ANSYS Thermal Analysis in a Stepped Bar-Det.of stresses, Nodal Deflections etc: The main aim of ANSYS Thermal Analysis in a Stepped Bar is to determine the Nodal Deflections, Reaction forces, Stresses induced in the stepped bar etc.under the application of uniaxial load. Here, I am using Nodes and Elements to construct a stepped bar of the given dimensions in the problem. In order to analyze the stepped bar under the Application of uniaxial load in ANSYS Software, we require 4 steps.
An axial load of P=40KN is applied at 30˚C to a stepped bar as shown in the figure.Determine the Nodal deflections and stresses induced in the stepped bar when the temperature is raised to 80˚C.Given,
A1= 2000mm2 ,A2=1200 mm2 ;
E1=2*105 ; E2=1*105 ;
α1=12*10-6 , α2=18*10-6 ;
The Procedure of ANSYS Thermal Analysis in a Stepped Bar are as follows.
Structural & Thermal—> h-method—> OK.
Add—> Add—> Link-3dfinite stn 180—> OK.
For ANSYS 14.5 Users:
Add/Edit/Delete—> Add—> Link180
- Real Const.Set No. 1 & Area A1=2000mm2 . Apply
- Real Const.Set No. 2 & Area A1=1200mm2
For ANSYS 18.0 Users:
Go to Sections—> Link—> Add—>
Section ID =1 & Area A1=2000mm2
Section ID =2 & Area A2=1200mm2 —> OK.
Material Models—> Structural—> Linear—> Elastic—> Isotropic—> Provide the Young’s Modulus (E= 2X105) and Poisson’s Ratio (µ) =0.3—> OK.
For Coeff.of Linear Expansion(α1),Go to
Thermal Expansion—> Secant Coefficient—> Isotropic—> ALPX(α1)=12e-6—> OK.
Material Models—> Structural—> Linear—> Elastic—> Isotropic —> Provide the Young’s Modulus (E= 1X105) and Poisson’s Ratio (µ) =0.3àOK.
For Coeff.of Linear Expansion(α2),Go to
Thermal Expansion—> Secant Coefficient—> Isotropic—> ALPX(α2)=18e-6—> OK.
Create—> Nodes—> In Active CS—> Provide the Nodes 1,2&3 with the lengths as shown above in the figure. and give their respective values in X,Y&Z Direction as shown below.
Now,you need to construct these nodes by means of elements.For that,goto
For 1st stepped bar:
- Element Attributes—> [Link-180;Material-1;Real Const.Set No.1]
- Auto numbered—> Through Nodes—> Now,pick the 1st & 2nd Nodes.
For 2nd stepped bar:
- Element Attributes—> [Link-180;Material-2;Real Const.Set No.2]
- Auto numbered—> Through Nodes—> Now,pick the 2nd &3rd Nodes
To get the Solid View of the Stepped bar instead of a line,go to
- Plotctrls—> Style—> Size and Shape—> Display of Element—> ON—> OK.
- Plot—> Elements—> OK.
5.Constrain the body:
- Loads—> Analysis Type—> New Analysis—> Static —> Ok.
- Define Loads—> apply—> Structural—> Displacement—> On Nodes—> Pick the 1st & 3rd Node—> Apply—> Click on All DOF(Constrained in all Directions)
Define Loads–>Apply–>Structural–>Force/Moment–>On Nodes–>Select the 2nd Node and apply the force in horizontal(Negative X-Direction) direction as shown below.
Fx = -40000N
- Define Loads–>Settings—> Reference Temperature = 30˚C (Initial Temp)
- Define Loads–>Settings—> Uniform Temperature = 80˚C (Raised Temp)
- Analysis Type—> New Analysis—> Static—> OK.
- Solve—> Current LS—> OK.
IV.GENERAL POST PROCESSOR
- Plot Results—> Deformed Shape—> Deformed Shape with Un-deformed Model—> OK.
- Plot Results—> Contour Plot—> Nodal Solution—> DOF Solution—> Now take all the displacement in X,Y&Z component of Displacement along with Displacement Vector sum.
Plot Results—> Contour Plot—> Nodal Solution—> Stress—> Now take all the stresses induced in X,Y&Z component of stress along with Vonmises stress.
Take the maximum stress induced in the body i.e. Vonmises stress which should be less than the Yield point of the material.Then only,the component is safe under the application of loads else the design is of a failure case.
General Post Processor–>List Results–>Reaction solutions–>All structural Forces–>OK.Now you can get the Reaction forces at the supports.
- How to perform Static Analysis of Structural Truss System in ANSYS APDL?
- Static Analysis of Cantilever Beam under Point Load- Vonmises Stress,DOF,Reaction forces,Nodal Solutions etc.
- How to do the cantilever beam using nodes in ANSYS APDL?
- How to import a model from CATIA(.Cat Part) to ANSYS 15.0?
- How to import a model from CATIA to ANSYS via Creo?
This is the complete explanation about ANSYS Thermal Analysis in a Stepped Bar under uniaxial Load in a detailed way.If you have any doubts, feel free to ask from the comments section. Please Share and Like this blog with the whole world so that it can reach to many.