Community
I haven't tried using this before but I think you can click on my profile name and send a private message to me through the forum with the model. If that doesn't work my email is listed in my profile on the right. I'll Take a look at the model, if there is anything I can help with I'll give suggestions or I'll bring a colleague that is more suited to the issue.
Regards,
Todd
Todd Alford
Sr. Learning Content Developer
My email address is just my username @autodesk.com. Firstname.Lastname. Shoot me the model and I can take a look at what is going on or get it to a colleague.
Regards,
Todd
Todd Alford
Sr. Learning Content Developer
Thanks for the information. It looks like the link is missing, but I can provide some additional guidance for you based on the testing I have been doing and looking at your total assembly more closely.
Based on the load and amount of deflection you mentioned, I have a material from an old training manual we had for one of our other tools that seems to behave reasonably close to your expected outcome that I am using for some further testing right now. We never had the exact material spec, so I cannot confirm how close it is to what you are using, but it allowing me to move forward.
That said, based on the desired deflections you are expecting, we are going to need to approach the problem differently that your original setup. If you look at the attached image, with 0.75" of displacement, we are already missing the true behavior that would be present in the context of your assembly, with the top surface moving below the tapered surface. In reality, the top plate would hold this all in a flat state. Because of this, the upper part will need to be included in the simulation and contact will need to be defined. It is important to note that this will add another level of complexity to this solution. I will work on getting this setup for you throughout the day. Stay tuned.
Sorry for the delay. I had to collaborate with our solver team on this, as I encountered some issues along the way with the setup. Rubber contact problems like this are tricky.
As I had mentioned in a previous post, based on the amount of compression you were looking for, applying the load just to the top surface was not going to give the proper behavior, so this needed to be modeled as an assembly with the top and bottom plates and the center shaft. See the following image. As you test other shapes, you will likely want to use a similar approach where you model all of the parts that will drive the contact and leverage symmetry where possible to simplify the solution.
If you recall, I mentioned that I had some Mooney Rivlin data from an old training manual. I am using that for this exercise, you will be able to see the material data in the Fusion Material library for this file. Use the Manage Physical Materials option under the Material drop down, select the Mooney Rivlin Example model and look at the properties on the Advanced tab. I will point out that this material looks to be about twice as stiff as what your material is, as the force required to compress the bushing higher than what your measurements. This material is probably fine as you start to compare this shape to other shapes and are looking at the performance of the shapes against each other, however, if you are looking to get detailed stress and strain results for the bushing, you will need to provide more accurate material data.
In addition to using the Mooney Rivlin material, and the quarter symmetric version of the assembly, I needed to make a few other tweaks to the setup.
1. Before meshing the model, select Manage>Settings and go to the Mesh heading. Expand Advanced settings and switch the Element Order to Linear. This is a trick the solver team suggested for working with Mooney Rivlin materials.
2. After running the Automatic Contact tool, you will want to modify the contacts from Bonded to Separation. This will allow the bushing to slide as it is compressed. You may want to consider adding friction to this for a more realistic simulation. The attached file has the contacts defined as frictionless.
3. Once you have changed your Contacts to Separation, click on the pencil icon next to each and define the following values; Max activation distance - 0.4" and Stiffness Factor = 0.01
The attached model is setup per this email and ready to run at both 0.75" and 1" of displacement. Please review the setup on each of these models and solved them to see the results as shown in the image below.
If you have any other questions, let me know.
Thanks for your patience.
Mike
I have made some additional progress on your simulation, and I would like to share my findings so far. When troubleshooting these types of issues, it is often helpful to look at the problem in basic scenarios to see what is actually happening.
The first thing I did was to try and run the problem with Bonded contact, rather than Separation contact. This greatly simplifies the problem, however, it may not give the most realistic behavior of the interaction between the top and bottom of the bushing and the metal plates. In doing this, I was able to get the problem to solve. See the following image. I have attached the model for you to review the setup. In looking at these results, I can observe that stress is being created at the contact faces, as the bonded contact is preventing the bushing from separating from the plates, which in reality would probably not happen.
To further validate this finding, I simplified the problem even further, to see what the bushing wants to do when not bonded, as the Separation contact was not solving. To do this, I suppressed all of the parts, expect the bushing, applied the Prescribed Translation to the top face, and a boundary condition to the bottom face to only resist motion in the vertical direction. This scenario is still a bit over-constrained, but is more representative a of a frictionless interaction with the plates, however it prevents the load face and the constraint face from tipping or separating from the "contact" surface. Again, in the image below, you can see that the "constraint" to keep the top and bottom faces horizontal are preventing the way this shape wants to behave under compression.
In this situation, the sliding and tipping behavior that this specific shape wants to do as it is compressed starts to take this problem beyond the type of motion that the Nonlinear Static solver can handle, as the motion is not very stable. If you compare this to the previous shape, the motion that was experienced during compression was very simple, as it was just sliding. Further, sliding friction problems, in general, become a bit hard for the Nonlinear Static solver to handle, because the notion of is it sliding vs. is it sticking is rather dynamic in nature. For this shape specifically, I have worked with our dev team, and we don't think we will be able to get your a truly representative solution using Nonlinear Static for this case.
That said, our Event Simulation solver is better suited to these more dynamic types of problems. More details on this approach in a follow up post.
Hi @SlawsonEngineering -
Now on to the Event Simulation topic. This brings both good news and bad news.
The good news is that this solver solution is much better at handling these sliding/separating contact problems with dynamic behavior. For both models, I was able to use the same setup as we were using in Nonlinear Static with friction included and get results. Please see the following images. A key note here is that this solution is time dependent and best suited for small duration events, 1 second or less is ideal, however, we are currently working on technology to improve this for longer duration events. I bring this up because the rate at which the compression occurs will have an impact on the resulting shape. If it is loaded slower, there is less likelihood that these shapes will buckle, where if they are loaded rapidly, then they might behave differently. You will see some of this behavior in the solid bushing, as it is both loaded more rapidly than what we did in Nonlinear Static and includes friction.
Now for the bad news. Unfortunately, when trying to do this in the current version of Fusion, I encountered some solver issues that prevented me from getting the results you see in the images above. I have since been working with our development teams to fix these problems, and these fixes will be released in a future update. I will update you on this thread when the fixes are live in production and I will share the working files with you.
To end on some good news, once the fixes are released, this will be your most robust path forward. If you remember, we made a number of changes to various settings when using Nonlinear Static solution that we did get to work, however, that was not required to get these to work in Event Simulation.
I am sorry for the time it took for us to find a good path forward and that we have a bit more time in front of us until we can solve these types of problems in a more reliable fashion, but I think once these fixes are in place, you will have a very robust solution for modeling these types of problems.
Thanks,
Mike Smell
Product Manager
Fusion 360
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
![Autodesk Design & Make Report](https://forums.autodesk.com/t5/image/serverpage/image-id/1350519iCB55845EBFC43016/image-size/large?v=v2&px=999" "Autodesk Design & Make Report")