Learning Forum

[Adisa]

Hello everyone,

I have tried to do creep analysis, but in ansys i cant include creep strain (see pic. below).

I tried to analysis simply beam, where i used Norton model of creep, but i have problem with this. I use a student Ansys.

Best regards.

Thanks!

[Adisa]

Peter,

Thanks so much for the answer.

I am confused, I use default steel with Bilinear Isotropic Hardening and Yield Strength 250 MPa.

The beam is load with 50 kN, and that do not have the plastic strain, because the yield stress is larger than stress on the beam (167 MPa).

The properties of material:

Which the mathematical model need to use that the creep strain can be used instead the plastic. Whether I'm wrong
defined the material? What should i do that the creep occurs and that it changes by mathematical models of the creep (time,strain,Norton..) rather than by Tangent Modulus of B.Isotropic Hardening.

 Thanks one more.

 

[peteroznewman]

I will post more later.

[peteroznewman]

In a Static Structural model, you have to use the Creep Controls under Analysis Settings to turn creep On.

This shows Creep is On in Step 2, which is because if you apply a force, you don't want it ramped on over 1000 seconds you want it on at a constant value, therefore, in Step 1 the Force is ramped on in 1 second, with Creep Off, then in Step 2 the force is constant.  After the solution, there is an Equivalent Creep Strain result.

I made a model of a 1 m long part, that has 100 MPa of stress, and has 1000 seconds of creep time with a Norton Material with these artificial constants:

The total deformation at 1 second before creep is 1 mm, after 1000 seconds it is 2 mm.

The creep strain calculated by ANSYS is 0.001

Norton equation is shown below and can do a hand calculation of the expected creep.

creep strain rate = 1e-8 * (100 MPa)  = 1e-6

creep strain hand calculation = 1e-6*1000 sec = 0.001

length increase due to creep = 0.001*1000 mm = 1 mm.

For those looking for real creep constants, pgl has this post.

ANSYS 17.2 archive is attached.

[Adisa]

Peter,

Thank you so much, the problem is solved.

I use ANSYS 18.1.

Best regards.

 

[quang79]

 Hi Adisa and Peteroznewman.

I am starter using ANSYS.

I want to make a simulation of creep damage of turbine blade. However, I do not know how to do.

I tried to read some tutorial but can not successfully simulate.

Please help me that make a tutorial of creep damage simulation.

Thanks and Best regards,

[peteroznewman]

Hi Quang,

I see you created a New Discussion, which is the right thing to do as this discussion is solved and it's not yours.

Regards,
Peter

 

[Arashord]

.

[Arashord]

.

 

[Arashord]

.