April 13, 2023 at 9:39 ambiao.zhouSubscriber
I know that in ANSYS, if I select the current coordinate system as the cylindrical coordinate system (csys,1), then x represents r, y represents r*Δθ, which is the distance along the circumference, and z is consistent with the Cartesian coordinate system. However, when I process my modal shape results in the post-processor (/post1), I still encounter difficulties in understanding.
I tried to perform a modal analysis on a compressor's bladed disk and extract its mode shapes. The modal analysis is based on a single-sector model with cyclic symmetry settings.
As shown in the figure below, when I predefine the global coordinate system as the global cylindrical coordinate system (csys,1) and specify the result coordinate system in /post1 to also use the solution coordinate system (rsys,solu), I extract the modal shape data of a single sector. The value of y (which is rθ) is very large. When I divide y by x to obtain the θ value in the cylindrical coordinate system, it still exceeds the range of (-π,π), which confuses me.
When I extract the mode shapes of the entire disk, the value of y is still very large, indicating that the error is not caused by extracting the mode shapes of a single sector.
I would like to know what such a large y value represents, whether the θ it reflects is truly usable, or if I need to do some processing to make it usable. (Please note that I used the PRNSOL command to display the mode shapes, and GPT-4 told me that the mode shapes extracted using this command have not been scaled, i.e., they are the original mode shape data.)
April 13, 2023 at 2:41 pmChandra SekaranAnsys Employee
I know that in ANSYS, if I select the current coordinate system as the cylindrical coordinate system (csys,1), then x represents r, y represents r*Δθ, which is the distance along the circumference, and z is consistent with the Cartesian coordinate system.
In a cylindrical coordinate system the X represents radius, Y represents angle in degrees (not distance), and Z represents axial location.
April 14, 2023 at 1:35 pmbiao.zhouSubscriber
First of all, thank you very much for your answer.
You believe that the Y in the cylindrical coordinate system does not represent the circumferential displacement but the angle. However, I found this statement in the ANSYS help documentation, which states that when specifying the result coordinate system as a cylindrical coordinate system using RSYS,1, UY represents the tangential displacement.
April 14, 2023 at 1:26 ammjmiddleAnsys Employee
Using cylindrical coordinate systems can be confusing, or any CS that has an angular axis, for that matter. The main reason is that all elements and nodes in APDL have Cartesian CS. So while you can specify preprocessing values (CSYS) using a cylindrical CS, you can never really retrieve results (RSYS) in a cylindrical coordinate system. In either case it is using pseudo cylindrical CS. It rotates element or nodal coordinate systems (Cartesian CSs) to be aligned with local cylindrical directions at every element centroid or node. In the case or preprocessing (loads/constraints), those directions may only agree at the start of the analysis if any angular loading or deformation occurs throughout the analysis. Refer to the Ansys help section (https://ansyshelp.ansys.com/): //Mechanical APDL// Basic Analysis Guide // 7. The General Postprocessor (POST1) // 7.3. Additional POST1 Postprocessing
Radial or Z displacements alone will not cause a problem with results in cylindrical CS and are easy to interpret. When angular displacements occur (by loading or deformation), then both cylindrical X and Y will be hard to interpret and my not be very useful to report in cylindrical CS.
For reporting results in a true cylindrical CS, I find it best to use a a Cartesian RSYS where x,y coordinates are in the plane of r,theta. Then convert for each node. Assuming UPCOORD was not done:
UR = sqrt((NX(Id)+UX(Id))**2 + (NY(Id)+UY(Id))**2) – sqrt(NX(Id)**2 + NY(Id)**2)
Use atan2(y,x) to get cylindrical angle (same as tan(y/x), except it accounts for angle quadrants due to signs of x and y).
UTheta = atan2(NY(Id)+UY(Id), NX(Id)+UX(Id)) - atan2(NY(Id), NX(Id))
April 14, 2023 at 1:29 pmbiao.zhouSubscriber
First of all, thank you very much for your answers.
In my analysis, I specified the global cylindrical coordinate system as my solution coordinate system and nodal coordinate system from the beginning. In post-processing, I also used this coordinate system. Even so, are the results I extracted still not the real global cylindrical coordinate system?
I am very interested in your idea that the cylindrical coordinate system specified by RSYS is actually the local cylindrical coordinate system of each node. Can you provide the source of this statement? I didn't find this statement in the help documentation.
You finally shared how to obtain data in the real cylindrical coordinate system. You think I should extract data in the Cartesian coordinate system through RSYS,1 and finally convert it through formulas. I will give it a try.
If you can tell me more about the inherent problems of the cylindrical coordinate system in ANSYS and how to extract data, it would be of great help to me.
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.