Contact between match solid

  • 63 Views
  • Last Post 6 days ago
mekafime posted this 6 days ago

Hi,

Please, I to try to join two parts of a solid, but I have errors. Whats is the best method?

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 6 days ago

Hello, you can use either shared topology or use a bonded/no separation contact

There are numerous posts in the forum on shared topology.

Post 1

Post 2

Post 3

This is what we have from the manual on bonded or no separation contact:

  •  Bonded: This is the default configuration and applies to all contact regions (surfaces, solids, lines, faces, edges). If contact regions are bonded, then no sliding or separation between faces or edges is allowed. Think of the region as glued. This type of contact allows for a linear solution since the contact length/area will not change during the application of the load. If contact is determined on the mathematical model, any gaps will be closed and any initial penetration will be ignored.
  •  No Separation: This contact setting is similar to the Bonded case. It only applies to regions of faces (for 3D solids) or edges (for 2D plates). Separation of the geometries in contact is not allowed.

For more help please specify what you are doing and the errors that you are seeing?

~Sandeep

mekafime posted this 6 days ago

Thanks, 

I to try use "No separation" o "Bonded" but when I to select a face in solid don't selection in "Contact" or "Target"

SandeepMedikonda posted this 6 days ago

But aren't they already penetrated? Its hard to tell, can you hide the parts that are opposing and post a pic? Sometimes, you have to interchange contact and target surfaces.

If you just want the geometries to remain attached, why don't you try the boolean operation on geometries that Peter suggests in this video.

mekafime posted this 6 days ago

Hide a part

 

peteroznewman posted this 6 days ago

Mekafime,

Solid bodies that share a coincident face can be connected without contact definitions in DesignModeler by selecting the bodies in the Outline and RMB to Form New Part. This is the Shared Topology that Sandeep mentioned above.

I have experienced that frustration when the face I picked is not accepted into the yellow highlighted field. I'm not sure why that is, but I have managed to get something working in the end.

If you make a Workbench Project Archive .wbpz file, you can attach it after you reply and I will take a look at what you have.  In your reply, say if you want relative motion between bodies, such as sliding, or no relative motion, like being glued together.  I don't understand why you have all "No Separation" which allows sliding between bodies on the shared face, instead of Bonded contact which glues the faces together and allows no sliding. But your best option may be to Form New Part in DesignModeler, have no contact and use Shared Topology.

Regards,
Peter

mekafime posted this 6 days ago

Hi, 

Thanks for your answer, I have two errors:

- The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

- The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information.

 

I have the model in .wbpz, how i can attach the file?

Attached Files

peteroznewman posted this 6 days ago

What version of ANSYS are you using?

mekafime posted this 6 days ago

18.2

peteroznewman posted this 6 days ago

In DesignModeler, you have Multibody Parts, but the bodies are not grouped in a useful way. For example Part3 has bodies that don't touch each other.

What is the goal of your analysis?  Is it to analyze the stress in the triangular sections that look like they may represent welds?  If so, I can see why you might want the large and small rectangular tubes to be two separate parts, then the weld beads to be two separate parts and use bonded contact to obtain the force going though the weld beads.

What is the intent of the thick plate on the bottom of the large tube?  That can be left as a separate part.

The correction is to Explode the existing parts, and recombine them into those four meaningful parts.

You could get a nice mesh with no slicing. I changed all extrusions (except the first) to Add Frozen.

Now you have 5 solid bodies, each nicely sweepable, and you can use two bonded contacts to connect the two weld beads to the big and small tubes, and another contact to connect the thick plate to the bottom.

You also have to suppress the 3 surface bodies, as they are not involved in the simulation, right?

 I see that you want to do a 1/4 model, so you do need two slices to do that, but no more!

In Mechanical, I see you have a Frictionless contact between the large plate and the large tube, but the force is in a direction to open that up. Change the Frictionless contact to a bonded contact and the problem might solve.

I have to move over to the other computer where I have a Full license as this geometry and mesh has exceeded the Student license limits, so I will read your replies tomorrow.

Regards,

Peter

 

  • Liked by
  • mekafime
mekafime posted this 6 days ago

Peter,

- The goal is calibrate a model in Ansys of a thesis to modificate dimensions and investigate others parameters.

- The welds is to improve the stress in model

- The thick plate represent the bank of testing, in the thesis the autor uses it

- The model is simmetryc, for this reason only the fourth part is neccesary, I think ...

peteroznewman posted this 6 days ago

Mekafime,

Your model converges if you change the frictionless contact to bonded. The force applied is in a direction to separate the parts and there is no gravity, so there is no static equilibrium when you pull one part away from another part that is fixed. A different change that would allow this model to converge would be if you reversed the direction of the force and pushed the parts together.

Under Analysis Settings, you have specified 2 steps, but there is no change in step 2, so make it 1 step.

You have bonded contact between the small tube and the large tube, and the highest stress is in the corner. Did you intend for those faces to be bonded as well as the weld beads?

If you click on Geometry, you can display by Material. I expect you meant to have a different material assignment than what is shown below.

If I change all the bodies to Duplex, I see you have Multilinear Plasticity included.

The first entry for stress is supposed to be the yield strength. Why so low a value?
Have you entered True Stress and Plastic Strain, not Engineering Stress and Strain?
See the spreadsheet in this article Sandeep has pointed to before.

When you use plasticity, you must turn on Large Deflection under Analysis settings.

After making these two additional changes (material and Large Deflection), the model still solves, but a review of the results shows a problem, the weld bead contact is not properly defined.

I added one new Bonded Contact. Now the model looks right. The maximum strain appears on the inside of the wall, but that may move around when you refine the mesh and use smaller elements.

Attached is the ANSYS 18.2 archive.

Regards,

Peter

Attached Files

mekafime posted this 6 days ago

Peter,

Thanks for your help !. 

I think that bonded contact between small tube and the large tube is to try avoid two pieces has interferences, the welds must doing the work.

All material is Duplex.

I didn´t understand the spreadsheet of Sandeep, I to tried introduce manual valores seeing the chart plot

"Initial Information" is a new method for me, I will try to learn.

peteroznewman posted this 6 days ago

You should delete the bonded contact between the small tube and the large tube, leaving only the weld bead contacts to carry the load.

To get accurate results, you need to take the Engineering Stress-Strain curve and use the equations to compute True Stress, Plastic Strain, Elastic Strain and True Strain.  The curve of True Stress-Strain has higher values of stress than Engineering Stress-Strain.

Here is another reference to creating a Multilinear Plasticity Hardening Table. This is a little more complicated than the reference given above because it is using experimental data that includes an offset on the Engineering Strain zero.

Please share the reference you have for the stress-strain curve for the Duplex material.  What is the Yield Strength of Duplex?  What is the Young's Modulus of Duplex?

mekafime posted this 6 days ago

 

 

I took differents points from this plot (n=15) and introduce to the material table in Ansys.

 

The material properties, I used 160x80x3

SandeepMedikonda posted this 6 days ago

Hi,

  I believe you are referring to this discussion.

The following resources should help a little: 

Resource 1

Resource 2

~Sandeep

 

Close