June 26, 2019 at 1:48 pmAnnaYangSubscriber
I was trying to solve a steady-state thermal deformation problem in ANSYS Workbench 17.2.
I solved the steady-state temperature field in Steady-State Thermal and tried to solve the thermal deformation in Static Structural.
The geometry and engineering data are shared, and the solution of Steady-State Thermal will be imported to the setup of Static Structural.
There are 13 solid parts and 1 fluid part in the geometry, and the temperature field can be solved and imported to Static Structural as thermal loads.
However, when I tried to solve the deformation in Static Structural, there's always an error:
"An Internal Solution Magnitude Limit Was Exceeded. Please check your Environment for inappropriate load values or insufficient supports."
Here is the setting in Static Structural:
1. Imported Load - Imported body temperature. (Min: 25.106 ; Max: 36.556)
2. Fixed Support or 0 displacement in gravity direction on the bottom face of the whole structure. (Both had been tried)
Please give me some suggestions, thank you!
1. The geometry includes 13 solid parts and 1 suppressed fluid part.
Since the Elasticity property is needed in Static Structural, the fluid part is suppressed.
2. The contact regions, no. 3, 6, 9, 13, 14, 16 and 18 revolve to fluid part, also suppressed.
3. Fixed Support at bottom face.
4. Imported Load - imported body temperature
the source bodies is set by manual way, only import the temperature of solid parts. (1-13)
June 26, 2019 at 2:03 pmjj77Subscriber
I would follow the advice the solver gives and check that you sufficient support (e.g., fixed support) so parts do not "fly" away. Also make sure there is contact in between parts.
Also static is a solid structural solver not a cfd solver, so not sure what fluid you have
If you post some images of the set up/contacts/supports/..., then someone can see and tell you more.
June 26, 2019 at 2:18 pmAnnaYangSubscriber
Thank you for replying.
I have set fixed support to try to avoid the "fly" problem, but the error still popped up.
And yes, the fluid part was suppressed at the step of "model" in the Static Structural, it's the reason that model didn't shared.
Thus, all the contacts revolve the fluid region have been suppressed, too.
A test simulation which has a relative simple geometry ( 3 thin Plates : Solid -- Fluid -- Solid ) was done to make sure the suppression won't be a problem.
I will add some images later as you suggested, thank you!
June 26, 2019 at 2:49 pmjj77Subscriber
It looks like something is not connected, I would try using inertia relief with small displacement (large deflections off), and then you can see which parts are not connected. Also do a modal analysis on this part as it is with the contact set up you have (without temp. loads), and if you see some 0 Hz modes indicating rigid body movement, and that will tell you what is not supported or connected well..
June 27, 2019 at 7:13 amAnnaYangSubscriber
I tried turn on the inertia relief with remote displacement (Y component = 10 mm), and run the model without temperature loads all last night. However, the solution took much more time solving and the error popped out again.
Since it was the first time to use the remote displacement method, I was wondering if the setup was wrong.
Here's the setup:
1. Fixed support at bottom part.
2. remote displacement (Y component = 10 mm) at another small face (circled with red line) which perpendicular to Y direction.
3. inertia relief turned on.
June 27, 2019 at 7:48 amjj77Subscriber
I would remove that extra remote displacement and as I said run it in modal analysis with the exact set up, so all contacts you have active and the fixed support and see how it behaves. If there are rigid body modes (0 Hz) that will tell you if something is not connected or supported properly.
June 27, 2019 at 9:06 amAnnaYangSubscriber
Thank you very much. The modal analysis was conducted and it's like you said that there indeed was one part which was not connected properly!
But there was something I don't understand that only the 0 Hz mode I should put my attention to since all the 6 modes are very small ?
And the part didn't get connection well is the rotor of a drive motor, so it should be grab by the stator with magnetic force in the reality.
How to put a non-contact connection between the rotor and stator in the model ?
June 27, 2019 at 9:25 amjj77Subscriber
We get 6 rigid body modes for each mode so to say (since we have 6 dof). SO the rest ones could be the same rotor moving, or rotating most likely in a rigid body rotation.
Not sure how the machine is build up, but I assume the rotor is supported and fixed somehow by bearings and the ends of it, and the stator must be also fixed/connected in the casing somehow so you need to provide these supports or contacts between the parts.
At least now you know which parts are not connected/supported well.
June 27, 2019 at 9:33 amAnnaYangSubscriber
A hydrostatic bearing is adopted in this machine, so the bearing is the oil film (fluid part which is suppressed in solid solver).
And yes, there are other parts to fix the spindle, I will check the rest contacts between these parts and try the Static Structural again after that.
Thank you for your suggestions, they are very helpful!
- 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.
- 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
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.