March 31, 2022 at 8:17 amjp_jasonSubscriber
as part of a project, I have built a blade from fiber composite with Ansys-ACP. To perform an evaluation of the model results I need to calculate the deformation of the points at the leading edge and trailing edge at the blade tip (see picture). By creating a named selection and assigning the desired point using geometry selection, the picture in the appendix is obtained. So far so good.
By doing a parametric study and varying the orientation of the laminates of the composite blade, I would like to investigate the effect on the deformation at the two points at different laminate orientations. However, a change of the orientation of a laminate in ACP leads to the fact that in ANSYS-Mechanical the Named Selection of the point is no longer recognized and consequently automatically suppressed.
Am I missing something? How can the problem be solved or bypassed?
Any help is appreciated!
Thanks in advance.
JayMarch 31, 2022 at 2:57 pmAshish KhemkaAnsys Employee
Please see if the following link is of use to you:
Orientation of the layer application for curved surfaces in acp (pre) ÔÇö Ansys Learning Forum
Regards Ashish Khemka
April 5, 2022 at 10:42 amjp_jasonSubscriber
thanks for the quick response. I read the linked thread but unfortunately this is not what I am looking for. Maybe I didn't describe my problem in an understandable way.
I want to do a parametric study on a fiber composite blade. In the parametric study the orientation of the laminates is changed. The objective is to study the influence of the orientation of different laminates on the torsional part of the first vibration mode of the blade. Thus, after ACP-Pre, a Stractrural-Analysis and a Modal Analysis follow (see picture bellow).
To calculate the torsional part I need the deformation of the blade tip once at the leading edge (A) and once at the trailing edge (B) (see picture bellow).With a defined layup I can define a named selection in Ansys-Mechanical at the two desired points. However, this is not possible for a parametric study. The named selection is suppressed when the orientation of the layup is changed.Consequently, I do not get the torsion part as output for different laminates in the parametric study.
I hope this could better describe my problem.
I am looking forward for your answer.
April 11, 2022 at 12:58 pmjp_jasonSubscriberHey is there any idea?
April 11, 2022 at 4:37 pmAshish KhemkaAnsys Employee
I have no comments for now. I am waiting if someone else can comment more on this query.
Regards Ashish Khemka
April 11, 2022 at 5:45 pmSean HarveyAnsys Employee
When you define the named selection for the point, you are using vertex, not node, right? Now if that is the case, maybe you are using solid composite and not shell? When solid composites are passed, the geometry is synthesized and we need to take additional steps to get name selections to persist. Can you confirm if it is a solid composite?
April 12, 2022 at 2:22 pmjp_jasonSubscriber
still thanks for your response.
like suspected I am using a vertex for the point and I can confirm it is a solid composite. What are the additional steps to get a name selection to persist?
I have found a possible solution: You can define in ACP-Setup two nodes at the leading edge and trailing edge of the blade tip as edge sets. This is transferred to ANSYS-Mechanical as a Named Selection that persist (if you don t change the mesh), but only as a surface. By the deformation of the generated surfaces the result can be approximated. Is there another way?
April 12, 2022 at 5:40 pmSean HarveyAnsys EmployeeSo here is what you do. You create an edge name selection in the base mechanical system. Then this will go to ACP as normal, when the solid is created, that edge turns into a face in the extrusion process. This you already know. The key is then insert another named selection, but change the scoping method to worksheet. You can then add rows to the worksheet to convert the face to edges, then to vertrices, then filter based on spatial location. You can hopefully see in the screen shot the details of the worksheet. In the end I have 1 vertex that will persist.
Please try and let us know. If the screenshot is not clear enough, please also let us know.
April 14, 2022 at 9:04 amjp_jasonSubscriber
I tried your method and it s working perfectly. Thanks a lot for the help!
April 14, 2022 at 7:48 pmSean HarveyAnsys Employee
That is what I love to hear. You are welcome!
Viewing 9 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
Ansys BlogTrending discussions
- ANSYS Workbench Measuring within Design
- Conformal vs Non-Conformal Mesh
- Error in meshing
- Meshing Error
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Ansys 19.0 – will not create mesh
- Dealing with inflation layers around sharp corners in Ansys workbench meshing
- How to resolve Mesh Failure
- Can I view which mesh files (the names of them) are loaded into Fluent?
- Mesh Generation Taking a Long Time
Top Rated Tags