April 1, 2020 at 1:57 pmJSmithSubscriber
Hello. I am having an issue with getting ANSYS Mechanical ADPL to create a linear mesh. I have created a 5 cm long extracted beam in SpaceClaim and imported it into Mechanical ADPL using Workbench. I have changed the mesh settings to have a Linear Element Order and large size to get 1 element. However, when I mesh, the statistics show 1 element and 3 nodes. When I add the node numbers I only see 2 nodes, but the program will run as a quadratic element. I've tried to restart and run the model again, and I get the same results. I am unsure what needs to be changed in the program to get the correct number of nodes. Any assistance that you can provide would be greatly appreciated.
April 1, 2020 at 1:58 pmJSmithSubscriber
Additional note: I have tried changing to a truss element as well and get the same node error. I will get linear results then, but I would like to still understand why there are 3 nodes instead of 2.
April 1, 2020 at 3:21 pmpeteroznewmanSubscriber
What evidence do you have that a model with a Linear mesh will run as a Quadratic element?
Is it because you see an extra node in the mesh Statistics as shown below?
That doesn't imply the element runs as quadratic. After this model solves, I can look in the Solution output and see that one linear element BEAM188 was used.
If I change to a Quadratic mesh...
then I get one Quadratic BEAM189 element in the Solution output.
You might ask, "Why is there an extra node?" I expect it is used to orient the beam cross-section.
If this post answers your question, please click the Is Solution link below (when logged in) to mark this discussion Solved.
April 1, 2020 at 7:14 pmJSmithSubscriber
I know that it is running as quadratic due to the results. I am comparing to a known solution from custom software to the output of ANSYS. The linear choice in ANSYS gives a quadratic solution. And the quadratic choice gives a cubic solution. I think it is associated with the additional node.
April 1, 2020 at 10:40 pmpeteroznewmanSubscriber
The terminology used by ANSYS and every other Finite Element program is that a linear beam element has two nodes with a quadratic displacement function, while a quadratic beam element has three nodes and a cubic displacement function.
Two nodes can deliver quadratic displacements because each node has rotation degrees of freedom as well as translation degrees of freedom.
The benefit of a quadratic beam element is that it can represent curved geometry, while a linear beam element can only represent geometry that is initially straight.
You seem to be looking for a two node element that has a linear displacement function. That is called a truss element, which NASTRAN calls a ROD and ANSYS calls a Link Element, or LINK180. That has only translation degrees of freedom and no rotation degrees of freedom, so the displacement function is linear. In the Details of the Line body under Geometry, you can change a Beam to a Link.
April 2, 2020 at 1:56 pmJSmithSubscriber
Thanks for that assistance. One last question. Where do I find this third node? It appears for both the beam and the link element. Thanks!
April 2, 2020 at 6:57 pmpeteroznewmanSubscriber
When you click on the Solution branch in Mechanical, you can Write Input File. I attached an example text file. It is listed in there. I don't know how you find it graphically in Workbench. I expect you can see it graphically in the Mechanical APDL program.
If your question is answered, please click the link below the post that best answered it to mark this discussion Solved.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- ANSYS Workbench Measuring within Design
- How to resolve Mesh Failure
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- Ansys 19.0 – will not create mesh
- Dealing with inflation layers around sharp corners in Ansys workbench meshing
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
© 2022 Copyright ANSYS, Inc. All rights reserved.