General Mechanical

General Mechanical

Stress calculation between 2 Material

    • deepsharma25
      Subscriber

      Hello,


      I am new to Simulation and my task is to find the stress between Adhesive and Contact as shown in the Image(Stress Simulation _Adhesive and contact).


      The adhesive is placed between Substrate and chip for isolation. But as the adhesive solidifies it deforms, deforming the contact. Thus, by simulation i would like to know the area with minimum stress.


      Problem is in defining the Physics. Below is the Physics defination: 


      Location in Physics region as 8 volumes ( 6 Contacts and 2 Adhesive) [The image shows only one side of Construction]


      Material for these volumes- One for Contacts and other for Adhesive


      Physics options is program controlled and Solid thermal conditions, temperature is 22°C


      In Structural conditions, displacement for Adhesive is defined, normal to surface.


      I have problem defining Interface conditions.


      Is the definition appropriate? What kind of interface needs to be defined?


      I thank in advance for your response and time.

    • peteroznewman
      Subscriber

      Hello,


      I'm pasting your image inline for the ANSYS staff who are not allowed to download attached files.


      I think you are showing:



      • Adhesive is green solid,

      • Chip is purple with blue conductors,

      • Substrate is light blue,

      • Contacts are brown

      • Base with rib is white.



      I assume the blue conductors on the chip are just modeled as a face carved into the rectangular chip solid, and not a separate solid?


      Can you assume the Base and the Substrate are one solid for this analysis and are united (merged) together?


      If you assume Symmetry, you can cut your model in half and just look at this one end. If you do that, you will have 6 solids instead of 10, but only symmetric results are calculated. If you use Symmetry in a plane along the length of the center of the chip, that will make the model even smaller.


      I assume the Chip rests on the Base, but is not bonded to the Base. In that case, you can use frictional contact.


      Use Bonded Contact from the Adhesive to the Chip, the Base, the Substrate and the Contacts.


      Use Bonded Contact from the Contacts to the Substrate and the Chip.


      For all these materials, you will need to provide two properties, at least Isotropic Elasticity (Young's Modulus and Poisson's Ratio) and Isotropic Secant Coefficient of Thermal Expansion (CTE).


      You can use an artificial temperature change of 100C to simulate the curing of the adhesive by using a value of CTE that represents the size change in the adhesive due to the curing process, scaled to give the correct value at 100C change, not the actual CTE of the cured material.  Set the CTE of all other materials to zero, so they won't change size when the temperature changes.


      The solution to this model will show the stress in the parts due to the size change in the adhesive after curing.


      Regards,
      Peter


       

    • deepsharma25
      Subscriber

      Hello Peter,


      Thank you for your quick response. Below i have answered your questions:


      I assume the blue conductors on the chip are just modeled as a face carved into the rectangular chip solid, and not a separate solid?


      In the Image MMIC contact is blue conductor which is a separate solid but a part of Chip(MMIC).



      (Blue-Chip, Highlighted- Contacts)


      Can you assume the Base and the Substrate are one solid for this analysis and are united (merged) together?


      Base are Substrate are merged.


      If you assume Symmetry, you can cut your model in half and just look at this one end. If you do that, you will have 6 solids instead of 10, but only symmetric results are calculated. If you use Symmetry in a plane along the length of the center of the chip, that will make the model even smaller.


      Yes, i agree. In the below Image, i have made the changes.



      I assume the Chip rests on the Base, but is not bonded to the Base. In that case, you can use frictional contact


      Use Bonded Contact from the Adhesive to the Chip, the Base, the Substrate and the Contacts.


      Use Bonded Contact from the Contacts to the Substrate and the Chip.


      I generated the bonds. 


      For all these materials, you will need to provide two properties, at least Isotropic Elasticity (Young's Modulus and Poisson's Ratio) and Isotropic Secant Coefficient of Thermal Expansion (CTE).


      Yes, they were defined.


      You can use an artificial temperature change of 100C to simulate the curing of the adhesive by using a value of CTE that represents the size change in the adhesive due to the curing process, scaled to give the correct value at 100C change, not the actual CTE of the cured material.  Set the CTE of all other materials to zero, so they won't change size when the temperature changes.


      Defined!


      The solution to this model will show the stress in the parts due to the size change in the adhesive after curing. MMIC contact is a separate solid but a part of the chip.


      The physics is not solved and an error "Update failed for the Solve Physics component in Study.  External component has thrown an exception." is generated. Can you please help me?


      I am below sharing the link of the file. Your helpful comments will be appreciated and am thankful for your time.


      Ansys File: https://drive.google.com/open?id=1ZG9t69toAaiYbqSuB6nkD9BDBdVRaCdD


      Regards,


      Deepak

    • peteroznewman
      Subscriber

      Deepak,


      I downloaded the file in your Google drive, however, AIM 19.2 gave me an error when opening it.


      Please open your project, and use File, Archive to save a .wbpz file.


      After you reply, attach the .wbpz file to your reply using the Attach button.


      Regards,
      Peter


       

    • deepsharma25
      Subscriber

       Hello Peter,


      I tried attaching it, but faced error. The same file as a link: https://drive.google.com/open?id=1XGLXlMH2g9ADi4fqeFxHbaFRJMWgjjem


       


      Regards,


      Deepak

    • peteroznewman
      Subscriber

      Hello Deepak,


      You couldn't attach it because the file size is 160 MB > 120 MB, which is the limit on this site.


      Unfortunately, this file also restores with errors.



      You might get your file size reduced if you save without the mesh. In Mechanical, the mesh is deleted by RMB on Mesh and selecting Clear Generated Data. If you know how to get into the Mechanical interface from AIM, then you can do that. In AIM, you might change the mesh settings and change them back, then save without doing the Generate Mesh operation.  


      Please clear the mesh, then save the file. Restart your computer, start AIM, see if you can restore the archive you gave me. If not, create a new archive. If the file size is < 120 MB, then you can try to attach and if not, give me a fresh Google link. If I get errors again, I will try to open the archive on a different computer. If that also fails, your file may be corrupt and you will have to start over.


      I noticed that once my copy of AIM has tried to open your file, it is broken and cannot open any known good files again after that until I restart the computer.


      Regards,
      Peter


       

    • deepsharma25
      Subscriber

      Hello Peter, 


      Thank you for the instructions. I hope this file works!


      Regards,


      Deepak

    • peteroznewman
      Subscriber

      Hello Deepak,


      I could open the archive attached above, but I am not skilled at AIM.


      When you cut the model in half, I expected to see either a Symmetry condition in the model or a Displacement of X=0 on all cut faces. Please show me that. Without that, the chip will just shift past the symmetry plane.


      Physics > Solver Options > Simulation Step 1 > Solution Progression 1
      Change Substepping to Adaptive and change Initial number of substeps to 10.
      That will help the solver converge on a solution.


      However, the solver failed with an error.



      •  *** ERROR ***                          

      •  The value of TEMP at node 14206 is 4.449199496E+18.  It is greater than 

      •  the current limit of 1000000 (which can be reset on the NCNV command).  

      •   This generally indicates that there are no temperature constraints or  

      •  convections applied.


      I recommend you make several simple models to build skill and confidence in the software



      • Simple block, fixed at both ends, subjected to a temperature rise to examine the stress due to the thermal expansion. You can calculate the expected stress by hand.

      • Same block, but put a square frame around the block that is bonded to the ends of the block. Hold fixed the outer face of the frame sides parallel to the block, leaving the frame sides bonded to the block free to bend.

      • Add symmetry to the second model and get that result.


      Regards,
      Peter

    • deepsharma25
      Subscriber

      Hello Peter,


      I just need some basic help and will try to explain in the images below.


      Yes, Displacement along with support is defined and can be seen in the image below.



      I did the changes and are presented in the image below:



      Regards,


      Deepak

    • peteroznewman
      Subscriber

      Deepak,


      On the cut faces, only X=0.  Y and Z should be free.


      That won't change the fact that AIM seems to be trying to solve a Thermal problem.  In Workbench, I can have a Static Structural model that has a Thermal Condition load such as I suggested above.  That does not invoke a Steady-State Thermal solution. I don't need to solve for where the heat goes or what temperature all the other parts are, I just need to increase the temperature of that one part to get it to expand according to its CTE.  I don't know if you can do that in AIM. If I uncheck Thermal in the Physics Region, then the Temperature boundary condition flags an error.


      I recommend you do the simple problems and show that AIM can do what Workbench can, and just use a simple Thermal Condition load in a Static Structural model. Below is a simple 100 mm long Structural Steel block, zero displacement at both ends (and two side faces), subject to a 100C temperature increase.



      The CTE for steel is 1.2E-5 /C so for a 100 C increase that is a strain of 0.0012 as shown above.


      Regards,
      Peter

Viewing 9 reply threads
  • You must be logged in to reply to this topic.