December 8, 2019 at 9:11 pmDeepeshSubscriber
I am trying to do harmonic analysis wth shaft and a disc over it and an extra mass (spherical) attached to the disc via beam.
That small mass is attached to disc via beam element
I have used bearings at both the ends of shaft and used rotating force on the disc as well.
This is the settings tree.
There are two errors which I am getting.
If anyone can help me fix there two?
December 8, 2019 at 11:48 pmpeteroznewmanSubscriber
I can't tell from the image posted whether the geometry and elements of the disk are solid elements or shell elements. I'm assuming the shaft is shell element .
If they are solids, that is a problem. Make them shells. The surface that is meshed with shells needs a vertex created to attach the beam, so the face should be split by a radial line and and circle to create the vertex.
Don't use a solid sphere at the end of the beam, use a Point Mass.
December 9, 2019 at 2:00 amDeepeshSubscriberAll are solids here. Sir, why would it be a problem?
Actually I tried removing beam element and it works fine but the result that I am looking to, has to contain beam element. So, dont you think there is something to be done with the beam element?
December 9, 2019 at 2:39 ampeteroznewmanSubscriber
Shell elements are designed so that a single element can compute bending stresses and each node has 6 DOF, three rotations and three translations. You can connect a beam to a single node of a shell element and it will be able to transfer bending moments from the beam to the shell.
A single solid element is very poor at computing bending stresses. You should have a minimum of 2 elements through the thickness of a thin solid. It is better if you have 4 or more elements through the thickness. You cannot connect a beam to a single node of a solid element because there is no rotational DOF to transfer moments from the beam to the solid. The only way ANSYS can connect a beam to a solid is by creating a spider of connection elements to spread the vertex of the beam across an area of solid element nodes. Try plotting the connection elements and you will see this hidden spider of connection elements.
December 9, 2019 at 8:25 pmDeepeshSubscriber
"The only way ANSYS can connect a beam to a solid is by creating a spider of connection elements to spread the vertex of the beam across an area of solid element nodes. Try plotting the connection elements and you will see this hidden spider of connection elements."
Sir, If you could please elaborate on this on how to perform this?
December 10, 2019 at 1:00 ampeteroznewmanSubscriber
Create an Archive .wbpz file of your project and attach it after you reply. I will use that model to demonstrate.
December 10, 2019 at 5:04 pmDeepeshSubscriber
December 10, 2019 at 7:41 pmpeteroznewmanSubscriber
Add a Modal analysis to your model. Solve that. Click on the Solution Information Folder. The main window will flip to the Worksheet tab. Click on the Geometry tab at the bottom left of the main window, you will see the Constraint Equations that are being used to connect one end of the beam to the disk.
Replace the solid disk and shaft with midsurface geometry. Split the face of the disk to make a vertex below the mass. Pull the ID of the disk Up To the Shaft midsurface. Use Share on the Workbench tab to connect the disk to the shaft. Use a Point Mass instead of the solid body mass. Now the Constraint Equations looks so much better, don't they?
December 11, 2019 at 1:43 amDeepeshSubscriber"Slice the face"
You mean using 'Split' option?
December 11, 2019 at 3:48 pmpeteroznewmanSubscriber
Yes, Split is the correct terminology. I made the correction above.
December 12, 2019 at 7:19 amDeepeshSubscriber1) I tried splitting the face of disc. Split is coming in as horizontal and straight lines by using 'split' option. I made a line perpendicular to disc and then revolved it. So it made a surface and then I used 'split' option. So now I have two surfaces on a single disc. Is this the way to split surface of a disc?
2) 'Pull the ID of disc into shaft':- is it like: dragging disc (left side under geometry tab) into shaft's component and then using 'Workbench' tab to share. Eventually making a contact between disc and shaft?
3) I can see the beam being shown as a single red line in the photo you uploaded. How do we convert it into that?
December 12, 2019 at 11:58 ampeteroznewmanSubscriber
1) Now I recall that Split seemed difficult to use, but you seem to have figured something out as long as you got a vertex on the surface. What I actually did was simpler. I clicked on the Sketch tool and picked the disk surface to sketch on. Then I drew a circle and two lines. Leave the sketch and return to 3D mode. The lines and circle have divided the surface into three faces.
2) After the midsurface operation, there is a half wall thickness gap between the shaft and the disk. Click on the Pull tool, click on the inside edge of the disk, click on the arrow pointing to the center then type U or click on the Up To button then click on the shaft surface. That will close the gap. However, if you just mesh that, the disk and shaft are not connected. You go to the Workbench tab and click the Share button, then a purple circle at the intersection shows that the mesh will be connected, and no Contact needs to be used in Mechanical.
3) In Mechanical, if you click on the sphere body, the mass of the sphere is shown in the Details window under Properties. Write that down if you want to use that exact value (or maybe you know the mass you want to use without reference to the sphere body). I assume you know the coordinates of the center of the sphere. Suppress the sphere body.
Right mouse click on Geometry and Insert Point Mass. For Scoping, click on the vertex on the disk. The coordinates of that point will be copied into the Details window. Edit the Y coordinate to move the Point Mass off the surface of the disk. Type in the Mass. That will create the image you see in my post.
December 13, 2019 at 1:58 amDeepeshSubscriber
Thanks a lot Sir, it worked.
Have some questions regarding this:
1)So, basically that point mass connection (Red colored) with the disc is acting as 'Beam'?
2)We don't need to use 'Beam' element option from connections?
3) I need a very rigid link between point mass and disc so that Mode of that point mass is passed to the disc without any intereference by the rigid link (Thats why I used 'Beam' from connections options). This normal point mass connection (Red) would work like Rigid Beam ?
4) We are dividing disc surface in 3-4 parts, won't it affect the results as now it is not a single body but divided surface ?
5) I wanna apply rotating force on this same disc in harmonic analysis, are there any changes required ? or I can directly proceed ?
December 13, 2019 at 3:52 pmpeteroznewmanSubscriber
1) A massless, rigid, Constraint Equation keeps the point mass connected to the disk. That is different from a Beam, which has a specific material and cross-section which together adds mass and flexibility to the model.
2) It is a Point Mass connected to the disk. You are not connecting a physical body that has a mesh so there is no way to use a Beam element.
3) See #1, CE is rigid.
4) Dividing the surface in geometry is just like dividing the surface up into "Elements" when you mesh. It won't affect the results unless you get a bad quality element.
5) Adding an unbalanced mass creates the effect of a rotating force by using a mass at some radius and rotational velocity. The Rotating Force load is the easy way to get this effect without the work you had to do to attach an unbalanced mass. Why do you want to also apply a rotating force?
December 13, 2019 at 5:45 pmDeepeshSubscriber
#5) Actually Sir, I wanted to use Rotating force as well as this extra mass(at some distance) from the disc.
#1) Case 1: Using 'Beam' between disc and sphere (Solid mass)
Case 2: Using point mass with CE
Which will give me more accurate result?
December 13, 2019 at 7:58 pmpeteroznewmanSubscriber
#1) If the physical system has a mass on a beam, then that is more accurate than a point mass.
December 14, 2019 at 3:34 amDeepeshSubscriberI tried with a solid mass (sphere) connecting to a disc via 'Beam' but is shows the error posted in the question. Sir, any suggestions on how to attach 'Beam' from disc to sphere?
I remove the Beam, that error 'unknown error' goes away.
December 14, 2019 at 4:24 ampeteroznewmanSubscriber
Keep the point mass. There are so many other areas where the model is only a coarse approximation of the physical system, the point mass is a fine approximation of the physical system.
December 14, 2019 at 4:40 amDeepeshSubscriberOkay Sir but just out of curiosity and knowledge that might help me in future analysis, is there any way for using Beam element with solid sphere but with point mass, we cannot use beam element?
December 14, 2019 at 3:00 pmpeteroznewmanSubscriber
You can have a beam connected to the disk. To do that, you have to go into SpaceClaim and on the Design tab, sketch a line on a plane through the vertex on the disk, then on the Prepare tab, define a cross-section and convert the line to a beam. Once you have done that, you can have three flavors of your model. Separate from Bonded Contact, you can also under the Connections folder have a Beam connection.
1) Beam only
2) Beam with a Point Mass connected to the end of the beam
3) Beam with a Solid Mass connected to the end of the beam.
All of these beams are different from a Point Mass on a Connection Element because the CE is rigid and massless.
Making that beam element manually in SC is a bit of work. Mechanical has automated the creation of a circular beam when using Bonded Contact, Type=Beam. With that you can insert beams between two objects. If the two objects are vertex points of geometry, then you get exactly one beam, but if you have two surfaces, then you can get a variable number of beams depending on the Pinball radius.
December 14, 2019 at 7:58 pmDeepeshSubscriber
Sir, posting few images. Please have a look at these:
Making a line in 2d sketch from that vertex
Coming back in 3D. Prepare-->Circular tube-->selecting this line-->Giving area(Left in properties box)
Point mass attached
5)Suddenly this extra surface comes. Is that a problem? before it wasnt there
6) Is this the correct way to make a beam from SC?
7) Modal analysis working fine with some weird deformations but it gives same error in harmonic that 'Unknown Error'
December 14, 2019 at 9:56 pmpeteroznewmanSubscriber
The last image with the huge rings means you typed in the wrong dimensions for the cross-section of the Tube in SpaceClaim. You have to go back to SpaceClaim and edit the Cross-Section and type in the proper internal radius and external radius of the Tube.
December 15, 2019 at 5:47 amDeepeshSubscriber
1)Sir, As you can see in the properties box, we don't have the option of giving an internal and external radius but only area. (Sir, please let me know if there is internal and external radius option anywhere)
2)meanwhile I tried another way:-- Creates a hollow beam till that vertex with some thickness and then used 'Extract' option which gave me below image after mesh. Is this the correct way? Or we have direct option of giving internal and external radii
December 15, 2019 at 12:26 pm
December 15, 2019 at 4:38 pm
December 16, 2019 at 1:14 ampeteroznewmanSubscriber
Click on the Worksheet tab and search the text for the word Error. What is the error?
What were the frequencies of the first 10 modes in the Modal analysis?
December 16, 2019 at 3:14 am
December 16, 2019 at 3:59 ampeteroznewmanSubscriber
#2) It seems like there are too many zero frequency modes. Look at each mode and see where the maximum deformation is located with the Result scale set to 0.0 Undeformed. Is there a duplicate beam that is not connected? See this example. See if fixing the excessive number of 0 frequency modes also resolves the Error message.
December 16, 2019 at 6:29 pmDeepeshSubscriber
Except few modes (taking in account 0-12 modes), rest max. deformation is at the beam (floating part)
There are only two places where it is shown (After checking the examply mentioned - to check for duplicates). This one is one side of the shaft. When i click other plane (Left bottom symbols of two planes), The other side of shaft gets selected
3) The other point where its showing duplicate is the vertex from where the beam is starting.
4) Actually should modes affect my harmonic analysis? because here I have given 'Full' and not 'Mode superposition'??
December 16, 2019 at 6:37 pmpeteroznewmanSubscriber
In SpaceClaim, did you go to the Prepare tab and click the Share button? If you did, then the line body should share the node at the vertex of the disk and the disk should share nodes with the shaft.
If you didn't do that in SC, you can repair the duplicate nodes in Mechanical by using Node Merge, but it is better to do it in SC.
4) Use a Modal analysis to check for missing connections between bodies even if Modal is not a pre-analysis to a full dynamic analysis, which will be incorrect or fail to run if a connection is missing.
December 17, 2019 at 3:55 pmDeepeshSubscriber
I clicked Share button and now the beam doesnt float but harmonic still shows the same error 'Gyroscopic matrix has been activated (RefFrame = ON on the CORIOLIS command) for rotating structure dynamics. When rotor spin is input
through the CMOMEGA command, the element axis must be along the spin
axis of the element component'
Sir, I've attached archived file just in case if you would like to see.
December 17, 2019 at 4:27 pmpeteroznewmanSubscriber
I don't do rotordynamics problems, so I hope someone who does can help you get this model to give some sensible results.
I previously gave you the ANSYS Help link to the Rotodynamics Analysis. Have you read that?
Here are 69 YouTube videos that you can study while you are waiting.
December 17, 2019 at 4:42 pmDeepeshSubscriber
Sir, This discussion till now, might have not given the end desired result but I learned a lot from this discussion. Thanks a lot, Sir!!!
Thanks for the YouTube links Sir, would go through them gradually.
Sir, I'll post this error for a separate discussion and would mark this discussion as 'Solution'. Would that be fine?
December 17, 2019 at 5:38 pmpeteroznewmanSubscriber
Dear Deepesh, you have learned a lot of useful model building skills that you will use in new models.
It would be best if you mark a post with Is Solution so the discussion shows as Solved. Start a New Discussion to ask a specific new question. This discussion has reached the Show More Posts length and some members don't like to read a long discussion.
- 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.