Moving loads Analysis. Bridge crane.

disla

Hi,

Just wanted to share with you something I thought wasn’t possible in Mecway. How to set up a load-train simulation (not sure about the name in English “moving loads”?¿?).
In this case without the need to do Dynamics or modelling the agent of the load itself.
In my case I’m interested in the effect on a bridge crane but it could be extended to a wide range of applications.

Traction is required because the load depends on position. Traction, needs to be applied to shell elements but if you need to apply it to a solid, it is enough just to overlap the shell on top of the solid with very low stiffness and merge the nodes.( Offset and then collapse or copy/hallow/merge). Springs are just to help me to check displacements.

The function is divided in two parts and you will find it very customizable.
First part controls the amplitude of the load. I’m using double step function but triangular should also work (not tested).
More elaborated shapes could be build adding more than one traction load.
The second part is responsible of carrying the load along the travel length.

Here it is : A*heaviside((B*t-D)-(x-C))*heaviside((x+C)-(B*t-D))

¿Surprisingly simple, isn’t it?

A Amplitude of the traction load.
B Parameter to control the speed.
C Parameter to control de width of the load. (Punctual=0 doesn’t work but can be very small value)
D Parameter to control the offset in time of a second Load train following the first one. Might be useful if you want more than one load (two cars or the two tires of a truck for example) or a more complex load shape.
t-The pseudo time set in the Time Period box controls the length of the travel.

Pay attention to the combination of units m/s , mm/min,….

I’m sure the users could also be able to adjust the function to set the desired direction (probably with an additional Heaviside) or starting time (probably with an additional Heaviside too). ¿Would be nice to see two loads crossing each other?

For an arbitrary direction check post “How to make line pressure linearly vary along length of line element”

The file is cool and only takes 2 minutes to run. Recommended. <1.000 nodes.

Victor

Thanks Disla. I thought I should post a screenshot because it looks so beautiful.



I added the triangular load function because it tends to produce a more mesh independent load whereas the step function used here can have bigger errors as it transitions across element boundaries. Not sure if it makes a difference in this case though.

kennethfugate

Victor, can you post the triangle load functions?

Sergio

That´s amaizing @disla ! I remember have seen a FEA model of a roller coaster with the buggy moving all around, does this kind of modelation in Mecway/CCX take in count inertial loads due to speed of movement?

MikeMcMullen

This could also be very helpful to me as well.

disla

Thank you guys,

I’m happy it’s being interesting and useful.

This is the triangular load: A*unittriangle(C,(B*t-0.)-x)

C Parameter to control the width in the step version of the load is now the first term into the unittriagle function.

Don’t know why, but it can’t converge so easy. I get a message like: “Pressure load requires too many sampling points. Using 1001 uniformly spaced time values for *AMPLITUDE.”
¿Maybe I’m short in memory . Just have 16 Gb?

Static analysis can’t consider inertial effects. To get them you just switch the analysis to dynamics 3D and check all the materials has density (Except Springs) . I tried and it works.
You need some damping on the springs to calm down the system a bit.

MikeMcMullen, I think you work with impacts on structures ¿isn’t it?. I’m almost sure this method could also simulate a blast and its pressure wave.
I would have to think some more but probably changing x by r will propagate in spherical direction in the space. I also think an exponential decay in the pressure it’s needed. That is an additional Ps(t)=Pso(1−t)e−k*t as Amplitude (A). ¿What do you think?

MikeMcMullen

Don't know. Haven't worked with blast. I believe a lot of the problem involves reflections as well as the inertial effects.
Calcullix might be able to be tricked into doing this since it has fluid and gas flow capacities, but that would be out of my league. Our bridges are not at much risk of that. Most interesting work lately is impact by trucks. A lot of other problems, moving truck loads in places not covered by codes, Prestress loads. Also impact by falling rocks.
I am a relative newby to the modern powerful FEM capabilities as most routine design work is done using simplified methods from the codes, but some things just are not covered well by the codes (sometimes the simplification is too simple, or does not fit an atypical case), and I seem to get many of these problems due to 50 + years of experience.
My first work with computers was repairing analog electronic (think vacuum tubes) and electromechanical in the USAF starting in 1965, and a bit later figuring out ways to modify them for added capabilities.

disla

Hi,

@MikeMcMullen . You are right. This would not capture reflections or shadowed areas unless the surface under traction is carefully assigned. Just direct blast impact and open structures where the pressure could freely develop.

The attached file is just to show that the same idea could be easily extended to a moving heat source. Useful for example for analysing of welding or in-line heating processes.

MikeMcMullen

That looks useful. While the fabricator normally figures it, the distortion for steel girder welding has to be figured into plate cutting for bridge girders.

Victor

@disla, the message "Pressure load requires too many sampling points. Using 1001 uniformly spaced time values for *AMPLITUDE." comes from Mecway converting the formula to a table of discrete (time, load) pairs for CCX. Mecway chooses time points for this table to keep the discretization error below some threshold but if the function is too complicated, the table could become huge so it's capped at 1001 time points and shows that message when it reaches that. I guess it's probably OK here, but if the formula had important details on the scale of time period / 1000, it could lose accuracy.

disla

Another cool application of moving loads is that they can reproduce increasing hydrostatic pressure on a filling process.
This is not proportional hydrostatic load P=p(z)*t , it is hydrostatic pressure P=p(x,y,z,t) generated by a fluid increasing level.
One should consider that Pressure and Traction as a function of position are not follower loads but for small deformations of the walls the error is small.

Pressure= (Rho*g*H /1000)* H *unittriangle(H *2,(z+ H)- H*t)

z (could be z, x or y) Pressure gradient direction.
Rho. Fluid Density [Kg/m3]
g Gravity [m/s2]
H Maximum filling level [mm]
T Pseudo-time Period (=1 sec)

New Mecway 2.15 allows to apply it directly to Solids.

mmartin

DISLA, brilliant.

Manuel

disla

Hi, @AndreaC91

I have reformulated the Heavyside to see if it is clearer. Now the time (t) and the time offset (t0) are grouped so they both have the same time units and velocity is clearly identified.

Amplitude*heaviside((v*(t-t0))-(x-width/2))*heaviside((x+width/2)-(v*(t-t0)))

Amplitude : Pressure or Traction on the surface.
v:Velocity of the Load front. [x/t] Units
to: Activation delay or second load delay. [sec].
t: Pseudo Time. It controls how much time (length) the front will travel.
Width: width of the double steep function [mm]




Example
-100*heaviside((1000*(t-0.0))-(x-75))*heaviside((x+75)-(1000*(t-0.0)))

Amplitude=-100[Pa]
v=1000mm/s
t0=0sec
t=1 sec
width=150mm

Note the front is referenced at the center so at time t=0 sec, ½ of width is already into the run. If you want to see how it enters and leaves the run completely , you need to delay the front width/2/v=0.075 sec backwards and increase the overall time t by 0.075*2
Result: -100*heaviside((1000*(t-0.075))-(x-75))*heaviside((x+75)-(1000*(t-0.075)))

disla

To get the dynamic response just move the analysis type to dynamic and be sure to set up densities for all materials. (Mine has some damping)

Andrea

Applying the moving load proposed by @disla ( Amplitude*heaviside((v*(t-t0))-(x-width/2))*heaviside((x+width/2)-(v*(t-t0))) ) I found good agreement with results obtained from structural software (only beam elements) with moving load.
Loads are applied to upper faces of solid elements (C3D8)
The problem is related to monorail beam supporting 2 bogies
HEB600 L12800 torsional restraints only at the ends- Bogie1 131.472 kN - Bogie 2 70.988 kN interaxis 750mm + Beam selfweight
Note: I didn't understand because at the first time step the first load is duplicated (see LIML file)
PS: could suggest how to find quikly the boogies position (forces) that causes the maximum beam deflection?

disla

Initial position: The boogie has velocity 1000mm/s and offset t0=.75 seconds. It is advanced 1000*0.75=750mm from the origin.
The center of the load is in between two elements and Mecway has split the load.
For the load to arrive on the center of the element, e.g. at a distance of 775mm it requires slightly more time.

t0=775mm/1000mm/s=.775s (actually .75s)

NOTE : with half width=25mm the load is fully contained in the element with width 50mm. If you make it wider you will see at some point how Mecway splits with more arrows at both sides

For the maximum deflection I would look for the maximum (export csv and Excel) of the Volume integral of the lower flange Strain Energy. According to that, it is at 5.9s. Positioning the cursor there I have located the -28.314mm.

Mishal

Not sure if this is possible on Calculix, but I have previously simulated a moving load using truss elements with prestrain applied to them. I had a node with the mass which was assigned a velocity. That node was attached to the boom using truss elements with prestrain assigned such that if the truss element was geometrically vertical it will have a small amount of compression which allows it to exist in the analysis. Thus the truss elements were essentially compression only with prestrain...

Andrea

Ok @disla....so also the second load must be shifted of 25/1000 s (25 mm half width and 1000 mm/s)
For deformations, avoiding C3D20 for too nodes model, is better C3D8I than C3D8. The last is too stiff.