January 8, 2019 at 2:38 pmliamjstrachanSubscriber
Below is my model of a compression test to measure residual stress in a thermally sprayed disc specimen. I am looking to produce stress vs distance graphs at the interface of the coating and substrate to show the mismatch in stress.
However, I am not entirely sure how to measure the stress on the coating and substrate interfaces, since the two parts are connected together.
Anybody got a solution?
Thanks in advance.
January 8, 2019 at 2:43 pmSandeep MedikondaAnsys Employee
Under the scoping method, instead of All Bodies, why not select just the surface and evaluate those results? You can insert 2 results for the 2 contacting surfaces and that way you can see the difference.
Guidelines on the Student Community
January 8, 2019 at 2:59 pmliamjstrachanSubscriber
Okay I see, however I cannot select the contacting surface of each component, that is my problem.
Apologies for the lack of understanding, I have only been using ANSYS for a short period of time.
January 8, 2019 at 4:32 pmpeteroznewmanSubscriber
You have a multibody part. The first item under Geometry that says Part is where the disk substrate and coating solids can be found. Those two solids share a common face. This is called Shared Topology. It means that no contact is needed under the Connections folder to hold the coating to the substrate.
When you have a multibody part, you can't plot the stress on the shared face.
You can plot the stress on each body separately, the coating and the substrate.
There is a different way to build this model, that is without Shared Topology and using Bonded Contact to hold the two faces together.
In DesignModeler, you Explode the Part to get two separate bodies that don't share a face.
In Mechanical, you need to have a Contact that Bonds the two faces together. Then you can plot the stress on each face separately.
January 8, 2019 at 7:06 pmliamjstrachanSubscriber
January 8, 2019 at 7:38 pmpeteroznewmanSubscriber
In Mechanical, RMB on Model and Insert > Construction Geometry
RMB on Construction Geometry and Insert > Path
Fill out the Details on the Path you just created.
You can Click on each face to fill out the coordinates of the centroid.
The default number of points to sample is 47. You might want more, I typed 100.
Insert a Stress result into the Solution branch and select Path instead of Geometry.
You will get the tabular data and a graph with 100 points.
The length is the true distance from point 1 to point 2. In my case, I had a 10 mm thick substrate and a 1 mm thick coating.
You can take the tabular data into Excel and normalize the distance.
If this answers your question, please click the Is Solution link below or reply with a follow-up question.
- 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.
- How to calculate the residual stress on a coating by Vickers indentation?
- Errors – Reinforced Concrete Beam
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Large deflection
- Colors and Mesh Display