see 56747 nodes, which corresponds to what you were saying. However, I think I will work out this issue with the complete software.

I'd like to have another clarification on the Mecway functioning that I can't find in the manual.
In the arch analysis there are mainly two load conditions: self weight of the model and variable load due to traffic. I'd like to run an analysis by applying the self weight first and then the traffic load. This because the self weight stabilizes the arch, while the traffic loads tend to produce tensile stresses.
As far as I understand, the CCX solver allows to increase all loads at the same time.
Isn't it possibile to run two different load steps, the first by applying the selt weight only and the second by applying the traffic loads after the self weight is already applied?

Thanks,

disla

You can do that easy defining a load table.
When Nonlinear Quasistatic analysis is active, loads can be entered as a function of time by means of a function or a table. Wait some seconds before activating the pressure load. You have a lot of possible combinations. Load functions are also available like heaviside, sin, cos, ...if you want to introduce them in a more complex way.

Once you familiarize with the software you can also introduce a load that cross the bridge. It is explained in the forum. Mpg video Attached.

https://mecway.com/forum/discussion/comment/5741/

AndreaC91

Thanks disla, I've defined the load tables and it works fine.

If I have understood correctly, in defining the Compression_only material, just the Young modulus and the tensile strength are specified. Doesn't the Poisson coefficient influence the analysis too?

disla

Good question. Don’t know sorry.

For questions more related with the theory involved you better ask at the Calculix forum directly. There are real experts there who can give you an answer or address you to some book or paper related with the subject.

https://calculix.discourse.group/

AndreaC91

I'll report a few strange things I have found by analysing and comparing the results of the non linear analysis with a linear elastic one.

1. In terms of stresses over the arch, the two solutions are equivalent, except at springings, where the non-linear analysis provides smaller stresses (about 15%). However, in the non linear analysis, at midspan I get a tensile stress of 0.03 MPa even though I've specified 0.02 MPa as maximum tensile stress value in the compression only setting. What do you think about this?
   
2. If I measure the volume of the arch (29.24 m3) and calculate the corresponding mass by considering the density value specified in the custom model definition (2100 kg/m3), I get a total mass of the arch equal to 61404 kg.
   By calculating the mass of the arch on the basis of total vertical reactions, I get a value of 42628 kg, about 30% smaller than the real one.
   I don't understand why I get this discrepancy. Since the weight of the arch is much smaller than the weight of the backfill, the global error in terms of reaction is low (about 5%), but I can't understand why there should be any difference.
   Looking at the value of the error (30%), it might be due to something related to the shell thickness (3 m). Any hint on this?
   
   
   

disla

Could you share your final set up ?
It will be easier to follow.

AndreaC91

Yes, sorry, I forgot to attach the files (NL = Non Linear; L = Linear).

disla

1-Ccx Manual:

The correction term is in fact identical to the term used to cut off tensile stresses for penalty contact in Equation(203) and Figure (130). Replacing “overclosure” and “pressure” by “principal strain” and “principal stress” in that figure yields the function f.

I guess “absolute value of the maximum allowed pressure” parameter should be read as : “absolute value of the maximum allowed principal stress”
It agrees with the result. If you just show the Arch in the Solution tree the values adjust for the arch.

2- ¿How do you get the reaction forces from shell elements?

AndreaC91

1) In my analysis, at time 1.0 s, the principal stress 1 at midspan is 3.2 MPa, which is the same of the tangential stress "stress_tt".



2) I was looking at the sum of external forces in the y direction over the named selection BASE-SX.

disla

Weight and reactions are very close too. It think it will get better with some refinement.
You can create a New table in solution.

Check in the manual.

AndreaC91

Sorry but I'm not following you. Can you please clarify what you have done?

disla

I found your problem.

You have not defined the element selection called ARCH.
Your custom model ELSET is pointing to nowhere.

Maybe Victor can take a look at this as it should fail and it is not.
Take into consideration these are kind of tricky things are out of normal Mecway procedures.

AndreaC91

Even if I define the Named Selection ARCH, I don't get any difference in the solution.
Did you manage to obtain different results?

My model still provides a wrong result of the arch weight, that I measure by using the function Sum applied to External forces in the y direction over the named selection BASE-SX.

In the same way, the maximum principal tensile stress at midspan (and in the same way the tangential stress, which should be equivalent in that point) at step 10 (t=1 s) is equal to 0.032 MPa, larger than the defined 0.02 MPa.

MikeMcMullen

If I recall correctly the tension limit of the compression only material type is not linear, but more like a yeild stress of a metal like material, increasing gradually. I think this is so that the slight increase in stress with strain allows for convergence, which is difficult for materials that have a negative stress strain slope. I think the compression like behavior of tension only materials is similar. For problems I have run where arching is an issue I have had to either have reinforcing to make the behavior modeled true, or reduced the tension so that the value achieved was reasonable. Either way the stress strain behavior does not match actual behavior of these materials, which for concrete reaches a peak of perhaps 0.1 times the compressive strength, then falls to perhaps 0.04 of the compresssive strength, then falls gradually to 0 at a strain of perhaps 0.02'/'. This works for lightly reinforced flexural sections where the yeild force in the reinforcing is roughly equal to the tensile strength of the concrete coded in. For arching the deformation induces an axial force which accomplishes the same effect as the nominal reinforcing and the best method is to adjust the material tensile capacity to achieve reported peak tensile stresses less than 0.2 of the material modulus of rupture.

i.e. The tensile stress strain behavior is not accurate for the compression only material, but one that allows for a solution. The method I use is to run as a normal material, and accept the load at which the modulus of rupture is achieved as the limit, or run as a compression only material with the tensile strength approximately equal to that provided by any reinforcing.

Victor

@AndreaC91, principal stress 1 at that location reduces to 0.019 MPa with a Refine x2 applied. I guess the tensile stress is being tested at integration points inside the element so it might be higher at the surface.

BASE-SX is only one side's support. Not sure if you doubled that? I get 801kN as the sum of external force Y on all the Y constraint nodes (displacement_nodes(2)) at t=0.5 s. Is that the erroneous value?

I'm pretty sure density is always mass per unit volume, not area, so I wouldn't expect thickness to be a problem.

disla

Hi Mike and thanks for your comment.

I started again from Andrea file and one additional refinement makes the big difference.

@Andrea.

I have set up the whole model as Compression only and everything keeps below 0.02 MPa.
If I set only the Arch, it exceeds punctually to 0.024MPa but it is in a corner where the node is shared with a regular element (Node value is averaged so it can exceed 0.02Mpa.

AndreaC91

With respect to the tensile stress value, I can't test the refinement effect due to the limit on the number of nodes in the version I'm currently using but, if this is the solution, there is no big issue.
However, my main concern on this point was that both the compression-only analysis and the elastic analysis provide the same tensile stress of 0.032 MPa.
This sounded strange to me but probably it is just a matter of refinement.

The problem on mass is of major importance to me and I need to work it out.

@Victor If I measure on BASE-SX the sum of external force Y at t = 0.5 s, I get 1610 kN. BASE-SX does correspond to one side's support.
On the other hand, if I measure on Displacement_nodes(2) the sum of external force Y at t = 0.5 s, I get 3204 kN, which is approximately the double of the value I obtained on BASE-SX.

Now, if I run an elastic analysis, the sum of external force Y over BASE-SX is 1702 kN, which should be the correct value from hand calculations.

What do you think?

Thanks,

MikeMcMullen

I believe the element properties are applied to the element, not the node. So if the stress in the element is under the tensile stress limit a corner could easily be over it. For a location where the stress does not vary drastically over the element these corner stresses will not have such a large error. The node in fact is a part of all the surrounding elements and constraints and the stresses and strains will never be right at a node. This is why many models have a finer mesh at these areas with rapidly changing strains or stresses.