Limiting tension at a support and dynamic factor application


Good afternoon,

I have produced the model attached and due to the skew I am getting some tension at the supports, as expected. I would like to however define a limiting value of tension at those locations so that anything above said value gets redistributed elsewhere. How do I do that?

Can you also please double check that I have applied my moving case correctly. I have defined two lanes and a vehicle and a moving load. Trains can travel along either lane and both could be loaded at the same time which I think I have entered but could you please just check. 

I was planning on applying my dynamic factors by hand. I can see the program allows you define different factors to different elements however this alters my deformed shape oddly. How is best to apply these factors?

My dead loads differ from my hand calculations by approx 7%. Is there a case where the elements are too thin they would not be counted?

Kind regards


Hi ,

To limit the support reactions you can use Boundary >> Point Spring, and then choose type as Compression Only or Multi-linear where you can specify the maximum reaction after which the support loses stiffness and redistributes. Please be aware that this is a type of nonlinear behaviour and this means that some of the assumptions of Linear Static Analysis are no longer valid and you will have to make appropriate modifications to your model to account for this. For example, the principle of superposition is no longer valid, thus, you will have to generate each loading scenario as an individual load case to be solved. You can no longer use Load Combinations for your load cases which have been solved separately.

Yes, everything seems OK with your moving loads.

Yes, you can specify the dynamic factors in the program, but we are not sure we understand your concern about the deformed shape. Can you please provide a screenshot and some more clarification on the issue?

Kind regards,
Technical Support Team

Good morning,

Does this mean, I would have to convert all of my moving load analysis results into static results. and then like you said analyse each load separately and then add the effects together at the end to get for example the maximum bending moment?

Kind regards

Hi ,

There are two items to note in relation to the Moving Load Analysis when it comes to nonlinear supports:
1) The moving load analysis is based on Influence Line method, which is a linear static analysis approach and the nonlinear supports will be considered as linear springs for the purpose of Moving Load Analysis, i.e. the nonlinear cutoff of tension will not be considered for the moving loads.

2) To consider the limited tension capacity you will have to export static load cases for the given effects and then check the effect for those, where the tension limit will be applied in the static analysis.

In the end, you will have to export static loads for the moving load effects of interest, factor those and combine them with the other effects (i.e. dead load, surfacing, etc.) into individual Load Cases to be analysed for the nonlinear supports.

Overall, it is generally a cumbersome procedure to deal with nonlinear effects and in many cases the effects are small enough that the permanent loads would cancel any uplift so that nonlinear spring definition is not necessary. However, this needs to be backed up with inspection of the structural behaviour and results and through engineering judgement support a decision not to model compression only supports.

On a previous note, I have just noticed your question on the dead loads. There should be no reason for any dead loads to be excluded. Please review your model and try to establish the reason for the difference. If you are still facing problems, feel free to send us your hand calc against the model results and we can try and help.

Kind regards,
Technical Support Team

Do you have any literature to explain the above. I am not sure how to define this correctly. I have 8 supports and want them all to be limited so that no tension is experienced in any of them and then I can take a look at the effects.

RE the DL's this is fine now.

In addition, can you take a look at my results for my moving load analysis. When analysing the effects of the combination (CB min Live load), you can see that there is hogging in one of my cross members and the trimmer beam towards the bottom right support which is not there in reality. Is this an error with the modelling of the shell elements as they are not quadrilateral around those locations due to the skew?

My deflected shape reflects these results. As the deflections are minimal it seems okay to ignore them but it does induce hogging.

Kind regards

Hello ,

I am afraid there is no specific literature we can provide on this, however, you can refer to any publication on Linear Static Analysis and Nonlinear Static Analysis.

The issue of superposition no longer being valid can be easily illustrated with a two-span beam, supported on compression only supports. If we examine three load cases - one with UDL on the left span, one with UDL on the right span, and one which is loading on both span, we observe the following results:

Case 1 - load on left span - we can see two equal reactions of 60kN as the 3rd support simply experiences lift off.

Case 2: Load on the right span - similar to case one but for the second span

If we combine these two load cases using a Load Combination - linear combination of results using superposition, then we get the sum of the two results seen above:

However, if we solve a third case which is the combination of the first two as combined load case, we will see that the reactions at the ends are reduced while the middle support has more load:

This is because of the nonlinearity of the solution due to the compression only springs. In the individual cases, each support which is away from the load is experiencing lift off, generating no tension reaction. However, when the two spans are loaded together, then there is no lift off but instead there is a reduction of the end reactions due to the favourable loading of the adjacent spans.

So to deal with this, you will have to go to Loads >> Static Loads >> Static Load Cases and define individual load cases for each design combination that you want to obtain results for. Then in each load case define all loads to be considered with factors, i.e. 1.35 SW + 1.35 SIDL + 1.5 LL in a single load case. And this for every combination.

To make this easier, in MIDAS we have the function Load >> Static Loads >> Using Load Combinations, which allows you to define new load cases based on the existing load combinations with the specified factors for each combination. You can find information on this function in the Online Manual:

As for the hogging moment at the trimmer beam, this is caused by the Rx restraints at the supports, not the plate elements. Due to the skewed layout the major bending of the beam has a component corresponding to the Rx reaction. You can see that when you load the beam, the load will distribute towards the support which is not a pin in the direction of the trimmer beam.

You can also see that there is a reaction with similar magnitude to the hogging moment in the beam due to the moving load:

To resolve this you need to either switch off the Rx restraint in the support or apply a moment release to the beam.

Kind regards,
Technical Support Team

Creation date: 11/12/2018 4:51 PM      Updated: 11/13/2018 3:29 AM
128 KB
425 KB
42 KB
42 KB
41 KB
40 KB
Main Model[1].mcb
1 MB
19 KB
16 KB
Bridge supports.PNG
3 MB
14 KB
36 KB
Main Model - release 2.mcb
1 MB
63 KB
100 KB
35 KB
Model V3.mcb
961 KB
43 KB
16 KB
Model V3[1].mcb
1 MB
277 KB
119 KB
48 KB
Model V3[1].mcb
959 KB
Model V3[1] (1).mcb
955 KB