adding a thin film component on a cylinder

  • 84 Views
  • Last Post 19 July 2019
  • Topic Is Solved
mjasolis posted this 12 July 2019

Hi! I am very new in ANSYS and I would just like to know how to add a separate component like a thin film or layer (7 mm x 4 mm) on the side of a cylinder (height = 140 mm, diameter = 43 mm). It will not cover the whole cylinder but only that size on the side. Thank you very much in advance

Order By: Standard | Newest | Votes
rwoolhou posted this 12 July 2019

Which software are you going to use? We have various approaches depending on the software & application. 

  • Liked by
  • Jackely
mjasolis posted this 12 July 2019

Hi Sir,

Thank you very much. I am using the Spaceclaim within the ANSYS Workbench 19.1.

The scenario is actually to observe the deformation of a strain gauge (7 mm x 4 mm; thickness of around 0.12mm) made of polyimide or epoxy which is "glued" on a stainless cylinder (height = 140 mm, diameter = 43 mm) under a static constant load of around 344 MPa for 1 hour.

Any suggestion will be helpful to a beginner like me.

 

peteroznewman posted this 12 July 2019

When you say a steel cylinder is loaded to 344 MPa, do you mean the cylinder is in a tensile testing machine that is applying a force on the end that produces a normal stress of 344 MPa?  

What effect do you want to include in the simulation?  Is it a viscoelastic stress relaxation in the polyimide over the 1 hour duration?  Do you have the material properties to model that behavior?

  • Liked by
  • Jackely
mjasolis posted this 12 July 2019

Dear Sir Peter,

The whole system is actually a load cell and the stainless steel cylinder is the cylinder in a load cell taking on force, mass, etc. The polymide is the backing or substrate of the strain gauge attached to the side of the cylinder.

There was a study saying that the creep error reading coming from the system is mostly coming from the polyimide and not from the stainless steel cylinder. I wish to prove show it and they said that ANSYS can demonstrate it. Provided of course I know the constants of the polyimide for the creep equation and I will have to still look for the material properties of the polyimide. If I dont find any, then I would change the polyimide with epoxy since it is also used as a backing or susbstrate.

Yes you are correct, there is a pressure applied on the top of the cylinder at 344 MPa.

peteroznewman posted this 12 July 2019

  • In SpaceClaim, sketch a 43 mm diameter circle on the XZ plane, then with the Pull tool, pull it up to 40 mm
    (don't bother with the 140 mm length).
  • Create a plane at the centerline of the cylinder. Click the Move tool, click the plane and drag it 22 mm out.
  • Now sketch on that plane a 4 mm x 7 mm rectangle at about the center of the cylinder. Click on the 3D Mode button.
  • Click on the Project button, box select the 4 lines, then click the check mark.  You now have a face on the side of your cylinder.
  • Click on the face, Ctrl-C to copy and Ctrl-V to paste.  You now have a surface separate from the cylinder with the extra face.
  • Turn off the visibility of the cylinder.
  • Click the the Pull tool, click the surface and pull it. Type in 0.12 and you will get a R 21.62 mm.
  • Now you have two solids.

  • Liked by
  • Jackely
mjasolis posted this 14 July 2019

Thank you very much sir! I am trying it right now. Just a couple of questions:

1. What do you mean by Click on the face, Ctrl-C to copy and Ctrl-V to paste? Do I click on the face already on the side of the cylinder or on the plane? And when I copy it, where do I paste it?

2. Does this simulate that the face is "glued" to the cylinder and not really originally part of the cylinder?

peteroznewman posted this 14 July 2019

1. I mean after you use the Project button, a new face appears on the side of the cylinder. Click that face.  When you copy and paste, a new surface is created exactly in place where the face is.

2. After you have two solids, you use Bonded Contact to glue them together in the Mechanical app, you don't do that in SpaceClaim.

mjasolis posted this 17 July 2019

Dear Sir,

I now have these in Space claim and mechanical.

1. In Mechanical, under Geometry, can I now delete the surface?

2. In the third photo, did I do it right regarding the bonded contact? Is it bonded now?

Thank you very much. 

 

peteroznewman posted this 17 July 2019

1. You can delete the surface in SpaceClaim, or you can Suppress the surface in Mechanical.

2. You have the proper faces picked in the Bonded Contact.

You can study Creep in a Static Structural analysis, you don't need to use Transient Structural.

mjasolis posted this 17 July 2019

Thank you very much Sir!

About that, can you please elaborate regarding study creep in static structural?

Creep is time dependent on constant load, right? That happens in transient right where I can set how long the pressure will be?

mjasolis posted this 17 July 2019

While trying to solve, these errors appeared:

I placed the Equivalent Creep Strain in the solution and highlighted/chose the small film. Then I pressed solve.

mjasolis posted this 17 July 2019

This also came out after I pressed solve

mjasolis posted this 17 July 2019

 And this is the Solver Output (I apologise for it is long)

ANSYS Academic Research                          

 ***************************************************************
 *            ANSYS Release 19.1     LEGAL NOTICES             *
 ***************************************************************
   
 PERFORM A TRANSIENT ANALYSIS
  THIS WILL BE A NEW ANALYSIS

 LARGE DEFORMATION ANALYSIS

 STEP BOUNDARY CONDITION KEY= 1

 USE SPARSE MATRIX DIRECT SOLVER

 CONTACT INFORMATION PRINTOUT LEVEL       1

 DO NOT COMBINE ELEMENT MATRIX FILES (.emat) AFTER DISTRIBUTED PARALLEL SOLUTION

 DO NOT COMBINE ELEMENT SAVE DATA FILES (.esav) AFTER DISTRIBUTED PARALLEL SOLUTION

 PERFORM A FULL TRANSIENT ANALYSIS
  USING HHT ALGORITHM

 USE AMPLITUDE DECAY FACTOR FOR SECOND ORDER TRANSIENT PARAMETERS
   GAMMA= 0.1000      (ALPHA= 0.3025      DELTA= 0.6000      ALPHAF= 0.1000      ALPHAM=  0.000    )

 NLDIAG: Nonlinear diagnostics CONT option is set to ON.
         Writing frequency : each ITERATION.

 DEFINE RESTART CONTROL FOR LOADSTEP LAST
 AT FREQUENCY OF LAST AND NUMBER FOR OVERWRITE IS    0

           
 *** WARNING ***                         CP =       0.906   TIME= 15:51:49
 The creep integration algorithm does not converge for element 4,       
 material 2, creep model 2.                                             

peteroznewman posted this 17 July 2019

I cut the long output from your post above down to the essential bits of information.

Use a Static Structural analysis. It has Time as part of the solution. Did you read the post in this link?

mjasolis posted this 17 July 2019

I will make it in Static Structural and get back to you. Thank you

mjasolis posted this 17 July 2019

Dear Sir,

I still get the same errors in Static Structural. Please advise.

peteroznewman posted this 18 July 2019

How many elements are there through the thickness of the strain gauge?

Please follow these directions to create a .wbpz file that you can attach after you post a reply so I can see your model. Also say what Release of ANSYS you are using.

mjasolis posted this 18 July 2019

Dear Sir,

Thank you very much. I am using ANSYS 19.1.

Attached Files

peteroznewman posted this 18 July 2019

Cut the model down to a 1/4 model, in other words a 2 mm x 3.5 mm piece and put symmetry conditions on the cut boundaries.

You only need a tiny piece of substrate behind the polyimide. In the example I show, I have created a 1 mm thick piece. I'm also ignoring the cylinder radius for simplicity and have made a flat substrate.

Here is the strain on the face in the Y and Z directions from the cylinder with the pressure, without the polyimide body..

Here is the strain on the tiny piece of substrate without the strain gauge.

See that the surface strain is identical. Below is the mesh on the polyimide. It has 3 elements through the thickness.

Below is the stress on the Polyimide with that strain. Note the large gradient at the "free edge" at the top. The bottom edge is the symmetry face.

If I simulate that for 60 seconds, I can plot the Equivalent Creep Strain, which has a gradient at the top free edge where the stress gradient existed. 

Attached is an ANSYS 18.2 archive which you can open in 19.1 (I don't have that version installed).

Attached Files

mjasolis posted this 19 July 2019

Dear Sir,

Thank you very much for this. Honestly , I didn't understand what you did but I will study it first and I might ask you some more questions. I really appreciate the help!

Michael

peteroznewman posted this 19 July 2019

Dear Michael,

You're welcome.  Please mark one of the posts above with Is Solution to mark this discussion as solved and open a New Discussion in Structural category when you have a followup question. You can point back to this discussion for background in the new discussion by using the Insert Link button and pasting in the URL for this discussion.

Peter

Close