December 9, 2019 at 11:08 pmrmaur29Subscriber
I have modelled conveyor drives and connecting pulley & structure in ANSYS and used modal analysis to identify natural frequencies in the model. I have obtained a first mode frequency of 7.5 Hz although the actual test results show that it should be 3Hz and the displacement of the system seems to be excessive. I have modelled the geometry as close as possible to provided drawings and ensured that the weights of the components match actual weights. I have checked all contact regions between components, but the first mode shape displacements seem too excessive and the frequency is 7.5 Hz instead of 3Hz.
Does anyone know what may be the reason why the model is not similar to test results?
December 10, 2019 at 12:16 amparkersheafferSubscriber
displacement of the system seems to be excessive
When you run a modal analysis in ANSYS you are not providing any input so the displacement that is displayed it not a real value. The displacement is to be used as a relative displacement in your model(how one point displaces from another).
If your natural frequencies are not matching its likely that the stiffness of your model is incorrect. It could also be mass but you mentioned you verified all your components.Without knowing more about your model i would suggest take a look at your contacts and joints. In a modal analysis you have two contact types bonded and no separation, frictional and rough become bonded and friction less becomes no separation. If any of the contacts change during your analysis you might be causing some over constraint which will impact your results.
One other potential source of error is the equipment you used to measure the 3hz natural frequency. I assume you used some calibrated device but its always good to check.
December 10, 2019 at 4:58 amrmaur29Subscriber
Thanks yes I believe that it was something to do with the contacts, as all weights were correct as well as geometry. I have made some changes to the pulley connections to increase its rigidity, but the problem is that to reduce the displacement it requires increasing stiffness, which increases the natural frequency which is not closer to test results. It has been tested multiple times to verify 3Hz so im its possible but unlikely
December 10, 2019 at 1:21 pmpeteroznewmanSubscriber
Rmaur29, Parker correctly said "so the displacement that is displayed it not a real value" yet you have said "but the problem is that to reduce the displacement...". If the displacement you are talking about is from the Modal analysis, you have not understood Parker's point.
The displacements in a Modal analysis are arbitrarily scaled and have no relation to measured displacements in a real experiment because there are no loads in a Modal analysis. One way to simulate real displacements is to add a Harmonic Response analysis to the Solution cell of the Modal analysis. In the Harmonic Response, you can insert a load. For example, a force that represents a periodic force from an unbalanced mass on a spinning shaft will induce some vibration into the machine, depending on the shaft speed. The amplitude of the machine vibration will depend on the magnitude and frequency of the unbalanced force and the modal frequencies in the structure.
If you want more specific suggestions on how to revise your model to reduce the first natural frequency, reply with images inserted into your post of the structure. The more detail you provide, the better will be the suggestions. Show how the machine is connected to ground. If you used a Fixed Support, that may be too stiff compared with the real machine. You could replace a Fixed Support with a Pinned joint to ground to add some flexibility to the model, lowering the first natural frequency. Parker may have other suggestions.
December 11, 2019 at 5:41 amrmaur29Subscriber
Thanks yes its my error that I repeated using the term displacement, I understand that a true scale of displacement is not represented in modal analysis mode shapes and that's fine, my main concern is just lowering the natural frequency and yes currently my supported is fixed whereas in reality there should be more degrees of freedom. I have attached the model screenshots including the fixed support, which I need to create some rotation release around the pins. currently attempting this but seems to be very tricky, as I'm splitting the pin into three sections and applying different degrees of freedom to each section so the pin isn't spinning on its own axis.
December 11, 2019 at 1:07 pmpeteroznewmanSubscriber
(1) Use the Insert Image button to put the image directly into the post because ANSYS staff are not permitted to open attachments.
(2) Learn to use the Snipping Tool to screen grab just the region of your display that has what you want to show.
The massive white border on the right and bottom edges of those files makes for a practically useless image.
December 11, 2019 at 9:21 pm
December 11, 2019 at 9:24 pmrmaur29Subscriber
First image is first mode shape of modal analysis, second is general layout of geometry, and the third is the torque arm/fixed support, which current doesn't allow rotation of components arounds pins.
December 11, 2019 at 9:27 pmparkersheafferSubscriber
You do not need to include the pin in the model, replace it with a revolute joint( 5 DOF constrained, 1 rotational DOF free).
December 11, 2019 at 11:27 pm
December 11, 2019 at 11:40 pm
December 12, 2019 at 12:07 amrmaur29Subscriber
Okay sorry now I understand revolute joint allows 1 DOF about z axis, I guess my question is what do I apply as reference and mobile faces? Im assuming the outer gusset plates inner hole faces as reference selection and the centre rotating member inner hole face as mobile?
December 12, 2019 at 12:08 amparkersheafferSubscriber
The revolute joint type already has the DOFs constrained all you need to do is select the reference and mobile faces.
December 12, 2019 at 12:21 amparkersheafferSubscriber
Sent that to address your previous question but you figured it out.
Im assuming the outer gusset plates inner hole faces as reference selection and the centre rotating member inner hole face as mobile?
Yep that should work.
December 12, 2019 at 1:02 amrmaur29Subscriber
yes thanks! it works now.
December 12, 2019 at 2:08 amrmaur29Subscriber
Does anyone know how to add frequency sweep in Ansys when applying an excitation force. I have done modal and harmonic analysis using the same supports. In harmonic I have applied a torque to the end face of the pulley shaft to represent the turning of the pulley shaft. just wondering can I flucturate this torque from a set 0hz to 30hz
December 12, 2019 at 4:05 ampeteroznewmanSubscriber
Any load that you add to a Harmonic Response is automatically a periodic load. The frequency of the load is varied in steps in a sweep from the lowest to the highest frequency requested in the Analysis settings. The response of the structure to each step in the frequency of the load is shown in the results.
If you request 6 steps from 5 Hz to 30 Hz you will get a result at every 5 Hz increment in the load frequency.
December 12, 2019 at 4:26 amrmaur29Subscriber
Thanks yes I see it, will give it a go.
- 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.