January 12, 2022 at 2:45 amwangx3Subscriber
1) Would it be possible to add a remote distributed mass in WB? I know I can add remote point mass. but is it possible to add the distributed mass, for example, along a beam?
2) How to add directional mass? for example, the added mass only works in 2 horizontal directions but will not in the vertical direction (gravity ) in the response spectral analysis?
thanks.January 12, 2022 at 7:01 amErik KostsonAnsys EmployeeHi
See this post (link below) that shows the command snippet for converting a remote point mass to be only active in the X-Direction (see the help manual for more info on mass21 element).
As for the distributed mass there is an option in Mechanical under the Geometry tab and is called Distributed Mass (it can not be remote of course, and is added on top of the face that we pick under scoping - this distributed mass option is to approximate say coatings/paint on steel deck, some floor coverings in office floors, etc, which are attached to a structure so it can not be remote.
All the best
January 15, 2022 at 3:19 amwangx3SubscriberThank you!
Following up on the distributed mass modelling, if it is for beam structure, would the loads be applied on the beam neutral axial or on its top?
Specifically, I have a frame structure for dynamic analysis. There will be some distributed load (mass) on the top floor. But the vertical centre of the mass is above the floor with a distance of d as sketched in the attached figure. Can you suggest how to model this distributed load (mass)? thanks.
January 17, 2022 at 8:34 amErik KostsonAnsys EmployeeHi
Distributed mass option (it uses surf154 or surf155/156 in the background) can not be offset.
One way which I have never used and that might be OK, is to use mpc184 with offset mass21 elements.
Here is how it would like:
We can not advice on how to script this, but other users might be able to help here.
The psevdo commands(APDL) snippet would be something like this:
Define mass21 and mpc184 elements
Define density for mpc184
Select all nodes for beams
Loop through beam nodes
Generate offset nodes (green dots shown above)
Attach/add mass21 to these new offset nodes (mass21 can be as mentioned with mass only in one direction)
Create mpc184 rigid links between beam nodes (red dots), and the new offset nodes (green dots).
All the best
January 17, 2022 at 10:01 amwangx3SubscriberHi Erik
Thanks. I have the same thought. First, I will discretize the continuous line load to concentrated node load first. Then I apply a remote point mass on the mid node of the beam. But noted that I should have sufficient nodes for approxiamations.
Another one I want to try is to apply an equivalent remote mass associated with all the beam nodes. but I don't know how ANSYS distributes the mass to the nodes. based on the distance to the centre of the total mass?
January 17, 2022 at 11:12 amErik KostsonAnsys EmployeeHi
When we use applied by with a remote attachment for the point mass, then there are some option (behaviour), such as coupled, deformable and rigid.
The rigid would make that connection of the mass down to the frame rigid, while distributed or coupled would distribute the mass more to the nodes of the frame without adding the stiffness the rigid option does.
If you search for remote attachments and points online and in the help manual you will find quite a lot of info on that.
Their behaviours are similar to RBE2 (rigid -remote attachment) and RBE3 (distributed remote attachment).
All the best
Viewing 5 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- How to calculate the residual stress on a coating by Vickers indentation?
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Errors – Reinforced Concrete Beam
- Command Object Snippet
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- An Unknown error occurred during solution. Check the Solver Output…..
- Large deflection
- Transient Structural analysis?
- Revolute joint (Static structural) Very high deformation
Top Rated Tags