May 4, 2021 at 8:57 amamit.pandeySubscriber
I am trying to setup a static structural simulation to test the behavior of a lens system with temperature change.
The lens system is held in an Aluminum outer body (lets call it barrel), shown in the Figure attached. This outer body is clamped on an Aluminum plate which is heated up, and in turn heats the lens system.
I know the forces that I want the clamp put on the barrel rim, so that can be set up a force boundary condition (BC) in the downward direction.
I am confused between the other boundary condition. The lower part of the rim is in contact with the aluminum heating plate and my earlier thought was to put a zero displacement BC in the vertical direction but the system will expand in the vertical direction which makes zero displacement BC not applicable.
Can anyone suggest if there is something that I can do to correctly represent the system as it is in the Figure?
Should a contact condition between the heating plate and the barrel be sufficient to represent the system?
Also, I am only using the barrel (with lenses and spacers) in my simulation. The heating plate and clamps are not included in the simulation. The idea is to represent them by BCs.
The lenses and spacers inside the barrel are not shown.May 6, 2021 at 6:34 am1shanAnsys EmployeeAre you doing a coupled thermal-structural analysis? If so you could define a bonded contact between the barrel and base plate, then fix the bottom surface of the base plate. This way the plate will expand pushing the barrel against the clamp. Regarding modelling of the clamps you could use different loads depending on the desired accuracy. The best way would be to assemble the clamps and define contacts between then. You could also use a ground body springs , where the body end is scoped to the barrel. You could insert a clamping force directly but note that it would not change (should ideally increase as the barrel expands and pushes against the clamps).
May 6, 2021 at 7:34 amamit.pandeySubscriber
Thank you for your response.
I am doing a static structural simulation with a thermal condition where I increase the temperature of the barrel from 25 to 90┬░C. My goals are to see the deformation in the lenses inside and evaluate the distance the lenses are displaced. I guess this could be called as a thermal-structural simulation.
The idea was to exclude the base plate from the simulation. I only simulate the barrel with the lenses and spacers inside.
What would you suggest if I don't want to include the plate?
Best regards Amit
May 6, 2021 at 12:23 pmpeteroznewmanSubscriberThermo-elastic structural simulations is one of my favorite topics! You don't need the plate or the clamps in the model.
I expect the barrel and lenses are all axisymmetric bodies, therefore an axisymmetric model is ideal for your simulation. In CAD, orient the optical axis along the global Y axis, and put the flat mounting surface of the barrel on the XZ plane. Use the XY plane to cut the solids and delete the pieces in +Z. Use the YZ plane to cut the solids and delete the pieces in -X. Now you have a 1/4 model with a set of faces in the XY plane. Copy those faces and paste them in as surfaces. This is easily done in SpaceClaim. Delete the solids. Now you have surface bodies in the XY plane on the +X side of the Y axis. If you were to revolve those surfaces, you would get back the original solids.
Start a new Static Structural model, do not reuse your current model, but you can link the Engineering Data cell from your first model. In Workbench, right click on the Geometry cell and in the Properties window on the right, change the Analysis Type to 2D and import the file with the 2D surfaces. Now open the Model and the geometry will import. In Mechanical, click on the Geometry branch of the Outline. There is a place in the Details window to set the type of 2D analysis. Select Axisymmetric. Now you are ready to define the rest of the model.
Pick the mounting edge of the barrel, and set a displacement of Y=0. That grounds the barrel, but leaves it free to expand radially along the X axis. Define frictional contact at the interface of the barrel and the first optical surface. Define another frictional contact of the first spacer and the second optical surface. Continue creating contacts: the first spacer and the third optical surface and so on. I expect the last spacer screws into the barrel to clamp the stack of lenses. Use bonded contact between the last spacer and the barrel.
Now you have an assembly that can have a temperature load applied and look in detail at the deformation of each optical surface relative to the bottom surface of the barrel. You must of course have the CTE defined for each material and the reference temperature of each material set to 25C and the Environment temperature of the model set to 25C so that there is zero strain at 25C and then you will see the effect when you apply a Thermal load of 90C.
May 6, 2021 at 1:35 pmamit.pandeySubscriberEDIT: Fixed the issue by moving the geometry to z = 0
I tried to transform the 3D CAD to surface CAD in SpaceClaim as suggested.
However, when I try to import the geometry, I get an error which is shown in the image attached..
Am I doing something wrong? Please suggest what i can do to avoid this error.
May 6, 2021 at 2:49 pmamit.pandeySubscriber
I finally got to the end where I was ready to run the simulation but I get errors:
Temperature BC was set to change from 25 to 90┬░C . I also tried with larger step end time but I get the same error.
After the first errors I changed the Newton Raphson option to Unsymmetric
The Contact friction are as follows:
I can't seem to be able to run the simulations. Could you please suggest what needs to be rectified?
May 6, 2021 at 3:43 pmpeteroznewmanSubscriberAnytime frictional contact is used, you must insert a Contact Tool under the Connections folder and generate the initial contact status. Check that all the contacts are closed on the worksheet. Any that are not closed but have tiny gaps, like 1e-3 sized gaps, those can be closed by editing the contact and setting the interface treatment to Adjust to Touch.
The other thing to do with frictional contact is under Analysis Setting, turn on Auto Time Stepping and set the Initial Substeps to 100, Minimum to 1 and Maximum to 1000.
If you have problems after that, please do File, Archive to create a .wbpz file. That can be attached to your reply and state the version of Ansys you are using.
If you can't share the file, at least post an image of the lens barrel cross-section that you have created.
May 7, 2021 at 8:49 amamit.pandeySubscriber
I tried to rectify the contact gaps with the adjust to touch method.
I also generated the "initial information" for the frictional contacts. Also changed the substeps as suggested.
With these corrections I was able to run the simulation and it looks good. All I need to do is validate the results with some experiments.
Thank you for the suggestions.
Quick question though, regarding the same simulation:
If I want to run a 3D simulation with the same BCs (solely because I have a tool that can take the deformed mesh information and import it to my Optical Simulation software and check the change in performance of the lens based on the FE data) could you please suggest a way to set up the 3D simulation? I would be really grateful.
Best regards Amit
May 7, 2021 at 11:00 ampeteroznewmanSubscriberGlad to hear the simulation converged.
You don't want to make a 3D simulation because you will lose the symmetry boundary condition that you got for free in the axisymmetric model, and that missing BC might give problems with convergence in 3D.
You don't need to make a 3D simulation. Simply export two directional deformation results, one for X and one for Y, as text files. Those will come with the nodal X, Y coordinates as well as the deformation for each node in X and Y. Convert that 2D radial set of points into a 3D cloud of points by rotating the points in 15 degree increments about the Y axis. You should be able to import that into your optical simulation software.
Please reply with the name of the Optical Simulation software you are using.
If you can insert an image of the lens assembly cross-section, that would be appreciated.
May 7, 2021 at 12:13 pmMay 10, 2022 at 7:08 amamit.pandeySubscriberHello Peter
I am running a similar simulation but this time, I cannot run an axisymmetric model because I need the deformed mesh to later fit a surface with SIGFIT and run optical analysis using ZEMAX.
I am still worries about the zero displacement constraints on the model. Do you think it is the right way to apply that on the bottom surface of the flange on the barrel without modeling the heating plate at all?
All in all I have two loads, 1. force from the clamps on the top surface of the flange and 2. temperature change from 25 to 90┬░C and just one constraint that I expect to prevent rigid body motion.
Best regards Amit
May 10, 2022 at 10:37 ampeteroznewmanSubscriberUse a Remote Displacement, Behavior = Deformable on the bottom face of the barrel and set all six DOF to 0. That will hold the center of that face fixed, preventing rigid body motion, without adding any stiffness and allow the barrel to freely expand.
Viewing 11 reply threads
Ansys Innovation Space
- 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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- 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
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.