May 24, 2022 at 1:08 pmjavat33489SubscriberHi guys. I have a circuit of 4 gears.
Three red gears rotate the black one in the middle
How to set joints correctly?
I can't get everything to rotate.
For each circle, I set the body-ground rotation to rtevolute.
Between myself, I connected each red with black (3 joint) as body-body - revolute. I also tried to set planar for them but then only two shafts rotate.
Help me please.
How to make a connection so that everyone rotates each other?
Or what's right?
May 24, 2022 at 10:29 pmpeteroznewmanSubscriberWhat output do you want from the simulation?
May 25, 2022 at 3:14 pmjavat33489Subscriber
May 25, 2022 at 9:29 pmpeteroznewmanSubscriberOne way to evaluate stress in the teeth does not require all gears to rotate. If the red gears all have the same torque load, the center black gear gets a revolute joint while the three red gears are held fixed at the hub. A Joint Load of Torque is put on the Revolute Joint. Frictional Contact is created between the gear teeth that are touching. This is done in a Static Structural analysis.
If the red gears each have a different torque, then you mostly care about the highest torque load. You can fix the hub of the center black gear and put a revolute joint on the high torque red gear and apply a joint load of torque on that one red gear. It will have the largest stress.
Here are some examples of spur gear tooth stress analysis.
May 26, 2022 at 6:25 pmjavat33489SubscriberYes you are right.
It is enough to leave only two shafts.
I have a paradox. When I set the rotation to 360 degrees, the two shafts only rotate 180 degrees. All body rigid:
If I set 720 degrees they make one revolution.
But if I add a shaft to the wheel, then the shaft slows down and the wheels spin in place:
I made animations (see above) but they don't work on the site
attached them as files:
May 26, 2022 at 6:31 pmpeteroznewmanSubscriberWhat is your purpose in rotating the gears? I thought your goal was to evaluate stress in the teeth. You don't need more than a few degrees of rotation on one gear to load up the torque and evaluate the tooth stress. The other gear hub is fixed.
May 27, 2022 at 4:03 pmjavat33489SubscriberI don't have many tasks. I need to rotate the gears to see what happens to the shaft that is attached to one gear. I will look at different loads, including on the gears. I need to figure out why this strange rotation is happening. Suspicion that revolute does not work between gears but planar works - I put it
May 28, 2022 at 5:12 pmpeteroznewmanSubscriberThe GIFs you attached don't show any animation.
The gear teeth don't look like the have the correct shape to transmit motion smoothly.
What helps to have a simulation run is a torque load on the shafts that are being driven by a rotational input.
You haven't said if you are using a Static Structural analysis or a Transient Structural analysis.
In Workbench, use File, Archive to save a .wbpz file and attach that to your reply (not the .wbpj file!).
Then I can take a look at that tomorrow.
May 29, 2022 at 7:10 pmjavat33489SubscriberI am using transient structural
May 30, 2022 at 12:57 ampeteroznewmanSubscriberThe gear teeth should be tangent to each other to begin the simulation. I opened the Geometry in SpaceClaim and moved one gear tooth face to be tangent to another tooth face.
There should be a moment on one gear to push the teeth together. The other gear needs a rotation defined to rotate the gears. ANSYS 2022 R1 archive attached.
May 30, 2022 at 6:54 pmjavat33489SubscriberThank you very much for viewing my project. I will look it up and write today
May 31, 2022 at 2:57 pmjavat33489SubscriberThanks a lot. I looked at your solution.
But it still doesn't work.
I need a torque of 24Nm = 0.024 Nmm, under this condition the wheel turns as before in my solution.
I attach animation
I also have questions:
1. What is 36*time in joint rotation?
2. How did you manage to use contacts and mesh on rigid bodies? Usually this doesn't work.
May 31, 2022 at 6:28 pmpeteroznewmanSubscriber36*time is the equation for the rotation angle of the joint. At 1 second, the joint will have rotated 36 degrees.
You can make Frictional Contact with rigid bodies.
The geometry you have shows multiple faces on the gear teeth and there are steps in the surfaces. This is not good. You should improve the geometry.
I have shown a working simulation with a larger torque. If you use a smaller torque, you may need to make other adjustments in the simulation. Nonlinear convergence is not easy to achieve so expect to spend some time tweaking the model to get it to converge. You may need smaller time increments or smaller elements. Adding some damping to the joint with the moment applied may help. You may find a smoother motion profile if you ramp a rotational velocity up from zero rather than a rotation. It may help if one of the gears becomes flexible instead of a rigid-rigid contact with two joints, the whole structure is extremely stiff which makes convergence more difficult.
May 31, 2022 at 7:19 pmjavat33489SubscriberThank you!
>> 36*time is the equation for the rotation angle of the joint. At 1 second, the joint will have rotated 36 degrees.
What if the angle of rotation depends on the moment? I can't set the angle directly, I only know the moment.
May 31, 2022 at 7:40 pmpeteroznewmanSubscriberFor low speed gears, the stress in the tooth is a function of the angle of rotation. A tooth first comes into contact with another tooth at angle A, and after a small rotation of dA, that tooth is about to leave contact. You only need to sample a few angles between A and A+dA to see different states of stress. These can all be Static Structural solutions. You can apply whatever moment is appropriate for each angle.
- 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
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.