Good Morning Everyone

[This was auto-generated. There may be mispellings.]

Good morning everyone. We are going to start our webinar on Contact Wear Analysis. First, a little bit about who we are, what we do. This is Ozen Engineering. We are the ANSYS distributor here in California. Ozen Engineering was the channel partner of the year in 2015 at ANSYS headquarters.

Here is a picture of ANSYS CEO on the right hand side and our sales team here and the ANSYS sales VP. In this webinar, we are going to talk about highly non-linear features.

We are going to talk about contacts, we are going to talk about wear which is coupled with contacts and also we are going to talk about non-linear adaptivity. ANSYS has made a lot of enhancements in the contact area.

Here is a slide that shows how far ANSYS has come in terms of specifying non-linearities. Now you can even do beam to beam contact just like you see here. You can basically handle beam to beam contacts including highly non-linear deflections in ANSYS.

This started back in version 15 and now in version 16 it has made a lot better. And version 17.2, it has really the best contact implementations ever, including the wear of surfaces that we have specified. With version 16, the contact stabilization damping has been introduced.

So rigid body motion often can occur in the beginning of a static analysis due to the fact that the initial contact condition is not well established. Contact stabilization introduces a viscous damping traction that is proportional to but opposite to the relative velocities between the two surfaces.

This stabilizes the problem. In the past, this has created issues with respect to convergence. But this contact stabilization has been introduced and it has made the contact solution a lot better since the introduction.

This enhanced contact stabilization scheme, prior to this release, automatic contact damping was activated based on the contact status of the entire contact pair in the previous sub steps. Now automatic damping is activated based on the contact status of the current iteration.

And damping is deactivated if any contact detection point has a closed status. In addition, the default damping coefficient has been reduced, minimizing the risk of degraded accuracy while still providing effective stabilization.

Overall, this contact stabilization has brought in a lot better capability in terms of providing good converged contact. For example, in version 15, when we were trying to do a contact problem, you would get 0.2% error in the reaction force.

Now with the contact stabilization damping factor set to 0.1, you can get 0.004% error.

Improved stabilization for sliding contact is being implemented starting with version 16. It can be activated through these key ops and it's very helpful to prevent rigid body motion due to larger sliding for no separation contact definitions.

The main topic today is really the contact surface wear.

The Archer's wear model simulates the progressive loss of material from the contact surface and assumes that the rate of volume loss due to wear is proportional to the contact surface pressure and relative sliding velocity at the contact surface.

In ANSYS, when we talk about contact surface wear, ANSYS updates the contact nodal locations and then re-predicts the contact pressure through the contact elements. As the contact nodes are moved due to wear, the contact pressure is updated as well.

To implement this in Workbench, you will have to insert commands under contacts, correctional contact, insert commands, and you will have to enter the TB commands. In Mechanical APDL, there are a bunch of commands to do this.

And if you want to implement this in Workbench, you will have to insert commands under contacts, correctional contact, insert commands, and you will have to enter the TB commands. Please note that although these slides are from Workbench, this is first implemented in Mechanical APDL.

And in Mechanical APDL, there are a bunch of commands to do this. And if you want to implement this in Workbench, you will have to insert commands under contacts, correctional contact, insert commands, and you will have to enter the TB commands.

In Mechanical APDL, you have to say TB, wear, and that is material 3. That's 4. 3. That's for that specific contact element. Anyway, in ANSYS Workbench, you just put in the word CID, and it will automatically grab that number. Penalty-based formulation is recommended for convergence.

Then that means, you can come in here, formulation, you can change it to penalty-based, and nodal detection is necessary. The material loss due to wear is approximated by repositioning the contact nodes at the contact surface. The new coordinates of the nodes are determined by a wear model.

The following models are available for use. The Archer wear model, which is given by the formula here, is dependent on a wear coefficient, material hardness, contact pressure, and the relative velocity. Wear calculations are based on the contact pressure if you're using Archer's model.

And you have to say TB, wear, and then four commas and ARCH for Archer's model. And then under TB data, you specify wear coefficient, K. That's the first entry there, TB data, C 1. C2 is material hardness, H. C3 is pressure exponent, M. C4 is velocity exponent, N. The C5 is an optional input.

And then the default is use contact pressure in wear calculations. Or if you set C5 to 1, it's going to use nodal stress in wear calculations. And if you use C5 is equal to 1, then it's going to average the wear increment over the contact area of the contact pair.

Use contact pressure in wear calculations. Or if C5 is equal to 11, you're going to average the wear increment over the contact area of the contact pair. And you're going to use nodal stress in wear calculations.

And then if you set C5 to 99, then it's going to calculate wear for post-processing purposes only. The following contact elements support modeling wear.

Contact 171, 172, 173, 174, and 175. To activate contact surface wear, define wear as a material model using this TB command, and assign it to the contact elements. You can use the TB field command in conjunction with TB data to define properties as a function of temperature and or time.

Now this is really important because this brings in a further nonlinearity into the problem where you may want to take into account temperature and or time. The implementation of wear involves two stages. First, the amount of wear is calculated by a wear model.

Next, the geometry is updated to account for wear. Wear models calculate how much and in what direction a contact node is to be moved to simulate the wear based on the contact results at the contact nodes. A generalized form of the RChurch wear model is available.

In addition, you can specify your own user subroutine. The wear increment, which is the rate of wear times the time increment, is calculated by the wear model and used to move the contact node along the direction opposite to the contact normal at that node.

Since this repositioning of contact nodes results in a loss of equilibrium, additional iterations are required to achieve convergence. If the solution fails to converge after the wear is applied, the usual procedure of bisection is used.

Wear is a material removal process, and the underlying solid element does not experience any strain or stress due to the movement of the contact nodes undergoing wear. A large wear increment can result in the opening of an initially closed contact pair.

This may result in convergence problems, especially if rigid body motion occurs. Thus, it's highly recommended that you use very small time increments when modeling wear.

Wear involves repositioning of the surface nodes to simulate material loss, and the element quality of the solid elements underlying the contact elements becomes progressively worse. The analysis may ultimately terminate due to element distortions.

Manual rezoning and mesh nonlinear adaptivity are available for these contact elements. For either method, the total accumulated wear thus far is applied to update the nodal positions, and then the quality of the mesh is improved. And then the analysis is restarted.

Wear is only active for quasi-static and transient dynamic analysis. If a linear perturbation analysis follows a static transient dynamic-based analysis that included wear, the effect of wear calculated at the end of restart point is also included in the linear perturbation analysis.

Wear must be defined before the first SOLVE command is issued. Wear coefficients can be modified between load steps by using tbfield,time command to define time-dependent values.

Although you can redefine wear data by redefining tb,wear between load steps, any analysis involving a restart will use the wear data defined in the first load step, irrespective of which load step is used as a restarting point.

It is recommended that, you use wear only with the following contact algorithms, augmented Lagrangian or penalty function. If you use wear, use either augmented Lagrange or penalty function methods.

If you use wear, with the pure Lagrangian contact algorithm, this can result in convergence problems and is not recommended. Wear is only available when the contact detection point is a nodal point. Also wear is only available for the following contact surface behaviors, standard and rough contacts.

When modeling wear, it's recommended that the underlying elements are structural solid elements or structural couple-field solid elements. Wear is not available for layered solids. In general, you should use asymmetric contact to model wear on only one side of the contact interface.

However, you can also use symmetric contact if wear is desired on both sides of the interface. In this case, define contact elements on both sides of the interface and use the option for nodal stress-based wear calculation to achieve better results.

During rezoning, since the geometry is updated with accumulated wear, the wear is initialized to zero. The same is true for mesh nonlinear adaptivity. Here, we are looking at a demo problem. This is basically, in ANSYS help menu.

Under mechanical APDL, under mechanical APDL, there is a section called technology demonstration guide. Problem number 43 there is contact surface wear simulation. In this contact surface wear simulation, there are actually three problems that they are showing.

The regular contact surface wear problem, and then mesh nonlinear adaptivity based on a wear criterion, and a user defined wear. So there are three different separate problems. So the first one is the wear criteria. Here we are showing one of them here.

This is the nonlinear adaptivity activated problem. And wear due to 30,000 rotations are simulated here. Here is the axis of symmetry, and there is a copper ring over here, and there is a steel ring over here. And there are 30,000 rotations.

So the question is after 30,000 rotations, how much wear is that? Here on the left diagram, on the y-axis we are looking at wear in the y-direction. And what is the y-direction? Y-direction is the axial direction here. X-direction is the radial direction.

Meaning going from left to right, and y-direction is in the vertical direction. That's the axial direction. So here, ANSYS is calculating the amount of wear in the hemispherical ring, and then wear in the flat ring. So this was specified as a symmetric problem.

And on the right hand side here, we are looking at the wear along the contact surface initially. And then we are looking at the nodal stress after wear. So the vertical axis is nodal stress in the y-direction. So as you see here, initially the contact, the stress in the y-direction was high.

But that after wear, the area, where it's acting is enlarged. But the magnitude came down. So wear evens out the contact pressure. Wear results in more uniform contact pressure, and increase in contact area. Again, on the left hand side, we are looking at contact pressure before wear.

And on the right hand side over here, we are looking at contact pressure after wear. As you see, it has a larger magnitude here before wear. And after wear, the contact area is actually larger. And it's kind of evened out. The contact pressure is kind of evened out. Over here.

Adaptive mesh morphing enables simulating large wear. In case you have large wear, this adaptive mesh morphing improves the mesh, and lets you put more elements. Because the more elements you have in the contact area, the better the prediction of the contact stress.

Here is the animation that shows what happens. As wear continues on. As you see here, the contact area increases as wear continues on. And the nodal locations are basically, the nodal locations are updated. So you can actually try this on your own. There are input files.

That you can download from ANSYS customer portal. This is, you can use an input file using the Archer Wear model. And this is the asymmetric contact. There's another input file using Archer Wear model. With nodal stresses for wear and symmetric contact.

That means with this, you can predict wear both on the contact side, as well as the target side. And an input file, demonstrating a user defined wear model. And there's also a userwear.f, which is a user defined wear model example. It's a Fortran, it's a Fortran file.

I mean, it's, it needs to be written in Fortran. And there's an example file in there. So, it's all there. So, you know, if you have any questions, please send them to info at ozunink.com. We'll get back to you with questions. Sometimes it's difficult to answer a bunch of questions.

But feel free to send them to info at ozunink.com. We are here available for software, ANSYS software sales. Again, we are the distributor in Northern California for technical support, training, and also consulting. Our number is 408-732- 4665. And our email address info at ozunink.com.

So thank you for attending this webinar. And we look forward to seeing you in our future webinars. Thanks again and feel free to send your questions to info at ozunink.com. All right. Take care.