Discussion Groups

Simulation Mechanical and Multiphysics

Reply
Contributor
Leonel16
Posts: 14
Registered: ‎06-26-2014
Accepted Solution

Setting up Thermal stress Analysis

249 Views, 6 Replies
06-27-2014 12:30 AM

Deal All,

I am new to the software and I urgently need your help to clarify below concern:

 

Analysis background:

                I need to know the stress build-up of my model caused by the change in temperature from 220C to 25C (cooldown condition) wherein my stress free condition will be at 220C. Since I have a stress producing change in temperature of (220-25 = 195C), what is the best way to represent this in Sim Mechanical.

 

Need to understand details of these two different approach on this analysis:

 

1.0   In the case wherein I will just set my load in the Analysis parameters as:

 

1.1 Source of temperature: Loads from FEA editor

1.2 Default Temperature: ______???????? – Is this value corresponds to the change in temperature (on my case 195C) or is this the reference temperature which my model will cools down to (on my case 25C) or this 220C?

1.3 Stress Free reference temperature: 220C – this can be set at element definition, set stress free temperature.

1.4 Temperature load – is it appropriate to set all parts/model to certain temperature (on my case 220C)?...or can this be set at 25C? what’s the essence of this temperature loading for me to relate into my objective of having a cool down condition from 220C to 25C.

 

                I understand that the software solves first for the displacement (then this change in temperature will be a factor for that during calculation), then once displacement is achieved thus stress and strain can be obtained. Now, how to represent this change in temperature on this set-up is a big puzzle to me which I need your help to clarify.

 

2.0   In the case wherein I will set my load in the Analysis parameter as: (load thermal profile from thermal analysis)

2.1   Source of temperature: Another design Scenario / Another simulation Mechanical file

2.2 Default Temperature: ______???????? – Is this value corresponds to the change in temperature (on my case 195C) or is this the reference temperature which my model will cools down to (on my case 25C) or this 220C?

2.3 Stress Free reference temperature: 220C – this can be set at element definition, set stress free temperature.

2.4 Temperature load – is it appropriate to set all parts/model to certain temperature (on my case 220C)?...or can this be set at 25C? whats the essence of this temperature loading for me to relate into my objective of having a cool down condition from 220C to 25C.

2.5 At what load case on thermal analysis is the appropriate step to be loaded here, in WHICH STEP TO USE OPTION.

 

DURING THERMAL ANALYSIS SIDE for item 2:

                2.6 What is the best approach to emulate the cooldown condition of temperature( from 220C to 25C) wherein I can capture the gradient and which in turn as load to look for the mechanical stress induced by this cooldown condition.

                2.7 In general given the scenario and objective of the analysis, based from your expertise and experience, what is the best way to emulate and approach of this study>

 

Sincerely,

Leonel16

Please use plain text.
Product Support
andrew.sartorelli
Posts: 54
Registered: ‎10-08-2013

Re: Setting up Thermal stress Analysis

06-27-2014 07:38 AM in reply to: Leonel16

Hello Lionel, welcome to the Simulation Mechanical community!

 

1.2 The default temperature is applied to all nodes with out a temperature load/boundary condition applied. If you are just doing a static stress analysis you would set it to your final temperature (25C), however if you are doing MES (time depedent analysis) you woudl set it to your starting temperature (195C)

 

1.4 If you are doing static stress and have set a default nodal temperature then you won't need to apply a temperature load. However, if you are performing an time dependent analysis then you would need to couple a transient thermal analysis with an MES analysis. You would add temperature loads/boundary conditions in the transient thermal analysis such that the part starts at 220C and ends at 25C. This can be done by creating a load curve for the boundary condition. You would then use the thermal loads from another design scenario in your MES analysis to apply the calculate temperatures to your part(s). This second method is my typical approach when doing a thermal stress analysis as it lets me verify that the temperatures are being applied in the exact manner that I want.

 

2.5 Are you refering to time-steps here?

 

2.6 If you are looking to see the time-varying stress then you would need to perform a coupled MES + transient thermal analysis.

 

2.7 As I mentioned above, I prefer the MES+transient thermal route. I'm sure some of the other community members will be able to share some of their experiences.

 

I also noticed that your company does have an active support subscription, so if you run into any problem please don't hesitate to log a technical support case through the subscription center.
______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!



Andrew Sartorelli
Please use plain text.
Contributor
Leonel16
Posts: 14
Registered: ‎06-26-2014

Re: Setting up Thermal stress Analysis

06-27-2014 08:40 AM in reply to: andrew.sartorelli

Dear Andrew,

 

first of all thanks for taking time looking into my post.

 

1.2. Thanks, its clearer now, this is my final temp when am doing static stress.

         Clarrification: Why 195C when am doing the MES?. should it be 220C since it is my starting temp?

 

1.4 OK, for the static stress I dont need to apply load temp since I will set a default nodal temp(25C) and have set my stress free temp(220C) at element defination . By doing this approach, is my goal of emulating the cooldown condition (from 220C to 25C) will covered by the software? I mean does the software knows already that there is indeed a delta temp of 195C, and its a cooldown condition?

 

I understand that performing thermal analysis first and have the temperature map as load for stress is the convenient approach, however, on my case, it is assumed that my model(all parts) is heated initially at 220C (which is assumed to be stress free) and then it is taken off from a chamber and let it cools down to 25C(again all accross parts). The time duration at which the model cools down from 220C to 25C, is unknown thus it is might be unrealistic to assume. Given this set-up, doing steady state thermal may not be again a good idea since it will just give me either 220C and 25C temp profile.

 

1.4.a - Being said then, what would be the best approach to emulate such condition rather than just applying stress free temp and default temp and let the software solve for stress given the delta temp?

1.4.b - In the absence of time duration of cooling down (from 220C to 25C), how can i run this in thermal analysis forst and make it coupled to static stress? Any idea please?.

1.4.b - If in case the time step is avaialble(time duration of cooling down from 220C to 25C), what is your recommended approach this on transient themal?. I have tried setting up this using a controlled temp as load and of course time varrying via load curve being 220C as my start and ends at 25C, BUT using controlled temp as load seems doesn't work fine, it only yield me either the all parts being at uniform temp gradient of 220C or the other way around (25C).

 

2.5 Yes, i am refering to time step. In an event that you have time step from your thermal analysis, which step then will you use as your load?. is it the step where the temp is athe highest?. is it the final/last step? how would I know that my objective of  understanding the stress caused by cooling down from 220C to 25C isbeing covered if I will just select a step out from that duration, hope you got my point.

 

2.7 I hope so that some of the members will share their experiences and expertise as well to beginners like me.

 

lastly, Yes, we are on subscription, and I am asking this in parallel as well, I opted to join and post it here so that some of the members will either benifit in the future should they have similar question,  if not contribute their experiences as well.

 

Hope to hear more clarification from you and from anybody. Thanks.

 

 

 

Please use plain text.
*Expert Elite*
AstroJohnPE
Posts: 529
Registered: ‎08-30-2012

Re: Setting up Thermal stress Analysis

06-27-2014 10:10 AM in reply to: Leonel16

Hi Leonel16,

 

It sounds as if you should run a transient heat transfer analysis to simulate the temperatures while cooling down. Guess how long it takes to cool down and use that time in the transient heat transfer analysis. The results will show you if your guess is too short, needs to be longer, or is just right.

 

After you have the results of the thermal analysis, you can copy the design scenario and change the analysis type to a stress analysis.

 

The advantage of a linear static stress analysis is the simplicity of the analysis: you will get results. The disadvantage of a linear stress analysis is that it will only use the temperatures from one time (time step, load case, whatever terminology the software uses) from the heat transfer analysis. Therefore, you either need to have a good idea which time step will cause the largest stresses, or you need to run multiple linear analyses and use a different time step from the heat transfer analysis for each one.

 

The advantage of a nonlinear stress analysis is that it will calculate the stress during the entire cool down time. The disadvantage of a nonlinear stress analysis is getting the model to converge or possibly long runtimes. I would guess that your assembly required minutes or hours to cool down.

  • This is essentially a static condition at each time step, so a nonlinear static stress analysis would be more appropriate than a nonlinear MES stress analysis (which includes dynamic effects).
  • Doing a static analysis requires the assembly to be statically stable, so be sure to constrain the model to make it stable, but you do not want to fix any directions that would prevent any expansion that is free in the real world.
  • Since the transient heat transfer analysis does not include any geometry changes due to expansion, the nonlinear stress analysis does not need to include large displacement effects. The nonlinear stress analysis can use small displacement theory which will make the convergence easier.

 

The general steps for a linear static stress analysis are as follows:

  1. Set the stress free reference temperature (220 in your case) in the Element Definition.
  2. Optionally, change the material model (also in the Element Definition) from the default Isotropic to a temperature dependent isotropic if the material properties change significantly over your temperature range.
  3. Edit the material properties. Make sure the coefficient of thermal expansion is entered.
  4. In the "Analysis Parameters" on the "Thermal" tab, set the "Source of temperature" to "Another Design Scenario in loaded file".
  5. The "Default Temperature" is not used UNLESS you have parts or nodes in the stress analysis that ARE NOT in the transient heat transfer analysis. The default temperature would be applied to such parts or nodes.
  6. Decide which time step (load case) to read from the transient heat transfer analysis with the "Which step to use" drop down. 
  7. On the "Multipliers" tab, set the "Thermal" multiplier to 1 for any load case in which you want to include the thermal expansion.

 

The general steps for a nonlinear static stress analysis are as follows:

  1. Change the material model in the Element Definition from the default Isotropic to one of the material models that includes thermal effects: thermoelastic or thermoplastic are the two main choices unless you need to get into viscoelastic or creep conditions. (These are the Sim Mech 2014 names. I have read that they were renamed in 2015.) All of these material are temperature-dependent.
  2. Set the "Analysis Type" (also in the Element Definition") to "Small Displacement".
  3. Set the stress free reference temperature (220 in your case) in the Element Definition.
  4. Edit the material properties. Make sure the coefficient of thermal expansion is entered. If my memory is correct, the material libraries do not have any temperature-dependent material properties, so you will need to define a customer-defined material and enter all of the material properties.
  5. In the "Analysis Parameters" on the "Thermal" tab, set the "Source of temperature" to "Another Design Scenario in loaded file".
  6. When reading the results from a transient heat transfer analysis, the "Nodal tempreature load curve index" is not used. It makes no sense to me to have results from a transient heat transfer analysis and then scale them by some amount. But to be safe, I would assign the temperatures to a unigue load curve number and set the load curve to a constant multiplier of 1.
  7. The "Default Temperature" is not used UNLESS you have parts or nodes in the stress analysis that ARE NOT in the transient heat transfer analysis. The default temperature would be applied to such parts or nodes. (I did not create a full model, but it appears that the Default Temperature may be disabled.)
  8. The "Which step to use" drop-down should be disabled when reading temperatures from a transient heat transfer analysis. It will read all of the time steps from the transient heat transfer analysis and interpolate the temperatures if the time step in the stress analysis does not match a time step in the heat transfer analysis. (Since I did not build a complete model, I could not confirm this.)

 

 

Naturally, you can include any mechanical loads such as forces, pressures, etc, and you need to constrain the model. There may be other input that you need to setup to complete the stress analysis, too.

 

Have fun!

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16.9 years experience with Simulation Mechanical
Please use plain text.
Contributor
Leonel16
Posts: 14
Registered: ‎06-26-2014

Re: Setting up Thermal stress Analysis

06-30-2014 01:07 AM in reply to: AstroJohnPE

Dear Jhon, Everyone,

 

Thank you very much for this very clear explanation.

Few clarification and im good to go, I guess I’m almost there getting this things done.

 

I have tried to run the using linear static stress analysis.

 

 During thermal transient stress analysis, I used control temperature as my load using load curve to satisfy the cool down condition(220C to 25C), I let it run for 40 sec overall, I let the model settle for 220C (0 – 10 sec) then ramp down to 25C (11- 30 sec) and then let it settle to 25C (31 – 40C). I set the time step at 5 per 10sec.(@10sec=5steps; 20=5, 30= 5; 40=5). I did get a temp profile at each step, but looking at each time step, there’s only ~1.5degC difference between min and max, this leads me to the following question:

 

 

  • Since the temperature profile across the model is almost at steady state(just ~1sec difference), selecting a step as a load to STRESS Analysis will just give almost a uniform temperature across the model(all parts) as if I just set the model (all parts) a default temperature. How does the software then knows or consider my cooling down condition on this case. I understand that I set a stress free temperature of 220C, but choosing say for example step 10(20sec) at WHICH STEP TO USE) which has a temperature of 123.7C max & 122.5 C min, this will just give me a stress delta temp of  ~96 C., way low to 195C delta temp from my original condition.
  • I run my model on static linear stress and stress result increases as time step increases ( Stress at 5step <10step<15step<20<step). Does this mean, the stress build up at 10 step is considered when solving the stress at step 15 and so on?
  • Because my model is composed of different layers of material ( from bottom (refer to attached photo)  -> copper trace , alumina, copper trace, solder, Silicon, solder, Copper), since I am using solder to form a connection between 1.0 copper trace and silicon 2.0 silicon and top copper, the 220C stress free assumption is came from the notion that it is a solder liqudous temperature wherein the materials are free to move and no stress build up yet. Now my question is, should I assign the stress free temp at the element definition only for Solder and leave other parts un assigned?.

 

stack.png

 

 

 

 

 

 

 

 

 

 

 

 

Thanks again, more power!

 

regards,

Leonel

 

 

Please use plain text.
*Expert Elite*
AstroJohnPE
Posts: 529
Registered: ‎08-30-2012

Re: Setting up Thermal stress Analysis

06-30-2014 10:58 AM in reply to: Leonel16

Hi,

 

I am a little surprised by a couple of statements regarding the heat transfer analysis, but I have never simulated soldering (or welding). For that matter, it has been a long time since I did any real soldering, so I am just going off of what I "think" happens, and it depends on the materials, size (mass) of the parts, etc.

1) I am surprised that the temperatures are uniform within 1.5 degrees C.

2) If I understand correctly, you are implying that you can touch the parts within 40 seconds of soldering them and would not feel any heat. Everything is within 1.5 C of 25 C. It's nice to know that I won't get burned when I pick up the parts. :-)

 

Now to your questions.

Question: "How does the software then knows or consider my cooling down condition on this case?"

Answer: As you stated, you told the software that there is zero stress at 220 C and that the model is at T degrees (~123 C). 123 C < 220 C, so the model is cooler than the initial condition. If you pick a time step closer toward the end of the heat transfer analysis, the temperature will be closer to 25 C, and the delta will be closer to 195 C.

 

Question: "Does this mean, the stress build up at 10 step is considered when solving the stress at step 15 and so on?"

Answer: Not at all. In linear stress, the results ONLY depend on the initial state (0 stress at 220 C) and the current state (123 C or whichever time step you choose). It has no idea whether the temperature reached 1000000000000 C at some time between the initial and current state. By definition, linear means "it doesn't matter what happens between initial and current".

 

Question: "should I assign the stress free temp at the element definition only for Solder and leave other parts un assigned?"

Answer: Technically, every part has a stress free reference temperature, whether you enter a value or leave it at the default value (0 F, I think). Ideally what you want to do is indicate that the temperature profile at time X from the heat transfer analysis is the stress free reference condition. But you cannot do that. (Perhaps you should add that suggestion to the Simulation Mechanical Idea Station: http://forums.autodesk.com/t5/ideas/v2/ideaexchangepage/blog-id/81/tab/popular)

 

The transient heat transfer analysis outputs the actual temperature at each time step. What you really want for the stress analysis is the "temperature difference" between the initial "stress free" condition and the current condition at each time step instead of the actual temperature at each time step. You could do this for a small model by using the "Results Options > Other > Tools > Nodal Results Translator" command. Export the actual temperatures from the transient heat transfer analysis to a CSV file, open the file in Excel, then create the "temperature difference" at each time step, and finally translate those results back to the transient heat transfer file format. During the stress analysis, you would choose this new .TTO file as the source of temperatures. Excel is limited to 1048576 rows (Excel 2010 on my 64-bit Win 7 computer), so as long as the number of nodes in the model times the number of time steps is less than that value, you can do it in Excel.

 

 

Soldering (and welding) are very complex conditions for simulation. Perhaps you can attend the July 2 "Hang out" that was announced a few days ago; it is discussing how to perform weld analysis. 

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16.9 years experience with Simulation Mechanical
Please use plain text.
Contributor
Leonel16
Posts: 14
Registered: ‎06-26-2014

Re: Setting up Thermal stress Analysis

07-01-2014 03:38 AM in reply to: AstroJohnPE

Hi Jhon, 

Very well!...thanks for your help...appreciate it!

More power to you and to Autodesk team...

 

Cheers!

Please use plain text.