load test
Before you try any Simulation, you should do some homework. The results of Simulation are used to make safety critical decisions and you really should fully understand the Sim environment in Fusion before you attempt to use it in design.
Start by reading the Simulation section from Help/Learning. Here is a link:
Thanks,
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Hi,
I thought a lot about your question and I think it is kind of typical and common question that every designer would ask. I support Phil’s perspective of learning things upfront as a safe and pragmatic approach, but I want to offer an alternative perspective: Just try it! You may learn a lot about your design and get directions of what to improve relatively easily.
Please let me share with you what I did with your model. It took me about 30 minutes so it may be worth investment of your time.
- I imported your STEP, switched to SIM workspace and create new Static Stress study.
- I created one load and one support
- I run the solve, ignored all the warnings (I can return to it later and make the setup perfect)
- I figured out that I really should add at least one manual contact there as parts moved. I added bonded contact (this is a fist iteration for getting quick results, finally there would be more contacts of different types)
- I run the solve again and get results that looks better, you can see a natural deflection there, etc. But the stress is really low – about 10 MPa.
- I could expect about 100 MPa from a steel so I increased the load to 10 kN.
- I run the solve and figured out that the critical part of my design is in two little support beams
- There is disproportion in size of the main beam and two little supports. I could address it by re-designing the supports, but I just suppressed it for now
- I run the solve again and identified critical areas between safety factor 0 and 2 be using tresholding
- These are IMHO artifacts of missing contacts (I did just one simple contact above) so I’m going to ignore it
- So finally here is the resultant picture
What I can learn from it:
- Load 10 kN is OK with safety factor above 2. So it will break (actually deform in non-returnable way) under 20 kN (20 tons of weight)
- BTW: 20 kN is a value that you probably never want to communicate with your customers. I would apply safety factor that would result in 5 to 7 tons in maximum of static load (if there is any dynamic involved it would need more analysis)
- Two little supports needs to be redesigned (if you would be interested I can show you how I would use Simulation to drive to better design of these)
What I would do as next steps:
- What was the design intent? If that would be to carry just 1 ton of static load then it is overdesigned. If you want to use it for 100 tons then a different design or at least sizes would be needed.
- I would redesign to little supports
- As a last step I would take the semi-final design and setup the simulation properly. It would take more than just 3O minutes of your time, you would need to carefully think about contacts and maybe heal some of your bodies from STEP. But it will give you more confidence in results
Just to be sure I’m on the right track I did a simple crosscheck. I created a simple model of beam with the same dimensions as your design and put there the load of 20 kN
It gives me 1.08 minimal safety factor. So this beam will be deformed/broken with almost the same 20 kN as I got above. That tells me that assumptions I did above were OK.
Please note that I did couple of assumptions and simplifications to quickly get initial results. This is the way I like to solve problems – in iterations to early identify big issues and solve smaller problems as a next step. Some engineers prefer to do a perfect simulation setup as a first step and use if for decision making. I just wanted to offer you a different perspective of using Simulation tool that is really easy to use.
Thanks,
Vasek
I also had been working on this, but more as a mesh study. The fact is the support tubes will fail first. Because they are long and slender they may fail by buckling long before they reach yield stress. Buckling analysis, which is not available, would only show this. Overall, I am impressed with the robustness of the solver to quickly solve this many dof with contact.
I am of the opinion that one should perform a simple hand calculation or start with the something like the beam model above to get a rough idea of the results. When a model gets complex, more things can go wrong, and then you then have an idea if the results are way off. First do a default mesh for a quick solve, then adjust the mesh size and use refinement once you see things are working properly. Start with simple models & refine as Vasek said.
For assemblies make sure you check off 'use part based measure for assembly mesh' in the Settings|Mesh dialog. It is a compromise--more advanced software allows you to set mesh size on each part (and more).
Suppress all unessesary components. The hook from the top of the inner boom does not need to be meshed. Because of the glued contact assumption, the pin did not need to be included. A model with more advanced sliding contact analysis would include this. If the contact forces on the pin could be extracted, an analysis of just the pin could be done. Maybe contact pressure would show it. Havn't tried it.
With contact you will probably get a warning to switch to GROUPS view. You then have to manually connect the two groups. Think about what surfaces will be in contact; when the two groups turn one color there still may be other surfaces that need contact to model the real situation.
SET UNITS AS SOON AS YOU ENTER THE SIM ENVIRONMENT! The default is custom & custom is metric.
Clone study lets you try different things with the same model setup & keep the original for comparison. Right click on the study name to get to it.
I plan to post some tips for those new to FEA. In the mean time, make some models & ask questions.
Thanks,
Paul
