General Mechanical

Applying diamterically fixed support to cylinder face

• liamjstrachan
Subscriber

Hello,

I am a new student on ANSYS and would like to know how I would be able to apply a fixed support to a 3D cylindrical model diametrically as ive tried to show in the picture attached.

• peteroznewman
Subscriber

Please describe in more detail what you are trying to model.

You can draw solid bodies and define contact between the flat bodies and the cylindrical body. A feasible model would have a fixed bottom plate, and a top plate on a vertical translational joint. A joint load can apply a force to squeeze the cylinder between the flat plates. Frictional contact would be needed, otherwise the cylinder can slip out from between the plates.

Ansys Employee

Moving to structural mechanics for better response.

Regards,

Keyur

• liamjstrachan
Subscriber

My model is composed of a 3D cylindrical component (20mm diameter x 4.76mm thick) with another 3D cylindrical component (20mm diameter x 0.25mm) bonded to its face acting as a coating. I am then trying to simulate the stress in the coating and at the bond between coating and substrate due to deflection when a compressive load is imposed vertically down on the component. For the component to buckle or cause some sort of deflection in the axial direction, i need to make sure the top and bottom of the component are fixed.

i appreciate your response and your suggestion seems perfect for what I'm trying to achieve, however since i am totally new to ANSYS, i still think I'm not fully understanding. Just a few questions:

1. do the flat plates need to be modelled into 3D also?

2, By fixed bottom plate, does this mean by bonded contact?

3. How do i make the top plate on a vertical translational joint?

4. If the plates are fixed by bonded contact (if thats what is meant) can i still apply a frictional contact on top?

Apologies for all the question, hopefully I'm making sense.

• peteroznewman
Subscriber

1. Yes, make the flat plates in 3D but make them thicker, like a 6 mm cube, so the cylinder is in the center and the contact faces must be tangent to the cylinder.

Symmetry should be used to make this problem easier and faster to solve. The cylinder gets squeezed from both sides equally, therefore if you put a horizontal plane through the center of the cylinder the top half and the bottom half of the cylinder look like mirror images. Therefore, cut the model in half (keep the top) and use a Symmetry boundary condition. Similarly, if you put a vertical plane through the center of the cylinder, the left side looks like a mirror image of the right side. Therefore, cut the model in half again (keep the left) and use another Symmetry boundary condition.

2,3,4. Use a Static Structural analysis block, and import or draw your Geometry in SpaceClaim, then close that and open the Model. Click on the Static Structural branch. Since you are not interested in the deformation of the cube, you can make it rigid. Pick the body in the tree and where it says Flexible, pull down and select Rigid. While you are there, rename the three solids: Base, Coating and Plate.

RMB on the Connections folder and Insert Joint. There are a row of filters on the toolbar for Vertex, Edge, Face and Body. Pick the Face filter. Select the top face of the top quarter cube. Change Body-Body to Body-Ground. Change Fixed to Translation. You then have to reorient the Coordinate System under the joint so that the X axis of that Coordinate System points in the Global Y direction.

Drag and drop that Translation joint on the Static Structural branch to create a Joint Load. Change from displacement to Force and enter the force you want, but use a negative number to make it point down.

The default installation will automatically create all the contacts, but they are all bonded. Select all the contacts and RMB to Rename based on definition. That will make it use the names you gave the solids above. Select the two contacts with Plate in the name and change them from Bonded to Frictional. Enter a friction coefficient.

Go to Engineering Data and create the materials for Base and Coating. At a minimum you need a Isotropic Elasticity and in there you enter Young's Modulus and Poisson's Ratio.  Refresh the Project, then in Mechanical, assign those two materials to those two parts.

In Analysis Settings, you will want to turn on Auto Time Stepping and use 100 substeps.

In Meshing you will want to add mesh controls to get nice small elements at the contact point.

Then you can finally Solve.

Regards,
Peter

• peteroznewman
Subscriber

• liamjstrachan
Subscriber

Appreciate the in depth response peter, it has been of great help and allowed me to model what I was after.

One last question, since this is trying to replicate a diametrical compression test, should I keep the contact between the bottom plate and the model bonded? or should I still keep the contact frictional?

• peteroznewman
Subscriber

The contact between the plate and the cylinder should be frictional contact, not bonded. If you use symmetry, there is only one plate, not a top and bottom plate.

You can show your appreciation by clicking Like below the posts that are helpful.

• liamjstrachan
Subscriber

I understand symmetry will make the problem easier, however for this project I have to simulate the full model.

Also, instead of cubes, im using two cuboids as the flat plates (assign steel properties to them and use them to apply compressive load) but when I go to extrude, I get an error "intersecting profiles are not allowed for 3D profile". How do I overcome this so I can model my two flat plates?

• peteroznewman
Subscriber

You can create a quarter model and use a feature in post-processing to mirror the elements and results so that it looks like a full model. A screen snapshot of that will be indistinguishable from a full model.

Delete the Extrude and the Sketch, which has 10 lines on it. On Plane 13, make a new Sketch. Use the Rectangle tool in Sketch to drag from one corner to the diagonally opposite corner. You will have 4 lines. That sketch will extrude cleanly.

• liamjstrachan
Subscriber

When creating the vertical translational joint, how do I orientate the coordinate systems so the local X is pointing in the global y direction?

• liamjstrachan
Subscriber

Managed to get the coordinate system rotated, however when I ran the simulation, I got the above error.

• Sandeep Medikonda
Ansys Employee

Please see if this suggestion from the manual help?

You need to constrain your model properly. How is the part in the middle constrained? I am assuming just using contacts, this could be the problem.

Regards,
Sandeep

• peteroznewman
Subscriber

You could get rid of this error by building a half model, cutting on the YZ plane and setting the cut face to have X=0, which is the Symmetry Boundary Condition. You can make the results look like a full model by mirroring the results display.

I assume the contacts are frictional with a non-zero coefficient of friction.

Under the Connections folder, Insert a Contact Tool and Generate Initial Contact Results. Check to see that all the contacts are closed.  If not, change the Contact to include Adjust to Touch.

Under Analysis Settings, turn Auto Time Stepping On and set the Initial Substeps to 100 and Maximum Substeps to 200.

• liamjstrachan
Subscriber

I have the coefficient of friction set to 0.2, should it be 0?

Also, there is the results of the contact tool.

Is there any way I could manage to share my file so that you could have a look at it if possible?

• peteroznewman
Subscriber

Coefficient of friction should be 0.2 not 0.

After you Insert a Contact Tool in the Connections folder, expand the Contact Tool and there will be Initial Contact Status. You have to RMB and Generate Initial Contact Status, then there will be a table in the Worksheet.

You can share your file so I can have a look at it by following these directions.

• liamjstrachan
Subscriber

My contacts are infact open, but I cant seem to find the "adjust to touch" selection?

Also, one I convert to a wbpz file, how do I attach?

• peteroznewman
Subscriber

After you post a reply, the Attach button appear on the right side of your post.  Browse then Upload.

• liamjstrachan
Subscriber

I changed the interface treatment to "adjust to touch" to close my connections. Now, the simulation seems to take forever to solve as it has been stuck (see picture attached) for the last 5 minutes.

• peteroznewman
Subscriber

The file you uploaded did not have the Adjust to Touch change made in the two contacts, which were open.  I made that change and a few other small tweaks. Once you hit Solve, you can monitor the progress by clicking on Solution Information and picking Force Convergence instead of Solver Output. Then you will see the graph below being plotted a point at a time.  That is a good way to know the solution is making progress.

The solver needed 24 iterations to apply the full load from the 100th starting step. If you solve again, you can try to replace the 100 with 20 and it might reduce the number of steps needed to get to the full load (Time = 1 s).

The wait time for the 24 iterations depends on the size of the model and the number of cores you are solving on. If you use quarter symmetry as I suggested above, you will cut your wait time to a quarter. If you use a rigid surface instead of a steel block, you will cut the wait time further. This full model took 5.8 minutes solving on a 15 core computer and 9.6 minutes on a 4 core computer. The solver needed  6 GB of free RAM to solve it without using the HDD. If you have a 2 core computer with only 4 GB of RAM, it will take more than 15 minutes. You can see the Elapsed time if you flip back to the Solver Output and scroll to the bottom.

Looking at the Stress results, you can see that you don't have small enough elements to capture the true solution, which is peak stress below the surface.  The coarse elements you have show the peak stress at the surface, which is incorrect. Smaller elements are going to increase the wait time for the solution. You don't need small elements all through the solid, just at the contact points. This is where the sizing mesh control Sphere of Influence is useful.

Regards,
Peter