July 23, 2018 at 12:46 pmmaethaSubscriber
I'm trying to model the attached geometry. My goal is to simulate the falling rock onto the structure. In a first setup I'd like to build a model which is working in static structural environment and after that with the explicit dynamic module.
I'm having problems with the connections between the different profiles (HE, UP, IP). Is there a way to "fix" them together, as they would be one structural system? I already tried contacts between areas, which seems not to work with explicit dynamics and share topology. Latter didn't make any difference.
I'm using ANSYS 18.1.
Thanks a lot!
July 23, 2018 at 1:40 pmSandeep MedikondaAnsys Employee
I am unable to open the model due to various reasons. Can you post some snapshots of the model, tree and the details windows?
Have you tried using bonded contact? I am surprised that share topology didn't work. Did it work in on analysis system and not the other?
Another option you would have is to use mesh connections.
July 23, 2018 at 2:00 pm
July 23, 2018 at 2:46 pmSandeep MedikondaAnsys Employee
Are you using SpaceClaim? If so, Can you use the 'Show Contact' tool to look and make sure that the edges are being shared? Make sure to change Share Topology to 'Share' in the properties window.
Even in mechanical, you can check this by turning on 'Edge Coloring' > 'By Connection'. This will allow you to see if the edges are being shared between components.
July 23, 2018 at 4:47 pm
July 23, 2018 at 5:41 pmSandeep MedikondaAnsys Employee
Here is the video on using share topology in Design Modeler.
Now, it looks like share topology is working here and the penetration you are seeing is because you are working with shell structures. So this is merely for visualization purposes. You can turn this off in Mechanical using View> Thick Shells and Beams.
Coming to your error, are you able to post snapshots of your error message, you analysis settings, boundary conditions/contacts etc. so that we can debug?
July 23, 2018 at 6:23 pm
July 23, 2018 at 7:00 pmSandeep MedikondaAnsys Employee
How far into the simulation does the model fail? Can you provide one more snapshot of your Force Convergence (In solution output change from solver out to force convergence)? Here is a very useful article on Convergence, may be looking at the newton-raphson residuals will help. Also, increase the number of sub-steps in your model?
July 23, 2018 at 7:06 pmpeteroznewmanSubscriber
One way to connect those profiles is to use an Automatic Node Merge. I used a 7 mm Tolerance Value and turned on Face/Face.
This is the result:
Note that one of the profiles didn't get any nodes merged at the 7 mm setting, and some of the elements are getting distorted during the merge.
A much better way is to create a Named Selection of all the faces of the U-channels on the top and second Named Selection of all the faces of the I-beams that they rest on and make a Contact Definition between two Named Selections. When I did that, I found that some face normals are not in the same direction as their neighbors, so that needs to be accommodated to use this method.
I suppressed your line bodies. I suppressed Fixierte Lagerung. I changed your springs from Body-Body to Body-Ground, I suppressed Körperwechselwirkung (Body Interactions) since you don't want extra complexity during the first attempt to solve.
Hope this helps. I don't have 18.1 available at this time, I was doing this in 18.2.
July 25, 2018 at 5:36 pmmaethaSubscriber
Dear Sandeep and Peter
thank you very much for your answers!
@Sandeep: The model fails quite in the last part of solving. Nevertheless the force convergence shows no entry.
@Peter: I've now created those two named selections and made a contact definition between them. Furthermore I suppressed the same as you did. Unfortunately I still get the same error message. I've also created a third named selection for the lower I-profiles and connected them to the middle H-profiles, which didn't make any difference.
What else could it be?
Thank you both!
July 25, 2018 at 9:04 pmpeteroznewmanSubscriber
In DesignModeler, I picked all the bodies in Oberbau and set the Shared Topology Method to Automatic.
I changed your groups to have 11 faces in UPE and 14 faces in HEA, the faces that touch each other, not the faces away from that plane.
I changed your IPE to have 4 faces and created HEA2IPE with the 14 faces on the other flange of the I-beam.
I updated the two contacts to use these two pairs of named selections and set them to use MPC contact, which is easy to visualize in the results, set the shell sides, and set a manual pinball radius. I don't know if those settings were necessary.
I added a contact tool to show that the contacts were were closed.
I changed it to solve with Auto Time Stepping On and set the initial substeps to 10.
I added a Modal to make sure all the parts were attached.
Now the Static Structural model solves (at least to 20% of the full load).
Attached is an ANSYS 18.1 archive.
July 26, 2018 at 3:43 pmmaethaSubscriber
Thank you very much!
As I tried to start solving with the explicit dynamics mechanical crashes with AnsysWBU.exe not working. Is there a way to analyze the .dmp file?
July 26, 2018 at 9:59 pmpeteroznewmanSubscriber
I don't know how to use a .dmp file. I recommend you try Transient Dynamics for the impact of the rock with the grate.
What is the impact velocity you have chosen for the rock? You should move the rock in DM to be in initial contact with the grate.
What plasticity model would you chose for the metal?
I recommend you start a New Discussion in the Structural Mechanics area to ask new questions about the impact of the rock because this topic could be marked as solved.
You can show your appreciation by clicking Like below the posts that are helpful.
July 27, 2018 at 6:57 ammaethaSubscriber
The impact velocity is around 20 m/s. I'll use the bilinear isotropic hardening model.
- You must be logged in to reply to this topic.
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
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- 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.