Fusion Ultimate - Non-linear
Can you offer @Anonymous some help on this subject.
Phil Procario Jr.
Owner, Laser & CNC Creations
Also sorry to hear about the struggles with an Event Simulation in Fusion 360. Are you getting a particular error message or can you elaborate what you are having difficulties simulating?
If you can share a sample design with me, I'd be happy to take a look at it and make some recommendations.
Potentially Interesting Content/Conversations about Fusion Simulation:
- Fusion Simulation Deep Dive
- Getting to know the Event Simulation study type in Fusion 360 Ultimate
- Quick start for event simulation
- Simulation in Fusion 360 - Don't Get "Stressed" Out
I believe you should be able to use the Transient Load to apply a point load to a vertex on the model geometry.
Are you having difficulty using this command or does this command not meet your requirements?
If there are any specific questions about the explicit solver (event simulation), I'm happy to do my best to answer. Please feel free to ask questions. I am happy to help.
Nathan Chandler
Principal Specialist
@Anonymous and @Anonymous -
I have been doing some investigation on the setup of the ROPS and FOPS files that were sent. In this post, I will discuss my findings on the ROPs file and follow up with another post on the FOPs file.
In ROPs - Study 10, I noticed the following issues with the setup that will definitely create some issues in getting the correct results.
1. By default, Event Simulation uses separation contact. This is different than Linear Static or Nonlinear Static in Fusion, and this is partly because many of the use cases we were targeting involved moving contact where parts where coming together over time. In the case of an assembly, such as your design, an extra step is needed to ensure the parts are "bonded" together correctly. This is an area we can certainly look to improve in the future. In the meantime, you should always take advantage of the DOF view on the Display Panel. This will allow you to see the unconstrained parts in the design. In the following image, you will see that the majority of the cab is not connected to the rigid sub-structure. To ensure that proper bonding is created for an assembly such as this, when running the Global Contact tool, be sure to check the Proximity Bonded option. You also have the Proximity Distance option which will allow you to bond across small gaps if required. After running Global Contact with Proximity Bonded turned on, notice the DOF view now shows everything constrained.
2. I do not believe that the loading has been applied properly. When I look at your load setup, I see a load magnitude of 2.254e5 N in the Transient Load Dialog. Next, when looking at the load curve, I see that you have defined a multiplier of the same value. This will give you a total load applied to the model of 2.254e5 N multiplied by 2.254e5 N at the time of 0.0008 seconds. My intuition tells me that this was not your intent and that the correct magnitude is what is defined in the Load dialog. In Event Simulation, the multiplier in the load curve is exactly that, as it will multiply against what is defined in the Load dialog at a given time. If your intended load is 2.254e5 N, then your Multiplier value should be 1.
In ROPs - Study 13, similarly, I noticed a few issues that would likely prevent you from getting the proper results.
1. My comments from above, both comments 1 and 2 are present in this setup. I would suggest using the suggestions above to correct the setup in Study 13.
2. Next, I see that you have an X translation boundary condition applied to the same face in which it looks like you have applied point loads by cutting small holes in the geometry. This boundary condition is constraining the load direction, so the only deformation that will happen on this face is at the holes. I am not sure if this was your intent or not, but this will prevent the entire structure from deforming beyond on these point loads.
3. It is important to note that there are TWO different behaviors that can be obtained when applying a force in Fusion. If you look at the Load Dialog, there is a checkbox for Force per Entity. In the model that you have setup, your magnitude of 45080 N is distributed equally across the 5 faces in which is it applied. If the Force per Entity box was CHECKED, then this full magnitude would be applied at each location. I point this out only because this could change your results.
I have attached an F3D that reflects all of these changes, see the 3rd and 4th studies in the browser.
A few additional general comments.
1. Are the 5 holes on the left side of the cab where the loads are applied being used to represent a point load? If so, there are some less expensive methods we can use to split the geometry. In the current form, mesh quality at those locations is pretty poor and the Event Simulation solver is not a fan very small and misshaped elements. Further, in reality, are these actually point loads, or is there some contact area from the mechanism applying the load?
2. The displacements seem a bit small. I would check the load magnitudes with respect to the dimensions of the model and the material properties.
3. I see you are defining the base of the cab to be rigid. If this is true, then you could consider suppressing those parts altogether and placing boundary conditions at the mating faces. This would help with your overall run times.
I hope this feedback moves you further along with this model. I will review the FOPs model and provide similar feedback.
@Anonymous and @Anonymous
Now on to the FOPs file, I will go through this study by study.
Study 1 :
1. Similar to the ROPS file, I would always pay attention to the DOF view to ensure that the contacts created accurately reflect the intent of the design. In the image below, you can see that even with bonded contact, parts are still red, meaning contacts were not established correctly. The plates on the rear of the cab are not touching the surrounding parts within the default tolerance. The plates on the top of the model do seem like contact should be created, so I will log this with our development team. By increasing the tolerance to 0.2 mm the parts will be bonded and would be ready to run. Again, pay attention to Body 107, as it may have gaps that you did not intend.
2. Considering there is no load applied to the cylinder on the top of the cab, this part should probably be suppressed.
3. I see that you have a number of connectors defined in this model. I will point out that without modifying the contacts from Bonded to Separation, these bolts will not contribute to the design, as the Bonded contact has all of the parts connected. Without changing all of the contact pairs, this model will solve with these minimal changes. See the following image.
Study 2:
1. The only difference I see between Study 1 and Study 2 is the lack of connectors. If you follow the steps used to resolve issues in Study 1, then this model solves and should results.
Study 4:
1. The comments for Study 1 regarding the cylinder on the top of the cab and the contact settings hold true.
2. Similarly, the default contact being bonded will negate the impact of the bolted connections.
Study 5:
1. This model was running as you sent it, however, if you look closely at the results and remember what I said about contact in Event SIM, there is no bonded contact throughout the assembly. This model should follow the practices outlined in a previous post to make sure that contact is correct for Event Simulation. Note: your connectors are suppressed in this study. This model is still running on the cloud, so no result images yet, but I expect the results will look fairly similar to what it looked like when the parts were in Separation contact, however, I expect the stress to be carried in a wider area once bonded.
I have attached an F3D for you to run with all of these changes.
Please let me know if you have any further questions.
Thanks,
Mike
@Anonymous and @Anonymous
Now on to the FOPs file, I will go through this study by study.
Study 1 :
1. Similar to the ROPS file, I would always pay attention to the DOF view to ensure that the contacts created accurately reflect the intent of the design. In the image below, you can see that even with bonded contact, parts are still red, meaning contacts were not established correctly. The plates on the rear of the cab are not touching the surrounding parts within the default tolerance. The plates on the top of the model do seem like contact should be created, so I will log this with our development team. By increasing the tolerance to 0.2 mm the parts will be bonded and would be ready to run. Again, pay attention to Body 107, as it may have gaps that you did not intend.
2. Considering there is no load applied to the cylinder on the top of the cab, this part should probably be suppressed.
3. I see that you have a number of connectors defined in this model. I will point out that without modifying the contacts from Bonded to Separation, these bolts will not contribute to the design, as the Bonded contact has all of the parts connected. Without changing all of the contact pairs, this model will solve with these minimal changes. See the following image.
Study 2:
1. The only difference I see between Study 1 and Study 2 is the lack of connectors. If you follow the steps used to resolve issues in Study 1, then this model solves and should results.
Study 4:
1. The comments for Study 1 regarding the cylinder on the top of the cab and the contact settings hold true.
2. Similarly, the default contact being bonded will negate the impact of the bolted connections.
Study 5:
1. This model was running as you sent it, however, if you look closely at the results and remember what I said about contact in Event SIM, there is no bonded contact throughout the assembly. This model should follow the practices outlined in a previous post to make sure that contact is correct for Event Simulation. Note: your connectors are suppressed in this study. This model is still running on the cloud, so no result images yet, but I expect the results will look fairly similar to what it looked like when the parts were in Separation contact, however, I expect the stress to be carried in a wider area once bonded.
I have attached an F3D for you to run with all of these changes.
Please let me know if you have any further questions.
Thanks,
Mike
Hi @Anonymous and @Anonymous -
A few comments on your last couple posts.
1. Currently, Event Simulation is in Tech Preview. The Tech Preview process allows us to collect feedback from users about what is working, what is not working and what additional functionality is required to solve a common set of problems. While this study type is in Tech Preview, it is free of charge and is time limited to jobs of less than 12 hours. Once commercialized, we will have a cloud credit charging scheme in place for this study, similar to other cloud solves where you see credits deducted with each run and jobs will not be time limited to 12 hours.
2. As I mentioned, part of the Tech Preview process is about collecting feedback. One of the major pieces of feedback we have gathered so far is Event Simulation's ability to handle scenarios where the time duration is longer than one second, as these jobs typically hit the 12 hour time limit. We have been actively working with our solver team to better handle these type of events and have been making some progress that will be made available later in a future release. In the current form, Event Simulation is best suited for short duration events and we have had success with customers doing snap-fits and crushing/collapsing of container type of problems.
3. Regarding the small displacements in the Event Simulation model, after further review, I believe the issue we are facing is due to duration of the event that we are needing to use to stay under 12 hours. With such a short duration to apply the load, the load is likely not overcoming the inertia of the cab. This can be demonstrated pretty easily with a simple cantilever beam. See the attached f3d. If you compare the studies, you will see that when Event SIM uses a constant load, the displacements are very similar to that of the linear static and nonlinear static stress runs, while the Event SIM model with the default duration, the displacements are much smaller. When the duration is increased, the displacements become similar to that of the static runs. While this is not helpful for your design, this does explain the behavior you are seeing. I have made a few tweaks to your designs and have those running now. When I get results, I will share an update.
4. Regarding the Polycarbonate material behavior, while I see that you have defined it as nonlinear, you have not defined any post yield data. When using the Nonlinear Plastic material model, for materials other than what is in the Fusion Nonlinear Material library folder, the user must define the post-yield curve. If you do not have this curve data, you can consider using the Elasto-Plastic material model where a Tangent Modulus value will be used to define the post-yield behavior. This approximated to 10% of the Young's Modulus by default.
Stay tuned for updates from my extended duration runs.
Thanks,
Mike
