Learning Forum

[murali macharla]

Hello Everyone,

I am performing the creep simulations and i am constantly getting error saying that creep limit ratio is exceeded and the analysis is stopped. I have tried all the creep limit ratios from 1 to 100 and i am still getting the error. Is there anyway to calculate the creep limit ratio ? and how should i achieve convergence here. Please someone help me . 

Best regards,

Murali.

 

[peteroznewman]

Hello Murali,

Have you turned on Auto Time Stepping?

Did you set it to time substeps?

What values did you use for Inital, Min and Max time substeps?

The corrective action is force the solver to use small time substeps on the Max time substep.

The Min time substep can be 100 times smaller than the Max time substep.

The Initial time substep can be equal to the Max time substep.

[murali macharla]

Here i am attaching the force convergence graph. I can't see anywhere it is trying to achieve convergence. The graph continue like this and stops at some point. I am thinking that material parameters are wrong. Is there anyway to check , whether the entered material parameters correct or not ?

 

 

 

[murali macharla]

Hello Peteroznewman,

I used auto time stepping.

I set the substeps as time steps.

Even after using the following settings the simulation is not coming convergence.

The settings looks like following .

Best Regards,

Murali.

[peteroznewman]

What load is applied in step 1?

If you turn creep effects off, what is the maximum stress at the end of step 1?

 

[murali macharla]

Hello Peteroznewman,

In all steps, the only load applied is temperature. In the first step, the applied temperature is 280c.

In the next steps, it is cooling down to room temperature from 280c.

If i turn creep effects off, the stress(Von mises) at the end of step 1 is 128 MPa. 

[peteroznewman]

What is the environment temperature?

What is the reference temperature of all the materials?

Is the step 1 temperature load Step Applied or Ramped up from the Environment temperature?

Try using Initial Time Step of 1e-4 s.

Turn on Large Deflection.

Turn off Weak Springs (why would you need them?)

[murali macharla]

The environment temperature is 280c.

The reference temperature of all materials is 22c. 

In step 1, the load is same as environment temperature i.e., 280c. In step 1 , the load(280c) is kept constant for 1 minute. Then it is ramped down in other steps.

I have already used the initial step as 1e-4, still not converging. I even went till 1e-8, there is no convergence.

Ok i will turn on large deflection and run the simulation.

I added week springs  as i am performing simulation on chip and substrate bonded with interconnect. Here they attach through bonded contacts. So, i turned on weak springs. And i also need to check warpage of chip and substrate, so it doesn't make sense to give boundary conditions. 

And yeah i am using only direct solver. 

[peteroznewman]

If you are assembling parts at 280C then want to monitor the creep as it cools down, both the material reference temperature in the CTE definition and the environment temperature should be 280C so that there is zero strain at 280C at the beginning of the simulation.

In that case, step 1 would not be a temperature load of 280C, it would be whatever temperature you want to cool down to.

[murali macharla]

so, in step 1 if i keep room temperature of 22c and time of 5 minutes as it is our cool down time. There is no need of adding any other time steps and temperature ?. Will that be enough to observe creep in cool down process?.   

[peteroznewman]

You want two load steps. Step 1 with a ramped temperature load of 22 C and an end time of 300 s to cool down over 5 minutes. Then a second load step to track continuation of creep for as long as you are interested with the temperature constant at 22 C. Could be an end time of 86,400 s to look at the creep after 24 hours.

Auto Time Stepping will ensure creep is accurately captured during the first 5 minutes and the 24 hours. You might have different Minimum and Maximum Time Step sizes for step 1 and step 2.  Carry over time step may be a good choice.

[murali macharla]

I made the changes as you said and the simulation is running. But, with 12 cores itself, it took 14 hrs to calculate just 3 seconds (still ansys need to calculate creep for 597 seconds), and it has generated almost 40 GB of data for those 3 seconds. I am not sure why it is like that. is there anything i am doing wrong. I have following settings.  

I am using 'direct solver'. 

weak springs 'on'

creep limit ratio is ' 100' . (any value below 100 is not making the simulation to run)

Initial time step : 1s

Min time step : 1e-4s  (simulation is not running for )

Max time step: 40s 

Environment temperature : 280c 

Will be waiting for your reply.

 

 

[peteroznewman]

If the computer has only 12 cores, using all of them does not deliver the shortest possible solve time. Use one less than every core. There is also diminishing returns, so the solve time might not be much longer at 8 cores than 11 cores.

The number of nodes and elements in the simulation has a significant impact on the solve time per iteration. You could use a coaser mesh and cut the number of nodes and elements in half by increasing the element size. The ideal mesh uses smaller elements where the result change rapidly, either in time or location and larger elements where the results change slowly in time or location.

The time it takes to solve a transient model is proportional to how many iterations it must make. That is determined by the convergence criterion you impose on the solution. If you give it a small convergence tolerance, it will need more iterations, if you provide a larger convergence tolerance it will do fewer iterations.

The step controls is a place where you might have used a smaller value for Max time step when the solver would have been happy with a larger value. That does not seem to apply to your situation.

Just because the first 3 seconds took 14 hours, doesn’t mean you can linearly extrapolate to estimate the solution time for 600 seconds because the rate of change exponentially decreases and when it does, the time steps will get much larger and it might only need a few more hours to finish. 

Click on the Solution Information folder. In the Details window is the Solution Output.  The default setting is Solver Output.  That is all text, but sometimes you get a clue as to what criterion is limiting the size of the step.  Change the setting to Time Increment. On this graph, you can see if the solver is bumping up against a Min or Max Time Step limit you imposed, or if it is choosing the best Time Step it has decided on.

You can control how much output you are getting by clicking on Analysis Settings and going to the Output Controls category.  Do you need both Stress and Strain?  If not, turn off the one you don’t need. Change Store Results At to Equally Spaced Points and type in 300, then you will only get results on a 2 second increment over the 600 second end time.

What version of ANSYS are you using?  Year and R#.

If you can share your model, use File Save As to a new name. In workbench right click on Model and select Clear Generated Data. That will delete the mesh, then File Save. Next do File Archive to create a .wbpz file choosing No Results and put that file on a File Share site like Googe Drive or OneDrive.