July 11, 2019 at 5:04 pmygauriSubscriber
July 11, 2019 at 8:56 pmpeteroznewmanSubscriber
Do you mean the pipe that seems to be passing through the bottle? If that pipe was supposed to be bonded to the bottle, then a large pinball radius needs to be included in the contact definition to make sure the bonded contact is working correctly.
July 11, 2019 at 10:12 pmygauriSubscriber
That is actually entire single body (suction bottle). Its not separate pipe. It will behave as single body.
July 12, 2019 at 4:37 ampeteroznewmanSubscriber
You have a skid with many components on it including pulsation bottles and an engine.
In your model, the lowest mode is the pulsation bottle, but you expected the engine to have the lowest mode.
If the mass of the pulsation bottle is higher than it should be, that will lower its natural frequency.
If the stiffness of the connections to the pulsation bottle is lower than it should be, that will lower its natural frequency.
Verify that the mass and connections to the pulsation bottle is correct.
July 13, 2019 at 7:34 amjj77Subscriber
I have worked on skid and machinery/pipe vibration on oil and gas equipment long time ago when apdl was the tool to use.
machines are typically just modelled as masses rigidly attached to the skids, and unbalanced and different forces are applied on these masses (your model is way to detailed - you need to think what is importnat here and what you are doing).
SO machines can be rigid, and pulsation bottles, depends on what is of interest. always measurements OMA (op. modal. analysis) were tuned to FEA (e.g., using FEMtools), because it is impossible to know all the details correctly, to have a reliable fea model.
See this website to see how these type of studies are carried out - require a lot of knowledge and experience, and are done by skilled trained engineers in vibrations, structural engineering that can perform advanced measurements and fea. E.g., see ODS Lloyd's register division which are specialists in these field. So there are a lot of things to learn. Look at their models and see how their tailored towards getting the results that are of importance. (Never used or seen a 3D mesh of all the details - this is a tendency from students to just mesh everything with tets, without understanding things). So to develop in this field one need the above skills (FEA, vibrations+measurements and structural engineering, so many things to study )
July 15, 2019 at 2:03 pmygauriSubscriber
I have verified the mass and connection. The mass of bottles is 173 lbs and its very less compared to engine. Also the bottle is connected to cylinder. Surface of bottle is connected to surface of cylinder. So even connection seems proper. Still not sure suddenly started getting 1st natural frequency for bottles. Also same connection was used earlier but at that time I was not getting this frequency.
July 15, 2019 at 2:10 pmygauriSubscriber
For my modal prestressed is not consider, so it means unbalance forced are not consider for modal analysis.. First step is to obtain natural frequencies and mode shapes. Also each parts in my modal has appropriate weights and all are connected using bonded connection.
And yes I agree that this things need experience and that's why I am trying to learn and get guidance from experts from this ANSYS forum and I am really getting good help.
So at present I am having issues with this mode shapes of pulsation bottles. I am not expecting this mode shape as 1st natural frequency.
July 15, 2019 at 8:49 pmpeteroznewmanSubscriber
You have a 4850 lb engine and a 173 lb bottle and the bottle has a lower natural frequency than the engine and you ask how that can be.
The mass ratio is 28:1 for the engine:bottle. If the stiffness ratio to ground was also 28:1, then both would have a similar natural frequency.
But if the stiffness of the connection of the engine to ground is more than 28 times stiffer than the connection of the bottle to ground, then the engine will have a higher natural frequency.
If you believe the bottle should have a higher first natural frequency than the engine, and if you have already verified that the mass of the bottle is correct, you must add stiffness to the material between the bottle and ground to raise its natural frequency.
July 16, 2019 at 4:18 pmygauriSubscriber
When I am using bonded connections and beam connections, at that time what should be the behavior? Rigid, Deformable or flexible?
Also for point masses that are being used in modal analysis should be rigid or deformable or flexible?
July 16, 2019 at 6:43 pmpeteroznewmanSubscriber
Read the ANSYS Help Mechanical Users Guide, Chapter 8: Specifying Remote Points, 8.2: Geometry Behaviors.
• Deformable: The geometry is free to deform. This is a general purpose option used when applying
boundary conditions such as a force or mass through ”abstract” entities not explicitly represented as geometry
inside Mechanical. This formulation is similar to the Mechanical APDL constraint defined by the RBE3 command.
• Rigid: The geometry will not deform (maintains the initial shape). This option is useful when the "abstracted"
object significantly stiffens the model at the attachment point. Note that thermal expansion effects cause
artificially high stresses because the geometry cannot deform where the load is applied. This formulation
is similar to the Mechanical APDL constraint defined by the CERIG command.
• Coupled: The geometry has the same DOF solution on its underlying nodes as the remote point location.
This is useful when you want a portion of geometry to share the same DOF solution (such as UX) that may
or may not be known. For example, to constrain a surface to have the same displacement in the X direction simply create a remote point, set the formulation to Coupled, and activate the X DOF. Because the DOF is
known, you can specify an additional Remote Displacement. This formulation is similar to the Mechanical
APDL constraint defined by the CP command.
• Beam: This option specifies that the Remote Point is connected to the model using linear massless beam
elements (BEAM188). This approach is more direct than using Constraint Equations and can help prevent
over-constraint issues that can occur with CE's. The following two user-defined properties are available to
define the connection:
– Material: specifies the material properties, except density, that will be used for the beam connections.
Using appropriate materials for the beams can help to more accurately model thermal expansion effects.
– Radius: defines the cross section dimension of the circular beam (CSOLID) and is sent to the Mechanical
APDL solver via the SECDATA command.
The Beam formulation can be useful when working with shells. For example, when you are trying to
model Spot Welds (p. 981) between two sheet bodies with holes.
You must determine which Behavior best represents the actual loading. Note that this option has no
effect if the boundary condition is scoped to a rigid body in which case a Rigid behavior is always used.
Presented below are examples of the Total Deformation resulting from the same Remote Displacement first using a Rigid formulation, then using a Deformable formulation, and finally the Coupled formulation.
July 16, 2019 at 8:07 pmygauriSubscriber
Thank you sir, that helps to decide for my problem.
- 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.