February 12, 2022 at 12:14 amVasilEvangelosSubscriber
I have a model that includes a large number of beam connections.
I am running a parametric study with the current model, and whenever the geometry changes the beam connections are not updated.
Is there any way of updating the connections automatically and not manually ?
Thank you in advance.
VasilisFebruary 12, 2022 at 9:50 pmRameez_ul_HaqSubscriber,it would be better if you could share some pictures on this thread to manifest what you mean by 'beam connections'.
If you are just connecting different beams together (to make them work as a single beam, for example), then you can directly go for the shared topology option in SpaceClaim or DesignModuler.
February 12, 2022 at 10:33 pmVasilEvangelosSubscriberThank you for your response.
I have uploaded, below some pictures of the model.
In the model I have more than 100 bolts, to support the plates, modeled as beam connections.
I want to run a parametric study, changing the thickness of the plates.
But while the geometry of the model changes, the "beam connections" they dont get updated, even if the mobile and reference geometries are scoped to named selections.
I was wondering if there is a way to update these connections, during a parametric study like this.
February 12, 2022 at 10:38 pmRameez_ul_HaqSubscribertry not using the named selections and just directly using the faces/edges for each beam connection, to whatever the topology you are scoping it to.
February 13, 2022 at 1:40 pmpeteroznewmanSubscriberWhen a Beam Connection is created, the Coordinate System is Global.
That creates a problem when the length of the part changes, the beam is left behind.
You have to make a Coordinate System scoped to the geometry that is moving, then use that Coordinate System in the Beam definition.
Now the beam will follow the length change.
ANSYS 2021 R2 archive attached.
February 14, 2022 at 9:32 amVasilEvangelosSubscriberThank you both and for your help.
I tried the method that you suggested and it's working.
This method is really helpfull because in bolts modelling tutorials, is stated that one major drawback of the "beam connections" is that you need to re-generate them from scratch if the geometry changes.
This step can save you a lot of time.
February 14, 2022 at 10:36 ampeteroznewmanSubscriberI wish ANSYS would change the Beam connection to automatically generate a coordinate system on the geometry selected for the Reference side of the connection. Or at least have a checkbox to request that. This becomes a big time saver if you are using the Object Generator to create hundreds of bolts.
February 14, 2022 at 10:44 amRameez_ul_HaqSubscriberI don't have ANSYS 2021R2 currently installed on my computer so I cannot download and check the archieve file, so I would be askinga question here about the new co-ordinate system that he has built.
January 5, 2023 at 4:59 pmSean HarveyAnsys Employee
I agree with you, so I submitted enhancement request 5ERAFE01052023 on this.
So we should be scoping the 'Moving co-ordinate system' to both the faces (I mean Reference face as well as Mobile face of the beam connection) if both bodies are changing geometry, and then just use this new co-ordinate system in both i.e. Reference and Mobile for beam connection, or we should be constructing a new co-ordinate system scoped to reference face and another scoped to mobile face, and then use these new co-ordinate systems for each of the reference face and mobile face separately, in beam connection? Would it make any difference between these two options?
February 14, 2022 at 11:04 ampeteroznewmanSubscriberFor Beam connection, where both faces are always going to be coaxial and close to each other, only one Coordinate System is needed and I scoped it to the Reference side. Then when typing the coordinates for each end of the beam, I used different values for the Y coordinate of the Reference and Mobile sides of the Beam using the same Moving Coordinate System.
I sometimes add Springs to Parametric Models and the ends of the springs can move independently when the Parametric dimensions of the two parts change. In that case, I create two Coordinate Systems, each one scoped to the spring anchor point on each part. Then in the spring definition, the coordinates are defined at (0,0,0) in each respective coordinate system. In this way, the spring is always created between the two scoped faces or edges.
Viewing 8 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
- 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.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
Top Rated Tags
© 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.