Hi,

If you want to define a Force versus Time you have to use an Array of Discrete Values obtained from the defined Force Curve.

For 2D and 3D Applications Ansys allows to use 2D or 3D Arrays with :

*DIM, Force, Array, Imax, Jmax, Kmax : to define an Array Parameter and its Dimensions.

Force can be Defined with *SET Command which Assigns user Defined Values.

Imax=n and Jmax=Kmax=1 : Corresponds to Force(t) Time History Forcing function.

The Third Dimension (Jmax=m and Kmax=p) can be useful to Model Fluid Flows with Specifying the Function as a Table Array

Parameter with Force and Time Values in a Non Linear Solution.

Best Regards

M.L.

Hello
friends

I
read about 3D beam to define it for a surface-to-surface contact, as you said 3D
beam surfaces can only be used as slave surface in contact definition, so I decide
do another way which it does not need define an interaction, I want to define
the moving train as a moving force or mass, now how I could do it? I don’t know
how I could make a mass or concentrate force move.

Sincerely

Hi

In some softwares (like Ansys) it is possible to define a Dynamic Force by an Array of Varying Values

from 1D to 3D Applications. Your case may correspond to Force versus Time.

Good luck

Mohammed lamine

It's not how you define springs (wether in property module or in interaction). The reason you see my springs in property module because you're importing input file. Since the model was fairly easy to generate, therefore, I didn't require CAE to model the problem (I wrote it). Few things are quite easy if you work with input file. Anyway, since you're working with cae, you will need to make reference points. First make them and keep them away from your model so that you can easily select these points and can create node sets. Once you've defined node sets of all the required points in your model, position these reference points to the desired location, and then everything will be easy. It is just my advice to make sets for everything you may need in the modeling, as many things become very easy

------

The world started with 0, is progressing with 0, but doesn't want 0.

I
think I found the problem

You defined
the spring/dashpots for part in property module, but I defined it in assembly
module because I do not know how you defined it in property module, I need 2
points to make spring/dashpots that I make them by reference point, also I assigned
equation constraint to them. How I could define spring/dashpots without
reference points?

I
checked your model, your points were node [52] and node [53], how you made and
selected them?

Normal
0

false
false
false

EN-US
X-NONE
AR-SA

MicrosoftInternetExplorer4

Hello
my friend

Now I understand
that I want to model just a moving force, as you said moving oscillator is
general. I tried model moving force but there is some error and problem in my
these models

I make 3
models, a model with moving force; second one with moving oscillator and third
one with a constraint force in the middle.

Again Zero
pivot warning was shown for two models, while all of my BC or joints were
perfect defined

After run of
each models, errors and warnings come, could you help me to solve these
problems?

I attached CAE
file too.

http://www.4shared.com/rar/LL5Ijuos/my_models1.html

Moving-force
model:

Errors:
Too many attempts made for this increment

Warnings:

-MPCS (EXTERNAL or INTERNAL, including those
generated from rigid body definitions), KINEMATIC COUPLINGS, AND/OR EQUATIONS
WILL ACTIVATE ADDITIONAL DEGREES OF FREEDOM

-There
are 2 unconnected regions in the model.

About
20 number of this warning :

- Solver
problem. Zero pivot when processing D.O.F. 2 of 1 nodes. The nodes have been
identified in node set WarnNodeSolvProbZeroPiv_2_1_1_1_1.

Moving
oscillator model:

Errors:
Too many attempts made for this increment

Warnings:
There are 2 unconnected regions in the model.

Cforce
model:

Errors: ----

Warnings:
----

Thanks a lot

/* Style Definitions */
table.MsoNormalTable
{mso-style-name:"Table Normal";
mso-tstyle-rowband-size:0;
mso-tstyle-colband-size:0;
mso-style-noshow:yes;
mso-style-priority:99;
mso-style-qformat:yes;
mso-style-parent:"";
mso-padding-alt:0in 5.4pt 0in 5.4pt;
mso-para-margin-top:0in;
mso-para-margin-right:0in;
mso-para-margin-bottom:10.0pt;
mso-para-margin-left:0in;
line-height:115%;
mso-pagination:widow-orphan;
font-size:11.0pt;
font-family:"Calibri","sans-serif";
mso-ascii-font-family:Calibri;
mso-ascii-theme-font:minor-latin;
mso-fareast-font-family:"Times New Roman";
mso-fareast-theme-font:minor-fareast;
mso-hansi-font-family:Calibri;
mso-hansi-theme-font:minor-latin;
mso-bidi-font-family:Arial;
mso-bidi-theme-font:minor-bidi;}

The difference among all these three is quite simple. Moving oscillator is the most general approach, and moving mass and moving force are two extremes. In moving force we account for only the load being transferred to the bridge due to vehicle's weight and the inertia of the vehicle is ignored (i.e. mass effect of vehicle is ignored). Moving mass is another extreme where the vehicle is assumed to be rigid, and the weight and well as inertia forces are transferred to the bridge. So in other words, moving mass and moving force are specialized form of moving oscillator case. Which extreme you want to use is dependent on the mass and stiffness of the subsystem (i.e. vehicle) w.r.t. the primary system (bridge).

------

The world started with 0, is progressing with 0, but doesn't want 0.

I want to model train moving on a truss bridge, as you said there are 3 trends to define vehicle
loads: 1-moving force 2-moving mass 3-moving oscillator. I do not know what is different among them
exactly but the simplest way is suitable for me.

Hi,

1. The surface for 3D beam can not be defined as the unique surface normal can not be determined from nodal connectivity. Therefore, 3D beam surfaces can only be used as slave surface in contact definition (check abaqus analysis manual -> spatial modeling -> surfaces -> element based surface definition). Therefore, you'll have to find another way around. Does your analyisis involve moving force only (inertia of subsystem to be neglected) or moving mass or moving oscillator?
2. Is is probably the deformation scale factor in the visualization. Make it one, and you'll see the oscillator passing the whole bridge.
3. The speed of the oscillator is 100 km/hr (27.778 m/s) and the length of beam is 25 m. Therefore, the time it takes for the oscillator to pass over the beam completely is 0.9s (25/27.77). Since, I am interested only in the response during the oscillator passes over the beam, therefore, the time period of dynamic step is 0.9s.

If you want to neglect the moving oscillator's inertia (i.e. it is moving point load), then there is an alternative that doesn't require definition of contact interaction. But this is specialized technique and valid only for moving force analysis.

------

The world started with 0, is progressing with 0, but doesn't want 0.

Hi dear sir A.kumar

I checked the input; here is some question about it

1. In the Interaction module you defined a surface-to-surface
contact (standard) which master surface is BRIDGE-SURF and slave surface is
VEHICLE-WHEEL. You defined BRIDGE-SURF as a surface. It is available to define
a beam as a surface just for 2 dimensional beams, but my model has 3
dimensional beams, so how I could define this contact?

2. Increments: in the visualization module there are 900 frames to
show moving oscillator, the oscillator passes half of bridge length, how I
could make it to pass whole of bridge length? And how I could change the number
of frames?

3. In Dynamic, Implicit step, why you define time period= 0.9?

Sincerely

You can not import directly the input file in abaqus/cae. In order to do that, do the following:

• Change the beam general section part in the input file to

*Beam General Section, Section=General, Elset=Bridge-Elements, Density=23.03
100.0, 2.94, 0.0, 2.94, 0.0
0.0, 0.0, -1.0
2.87E9, 1.1958E9

• Run the analysis, or atleast run datacheck.
• In abaqus cae, goto file -> import -> Model ... -> (select .inp, .pes as file type) -> import .pes file.

The input file is parametrized, and abaqus/cae doesn't support parametrized input file. Therefore, you need to import .pes file which is the copy of .inp file but with all the parameters substituted with their corresponding values. THen you should be able to see the whole model in abaqus cae, and you can go through different modules.

Let me know if you need further help.

------

The world started with 0, is progressing with 0, but doesn't want 0.

Hello Akumar!

Thanks a lot for your guide and sample input file, I make an .inp file with your text and run its job, I want to check its modeling data in different modules, but I just could access visualization step, how I could check other modules?

This is my email address : elhamaskari@hotmail.com

*Heading
1st Example Problem, Yang & Yau (1997). Units: N-m-s
*Parameter
Nel = 50
Nx, S1, S2 = Nel+1, Nel+2, Nel+3
********************** Refined Mesh ************************
*Node, Nset=Bridge-L
1, 0.0, 0.0
*Node, Nset=Bridge-R
<Nx>, 25.0, 0.0
*Node, Nset=Vehicle-B
<S1>, 0.0, 0.0
*Node, Nset=Vehicle-T
<S2>, 0.0, 1.0
*Ngen, Nset=Bridge-Nodes
1, <Nx>
*Element, Type=B21
1, 1, 2
*Elgen, Elset=Bridge-Elements
1, <Nel>
*Beam General Section, Section=General, Elset=Bridge-Elements, Density=23.03
100.0, 2.94, 0.0, 2.94
0.0, 0.0, -1.0
2.87E9, 1.1958E9
*Element, Type=SpringA, Elset=Vehicle-K
<S1>, <S1>, <S2>
*Element, Type=Mass, Elset=Vehicle-M
<S2>, <S2>
*Spring, Elset=Vehicle-K

1.595E6
*Mass, Elset=Vehicle-M
5750.0
*Surface, Name=Bridge-Surf, Type=Element
Bridge-Elements, SPOS
*Surface, Name=Vehicle-Wheel, Type=Node
Vehicle-B
*Surface Interaction, Name=Int-1
*Surface Behavior, Pressure-Overclosure=Hard
*Contact Pair, Interaction=Int-1
Vehicle-Wheel, Bridge-Surf
*Equation
2
Vehicle-B, 1, 1.0, Vehicle-T, 1, -1.0
*Amplitude, Name=Move, Time=Step Time
0.0, 0.0, 0.9, 25.0
*Boundary
Bridge-L, 1, 2
Bridge-R, 2, 2
Vehicle-T, 1, 6
********************** Self Loading Step ************************
*Step
*Static
0.1, 1.0
*Cload
Vehicle-B, 2, -56407.5
*Output, Field, Frequency=1
*Node Output
U, RF, CF
*Output, History, Variables=Preselect
*End Step
********************** Dynamic Step ************************
*Step, Inc=100000
*Dynamic, Alpha=-0.05, Application=Transient Fidelity, Haftol=5500.0
0.001, 0.9, 1.0E-7, 0.001
*Boundary, OP=New
Bridge-L, 1, 2, 0.0
Bridge-R, 2, 2, 0.0
*Boundary, OP=New, Amplitude=Move
Vehicle-T, 1, 1, 1.0
*Output, Field, Frequency=1
*Node Output
U, RF, CF, V, A
*Output, History, Variables=Preselect
*End Step

------

The world started with 0, is progressing with 0, but doesn't want 0.

Time varying displacement can be defined only in a step. So once you've defined a dynamic step, go to Load Module in Abaqus. Then create boundary -> from drop down menu, select the step you would like to define time varying displacement -> Enter Components -> at the bottom, amplitude (default ramp for dynamic) -> create amplitude...select the type that suits your purpose.

Alternatively, you can define amplitude variation through Load Module -> Tools Menu (on Top Menu) -> Amplitude -> Amplitude Manager -> Create Amplitude

Details about different amplitude types can be found in Abaqus Analysis Manual (Prescribed Conditions -> Overview

Note: If you would send me an email (through imechanica) or post me your email id, I can send you both papers. However, first one (Int J. Comput. Methods Eng. Sci. Mech.) is the more detailed one, so it has everything you need. Just don't use the simplified equivalent system matrices, since they misprinted the equations.

Let me know if you need any help. I will send you a sample input file.

------

The world started with 0, is progressing with 0, but doesn't want 0.

Hi Akumar!I read first article but I couldn’t access the second one. In the first article you said there are 3 trends to define vehicle loads: 1-moving force 2-moving mass 3-moving oscillator And you said we should define a connector between mass and the element that mass moves on it. Then define amplitude to show the mass position versus time, I checked the menu to do it, but I couldn’t define time-displacement amplitude.Could you help me?

Sincerely

Check out these two papers. These have exactly what you want.

Saleeb, A.F., Kumar, A., 2011, ‘Automated Finite Element Analysis of Complex Dynamics of Primary System Traversed by Oscillatory Subsystem’, Int. J. Comput. Methods Eng. Sci. Mech., 12(4), 184-202.

Kumar, A., Saleeb, A.F., 2009, ‘Computer Modeling for the Complex Response Analysis of Nonstandard Structural Dynamics Problems’, J. Aerosp. Eng., Vol. 22(3), pp 324-330.

------

The world started with 0, is progressing with 0, but doesn't want 0.