You are here
Moving Force
Tue, 2012-11-13 02:12 - wakeful
Hi friends
I want to define a moving force with a special velocity in Abaqus, like a train force on a bridge.
Is it available in Abaqus ? If yes how I could define it?
Thanks
Forums:
Check these two references
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.
Hi Akumar!I read first
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
Time varying displacement
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.
Sample Input File - 1st Example in Paper
*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.
thanks
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
You can not import directly
You can not import directly the input file in abaqus/cae. In order to do that, do the following:
*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
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.
Some question about input file
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
Hi, The surface for 3D
Hi,
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.
my goal
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.
The Difference
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.
models
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;}
I think I found the problem
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?
It's not how you define
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.
Your moving Force
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
Moving forceor moving mass
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
Re : 3D Applications
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.