Learning Forum

[Ali617]

Hello

 

I want to carry out a thermal-mechanical-analysis. Firstly I want to do thermal stress and then i want to import that load to Mechanical-Analysis-Component and want to find out the stress, strain and fatigue life of the probe. In thermal analysis I want to warm up my probe 5 minutes long and then cool down it again 5 minutes long. That is my 1 cycle(10 minutes). 

My questions are: 1-How can i warm up and cool down my probe succesively?

                              2- How can i carry out this cycle more than once?(For example 100times)

 

Thanks in advance!

[jj77]

The video below shows how to do a coupled transient thermal stress analysis.

https://www.youtube.com/watch?v=Ktv7bYewakM

 

 

 

This video below shows how to define a heat cycle for a transient thermal analysis, that is what you need to do define your cycles (heating and cooling) as in the video.

https://www.youtube.com/watch?v=HtbK-o6VM1Y

 

A good paper on this topic also:

 

https://www.ansys.com/-/media/ansys/corporate/resourcelibrary/whitepaper/thermo-mechanical-fatigue-wp.pdf

[peteroznewman]

I will create an example that has 10 cycles.

Use a Transient Thermal analysis block. Under Analysis Settings you can specify Number of Steps = 10. Step 1 has an End Time of 5*60 seconds. Step 2 has an End Time of 10*60, etc. Insert a thermal load, such as Temperature, and in Step 1 type the high temperature, then in Step 2, type the low temperature, etc.

Solve this model.

You can drag and drop a Static Structural analysis block onto the Solution cell of the Transient Thermal.

Make the Static Structural a 10 step analysis with the same end times as the Transient (for simplicity). There will be an Imported Load. Assign the 300 second Source Time of the Imported Load to the 300 second mark of this Analysis etc.

 Here is the time history of the Maximum Equivalent Stress.

I have to do more research on the fatigue calculation.

You can Insert a Fatigue Tool, and set the type to History Data, but then it wants a text file.

Maybe someone knows the next step and can reply.

Regards, Peter

[Hakim Dina Anjum]

Hey Peter!

How do I set the end time of the steps in analysis settings, could you help me out? 

[jj77]

In your example Peter the thermal stress varies almost like a harmonic sinus./cosinus., so one would take the largest peak, say if it is fully reversed (load) or define a fatigue ratio most likely, then use a mean theory (if not fully reversed) and out will come how many of these cycles one can have (stress life). If it is low cycle fatigue, then things are a bit more complex.

[Ali617]

Hello

Firstly thank you for your answers.

Peteroznewman .I did an analysis that has also 10 cycles but i found a wrong solution. As equivalent stress i found this

But actually it is supposed to be like that one

 

It is not about the stress values but the stress points or possible damage points. 

I have uploaded my analysis under my first post. Could you please say my mistake in this analysis?

[peteroznewman]

Hello,

Thank you for inserting images in your post. Without opening your model, I can say that the mesh is too coarse to get a reliable answer. Make elements at least 2 times smaller as a first result, say start at 2 mm. Under the Mesh Details, there is an Element Size setting where you can do that. The same effect will be made by adding a Sizing Mesh Control and picking the body.

I see you are on a Student license, so you have to stay below the 32,000 node or element limit. If you add a mesh control Method, pick the body and set it to Hex Dominant, 

Then you can run the analysis again with an Element Size of 1 mm to evaluate if the result changes much.

I don't understand how a pressure load would be applied to some faces and not others. Please describe in more detail how this part is physically loaded.

Is the part physically welded to an immovable object on the back?  That is what this Fixed Support is doing.

Please describe how the part is really constrained with other parts in the real world.

Regards, Peter

[Ali617]

Hello

Firstly thank you for your mesh-tips.

 

This probe is not welded but stays between two flanges.

And there is a gas-flow(1323K) which flows inside of flanges. The gas flows from red flange to the yellow one thats why it touchs just front areas of the probes.You can imagine it like a teststand of a turbine of turbocharger.

 

[peteroznewman]

Is the gas flow going past the object in the -Z direction?

If so instead of the pressure that you defined that is Normal to each surface:

Change the pressure to be in a Component direction

I see you have a Fluent model started. Obviously, once you get gas pressure from Fluent, you can apply those as a load instead of this pressure, which is just a place-holder for more accurate pressures from Fluent.

A slight improvement over a Fixed Support would be a Compression Only support.

If you do those two changes, you will get a peak stress in the sharp interior corner. Add a blend to the geometry to get rid of that sharp interior corner.

Regards, Peter

[VJ0085]

Hello, This is really an interesting thread and I am also doing something similar. I have questions for you:

1. In the above model, if the stress values exceed yield stress (plastic deformation) the plasticity model will need to be included (Bilinear/multilinear) in the material data for better visualization of the stresses, Am I right?

2. The material constants in the example are at 22 degrees but the temperature also raises to 600 degrees and back to RT again, now assume, if the material was PC, then in this case, how should I include the effect of temperature on Modulus and other parameters in the simulation? I mean to include this effect: https://www.ptonline.com/articles/the-effects-of-temperature

3. In my model I am supposed to simulate below condition "Put test sample in the chamber, -20deg C to +65degC each duration 15minutes, transient times in 1min, for 1cycle, total test 100 cycles". This is for the snap joint who failed after temperature shock test and cracks were found in the middle section and at the snap root after the test. I have been given another model to carry out the above simulation (temperature shock test) in Ansys. If I have to validate the design, should I perform the thermal fatigue analysis and follow the same steps mentioned in this thread? If yes, how should I include above conditions altogether in the setup? And if it exceeds the ultimate stress, can I safely say it will break with cracks developing at high-stress region point?

Sorry for the long question, but I am numb in fatigue analysis with some basic knowledge in fracture mechanics. 

[peteroznewman]

Hello,

1. Yes.

2. In Engineering Data, you can define Young's Modulus in a table with Temperature.

3. Yes, try this approach. If you include plasticity, especially with perfectly plastic (zero Tangent Modulus), you will never get to a point when stress exceeds the Ultimate Tensile Strength. This is when you compare Equivalent Total Strain with Elongation at Break to decide if the part has failed.

If you have more questions, it's better for you if you start a New Discussion, and put a link back to this discussion for reference. That way, you are notified when replies are posted.  Posting in this thread means the original poster is getting notified of new replies.

[VJ0085]

Hey Peter,

Thanks for the quick reply and explanation, I didn't know about notification thing, perhaps that's the reason I was wondering why I didn't receive notification for my post.

I will start a new thread soon, Thanks.