Modelling vacuum to observe cantilever displacement

  • 78 Views
  • Last Post 5 weeks ago
  • Topic Is Solved
Sebastianchi posted this 21 May 2020

Hi there, 

I would like to model the below.
Basically, I have a vacuum source as seen below and it is causing the thin tape to bend downwards (U shape).
May I know how can I model the vacuum or some guidance on how to model it as a vacuum force & calculate the corresponding magnitude on nodes/surface in workbench?

Thank you for your help in advance!

Best Regards,
Sebastian

Order By: Standard | Newest | Votes
Sebastianchi posted this 22 May 2020

Hi!! Can anyone help?

Would appreciate your kind help!

peteroznewman posted this 22 May 2020

A simple model is to create a face on the thin tape and apply a negative pressure to pull the tape down. You can have Frictional contact to allow the tape to stop on the block.  This is all done in Static Structural, or maybe Transient Structural.

A complicated model is the transient fluid-structure interaction where the air is modeled as well as the mechanical parts. In the block are some holes of a specific size with a vacuum on the inside of the holes. This creates an airflow which creates a negative pressure above the block and pulls on the thin tape.

If you want the dynamic response of the tape, the problem is that the pressure on the tape is not constant. If the pressure in the holes of the block is -80 kPa, the pressure on the tape is much less than that when the gap is 1 mm.  As the gap gets smaller, the pressure increases. Only when the tape is sealed on the block and the air velocity becomes zero does the pressure on the tape equal 80 kPa.  The complicated model will compute the change in pressure as a function of the gap.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 25 May 2020

Hi Peter,

Thank you for your feedback. I tried following your simple model, created the corresponding faces on the thin tape.
As the tape's dimension is much larger than the faces which I am applying my vacuum, I needed a total of 36,000 elements which takes alot of time to mesh.

Is there a way to decrease the number of elements?
The below is approximately depicts my situation. The yellow areas represent the areas which the vacuum is effective.

Thank you for your help.

Best Regards,
Sebastian

peteroznewman posted this 25 May 2020

I assume your tape is a solid body.

In SpaceClaim, on the Prepare tab, use the Midsurface button to replace the solid body with a surface body.

In Mechanical, that surface body will be assigned the thickness of the tape.  The surface will need a lot fewer elements to mesh than that solid.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 26 May 2020

Hi Peter,

With regards to your statement earlier of wanting a dynamic response, no I do not. I only require an end-state result. Is static structural enough for my analysis?
In real life, the tape touches the vacuum holes of the block.

Appreciate your help and input!

peteroznewman posted this 26 May 2020

Okay, perfect. Use shell elements, a negative pressure on those three areas and frictional contact between the tape and the block.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 29 May 2020

Hi Peter, can I understand more on the complicated transient-fluid interaction?
Do I have to use Fluent for this ? Or is work bench enough?

peteroznewman posted this 29 May 2020

Workbench is the front end file manager for all ANSYS products, both Structural and Fluids.

You can pull a Fluid Flow (Fluent) analysis system into the project page, just like you do with a Static Structural analysis.

You need Fluent to study transient fluid flow and that can exchange data with Transient Structural to do the interaction.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 31 May 2020

Hi Peter,
Thank you so much for your response. I will certainly take a look at the transient fluid flow to improve my analysis once I finished my key objectives.

Would like to consult you on another matter. I would like to couple static structural & explicit dynamic analysis together.I saw this on a youtube video but they did not show how to set this up. Would need your advice on this.


Sebastianchi posted this 31 May 2020

Could I know how did they add static structural anlysis to the explict dynamic analysis?

peteroznewman posted this 31 May 2020

Hi Sebastian,

If you want to simulate a transient event on a structure there are two methods: explicit and implicit and those are available as Explicit Dynamics and Transient Structural.

Transient Structural is a lot like Static Structural, just with time and mass added so that inertia forces are included in the equations and the solutions include time integration so they can step through time.

Explicit Dynamics is very different and was created to simulate events that implicit solvers would struggle with such as projectiles piercing armor.

I recommend you try Transient Structural for your problem. You don't need to link a Static Structural to a Transient Structural model. You just make the Transient Structural have two or more steps, where in Step 1, you turn off Time Integration while the Static equilibrium is solved, then in Step 2, Time Integration is turned on.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 31 May 2020

Hi Peter,

I understand, thank you for your advice. I think I may have left out some details on the second part of my analysis which may have confused you.

The second part of my analysis, after the thin tape has deflected, there are actually cuboids attached to the thin tape.As the thin tape deforms to a U shape,the positions of the cuboid changes as well,causing the edges of the cuboids to hit each other. 

A suction device is then used to pick up a specific cuboid, during the journey up, the edges of this cuboid collides with the edge of the cuboids beside it.

The main aim of this analysis is to find the stress due to this collision.

peteroznewman posted this 02 June 2020

When you say the cuboids are "attached" do you mean with some adhesive? Or do you mean the cuboids are in contact with the membrane, resting on the surface with gravity and friction holding them in place?

If the cubiods are fastened to the membrane with adhesive, then you can add frictional contact between the cuboid side faces to allow them to press on each other or "collide" and you will be able to see the stress in the cuboids.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 03 June 2020

Hi Peter, Thank you for getting back to me, yes, it is attached to the membrane with some sort of adhesive. The only information about this adhesive contact that I have is that it has a peel strength of 50N/m. For now I have used "Bonded" contact between membrane & cuboid. 

For the collision, just want to confirm with you that explicit dynamic is able to do the job. 

For the 1st part when the tape was deflected downwards due to the vacuum source (please refer to my 1st post), the cuboids collided with each other abit as their faces rubbed against each other. However, I was unable to observe the collision in static structural. I was only able to see the frictional stress at the end state as the faces leaned on each other (at end state).


peteroznewman posted this 03 June 2020

For the collision, Transient Structural will also be able to do the job. I would avoid explicit dynamics because the data is noisy.

For static structural, you should also be able to see the stress building up as the membrane goes down.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 03 June 2020

Hi Peter,

Thank you for your response. Appreciate your input.
Noted on not using explicit dynamics unless necessary. Still would require its usage for the 2nd part of my project.

For the 2nd part of my project, I am modelling for the situation where a pick up collet comes and extract the middle cuboid, at a specified velocity.
The focus of this part of the simulation would be to observe the collision when the middle cuboid travels upwards and its faces collides with its neighbouring cuboids.
I think I would have to use explicit dynamics for this. 

peteroznewman posted this 03 June 2020

No, Transient Structural can do this also.

If you wanted to fire a projectile at the middle cuboid and shatter it into hundreds of pieces, then you would use Explicit Dynamics, Transient Structural can't do that.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 03 June 2020

Hi Peter, 
Thank you for that light of inspiration haha.
Would like to confirm with you, I only have a vague idea but, do you mean I can put a displacement condition/velocity condition?

Thank you for your help on this, Peter.

Sebastianchi posted this 05 June 2020

Hi Peter, 
Am facing some issues with my solution converging.

I have tried the following steps:
Decreasing Minimum, maxium time steps in analysis settings, trying with both tetrahederal and hexagonal meshes.
I have also increased NEQIT from 26 to 100, but to no avail. the solution always gets stuck in this time step.

This is the solution information log for your reference.
It seems the the criterion constantly stuck at 0.1160 at a specific timestep and unable to decrease below it.

*** LOAD STEP     2   SUBSTEP    31  COMPLETED.    CUM ITER =    426
 *** TIME =   1.62000         TIME INC =  0.200000E-01
 *** RESPONSE FREQ = 0.9318       PERIOD=   1.073      PTS/CYC =  54.   
 *** AUTO STEP TIME:  NEXT TIME INC = 0.20000E-01  UNCHANGED

     FORCE CONVERGENCE VALUE  =  0.1246E+07  CRITERION=   6355.   
     DISP CONVERGENCE VALUE   =  0.1400      CRITERION=  0.7143E-02
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1400   
     DISP CONVERGENCE VALUE   =  0.1400      CRITERION=  0.7289E-02
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC = -0.1400   
     FORCE CONVERGENCE VALUE  =   18.72      CRITERION=  0.4202E-02
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.4462E-01
     DISP CONVERGENCE VALUE   =  0.1685E-01  CRITERION=  0.7437E-02
     LINE SEARCH PARAMETER =  0.3776     SCALED MAX DOF INC =  0.1685E-01
     FORCE CONVERGENCE VALUE  =   12.92      CRITERION=  0.2665E-02
    EQUIL ITER   3 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.6337E-02

[Edit: removed middle section of output.]

    EQUIL ITER  98 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2490E-02
     DISP CONVERGENCE VALUE   =  0.2625E-03  CRITERION=  0.1160E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.1054     SCALED MAX DOF INC = -0.2625E-03
     FORCE CONVERGENCE VALUE  =  0.5429E-01  CRITERION=  0.3895E-02
    EQUIL ITER  99 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.4155E-03
     DISP CONVERGENCE VALUE   =  0.2223E-03  CRITERION=  0.1160E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =  0.5351     SCALED MAX DOF INC =  0.2223E-03
     FORCE CONVERGENCE VALUE  =  0.2846E-01  CRITERION=  0.3900E-02
    EQUIL ITER 100 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.6080E-03
     DISP CONVERGENCE VALUE   =  0.6080E-03  CRITERION=  0.1160E-01 <<< CONVERGED
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.6080E-03
     FORCE CONVERGENCE VALUE  =  0.2411E-01  CRITERION=  0.3770E-02

*** ERROR ***                           CP =    2418.594   TIME= 15:11:01
 Solution not converged at time 1.64 (load step 2 substep 32).          
  Run terminated.


Sebastianchi posted this 05 June 2020

Would appreciate your kind help in converging my solution. Thanks!

peteroznewman posted this 05 June 2020

Is the thin tape modeled as a surface and meshed with shell elements?  If not, do that next. Don't use solid elements to mesh a thin tape.

Click on the Solution Information Folder. In the Details is a line for Newton-Raphson Residual Plot, type the number 3 then solve. This will create a plot of force imbalance in the solution for the last three iterations. The location of the maximum N-R Force Residual shows you where you need smaller elements.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 05 June 2020

Understood, thank you Peter for the response. 
Will get back to you soon with your advice implemented.

Have a great Friday!!

Sebastianchi posted this 06 June 2020

Hi Peter,

Your advice worked! Thank you so much!

Can I ask also, how do I turn on nonlinear analysis in transient structural? I think my analysis is linear, is there anywhere to check?

peteroznewman posted this 06 June 2020

Transient Structural automatically has Large Deflection turned on. You can see that under Analysis Settings. That is one form of nonlinearity called geometric. You also have another form of nonlinearity called frictional contact. The third form of nonlinearity is in the material model, where there are many nonlinear material models such as hyperelasticity or plasticity.

Glad to hear your model is working. If your original question was answered, click on Is Solution under the post that best answered the question. Open a New Discussion for any new question.

  • Liked by
  • Sebastianchi
Sebastianchi posted this 06 June 2020

Thank you so much, Peter.
Thanks to you, I managed to overcome many hurdles!

Sebastianchi posted this 5 weeks ago

Hi Peter,

There seems to have some differences in modelling the tape as a surface vs than a body.
May I understand from you what are the differences? 

Will there be any difference in the deflection?

Best Regards,
Sebastian

Close