September 4, 2022 at 6:27 amminghui.daiSubscriber
Few introundction in ansys help on how to set the inertia of the mass moment when define a point mass.
It descirbles they are the inertia of center of mass as marked red below, but I found someone else said it's the pricipal inertias as marked yellow, and may need to adjust the vectors if not allied with the global. could anybody give me a right answer on it. thank you very much
The Point Mass in Mechanical Workbench creates a MASS21 element for the mechancial solver to use. If you open the ANSYS Help system, you can read the description of that element in the Element Library. The inertia inputs are Principal Inertias relative to the coordinate system used to define them.
In SpaceClaim, on the Measure tab, click the Mass Properties button then select a solid body. Assign the body a Material in the Properties window. The Principal Inertia values and axes will display. Hover over any row and you can copy the data to the clipboard. Paste that into a text editor and repeat two more times to get the three values.
I have not figured out how to get this coordinate system into Mechanical. Looking at the options on the definition of a new coordinate system, I don’t see a way to do this.
What I would do if I had the solid object in CAD is simply to import this into Mechanical, assign it to be a Rigid Body, create a material with the correct density for that body, and assign that material to that body. Then the correct principal inertia will be submitted when you solve the model.
Here is the code for that rigid body that was sent to the solver, it is a MASS21 element.
/com,*********** Send Body as a Rigid Body ***********
keyo,1,2,1 ! Moments of inertia in nodal coordinates
keyo,1,3,0 ! 3D Mass With Rotary Intertia
You can see the local coodinate system being defined in the code above.
Thank you for your help. It's clear for me now.
for the principle inertia properties and coordinate systems, you could do a static analysis with a comand to get it as shown below.
But I still have a problem? how could we define the coordinate in workbench? by command? or calculate the rotate degrees by hands ( it seems quite low efficiency)?
Thanks for the tip about IRLF,-1
I don’t see a way, without using some APDL code or having geometry such as the solid block, to create a coordinate system in Workbench from the unit vectors provided.
With that solid block, I was able to select faces to orient the X and Y axes and create Csys_CoM as shown below, where I typed in the origin as provided in SpaceClaim.
Then I could use that coordinate system to define the Point Mass.
However, if I had the solid block in Mechanical, I would just use that as a Rigid Body and let the solver compute the principal inertias and axes.
Let’s say an assembly is purchased to bolt onto a structure and the vendor provided the coordinates of the CoM, the Principal Inertias and their unit vectors relative to a Csys on that assembly. Now I want to represent that using a Point Mass. The vendor may provide a shrinkwrap solid of the assembly, but that solid doesn’t have the correct inertia properties because the internal density is not uniform in the physical assembly. I can construct a small block using the first two unit vectors. Create a plane at the Z coordinate and make a point at the X, Y coordinates of the first unit vector. Repeat on a new plane for the second unit vector.
Enable 3D Sketch and draw two lines for the two unit vectors.
Pull the first line along the direction of the second line to the halfway point.
Pull the surface into a block, just a small distance so the three principal directions have different thicknesses.
Now you have a solid block to create the Coordinate System for the CoM that will have the correct Moment of Inertia Principal axes!
Yeah, create a line in spaceclaim to get the directions and then import to workbench, that is a method, but it's still complex and cost time for large models in our projects due to several compnents need to replaced with pointmass and the time is very long when transfer from spaceclaim to workbench.
- You must be logged in to reply to this topic.
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
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.