October 27, 2018 at 2:44 pm
October 27, 2018 at 3:29 pmpeteroznewmanSubscriber
First change, make sure there are 2 elements across the thickness of any part by setting Proximity to Yes and Num Cells Across Gap to 2.
Second change, put a Contact Tool into the Connections folder and Generate Initial Contact Results.
All the contacts are Closed, so now I tried to Solve, but I got that same error. The next step is to add a Modal analysis to find the loose part.
Drag the Fixed Support from the Static Structural branch and Drop it on the Modal branch.
Solve the Modal system and plot the Total Deformation. It shows one loose part.
Add contacts for the loose body, then the Static Structural model will solve (and the Modal will have a non-zero frequency for the first mode).
Now you can delete the Modal analysis, it did its job.
A bonus tip: the default mesh looked like this:
I added a Multizone method to the two lower angle brackets and they came out as shown in the Deformation contour plot.
October 27, 2018 at 5:23 pmsameerfaresSubscriber
Thank you so much Peter!
i need to understand on my own if i can what each step you performed does or mean. i 'd like to ask you more questions as i try to grasp your steps.
Could you send both files the one with modal analysis and the one after you removed the modal analysis?
October 27, 2018 at 5:44 pmpeteroznewmanSubscriber
Here is the 19.2 archive with the Modal analysis. You can delete the Modal whenever you want.
October 27, 2018 at 9:39 pmsameerfaresSubscriber
Thank you Peter!
October 29, 2018 at 2:10 am
October 29, 2018 at 2:50 ampeteroznewmanSubscriber
Restart your computer, download to a new folder, rename the download to temp.wbpz and try Restore Archive again.
I was successful opening the file attached to my last post.
October 29, 2018 at 8:13 pmsameerfaresSubscriber
Thank you Peter! It worked.
1. How does Modal analysis find the loose part? or what is it about the modal analysis that fined the loose part?
2. You stated to " Setting Proximity to Yes and Num Cells Across Gap to 2". What does that do or mean? Why isn't the program default to these? Are there condition where this setting is not right?
3.Do you always add a Multizone method? what does Multizone method do?
October 29, 2018 at 9:41 pmsameerfaresSubscriber
1. Below you added Multiple to Multiple bonded contact. 2 bodies with 5 faces. I can see each fillet weld can be welded to two faces for a total of 4 faces.One face is the thickness of slotted angle and the other face is the vertical plate of top chord angle. could you tell me what is the fifth face?
2. Is there a difference between Bonded contact and shared topology?
October 31, 2018 at 12:45 ampeteroznewmanSubscriber
Modal analysis can be done for parts that are not fixed to ground, like rockets and planes. Static Structural requires a connection to ground or it won't solve. Therefore, you can use Modal analysis to find loose parts.
Proximity = Yes means the meshing software will look at faces that are near each other. Num cells across gap means when two faces are near each other and there is a gap between them, the mesher will put two elements across that gap. This is only useful sometimes, like when you have thin walled parts, so is not the default.
If you mesh without Multizone, you will get a Tetrahedral mesh that will take about twice as many elements to fill the volume than would be required if you use Multizone, which breaks the volume up into sweepable pieces and meshes them with hex elements. Multizone doesn't always work. When it fails, you can either use Tetrahedral elements or spend a lot of time manually slicing up the geometry into sweepable pieces.
I picked all four faces of the slot, plus the face of the other angle bracket to get 5 faces on one side of the contact. I could have picked just 3 faces to get what was needed, but the faces that were needed were behind the weld bodies and there is an icon on the toolbar called Extend to All which lets me pick the cylindrical face, click that button to get the other three, then Ctrl-click the last face.
Bonded contact and Shared Topology have similar outcomes.
October 31, 2018 at 9:21 amsameerfaresSubscriber
Big thanks to you Peter!
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- How to calculate the residual stress on a coating by Vickers indentation?
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.