July 8, 2019 at 9:57 amnish2608Subscriber
I am performing random vibration analysis for a cubesat by applying the PSD graphs in all the three directions considering all the fixed supports.
I am getting unusually high amount of stresses in the bolt holes and around the bolt hole region. My modelling for bolt is the beam connection along with pretension given in the static structural which is then connected to modal and random vibration.
How do I interpret these stresses or even ensure that they are right?
July 8, 2019 at 10:07 amjj77Subscriber
Can you add some images of these regions and high stresses. Also are bolts modelled in 3D or by beams or the like?
July 8, 2019 at 10:22 amnish2608Subscriber
The bolts are modelled by 3D beams in ansys workbench. The stress in abnormally very high around the bolt hole and I'll add some images later.
July 8, 2019 at 10:29 amjj77Subscriber
It is most likely what is called a stress singularity - look it up and you will see a lot of info on that.
July 8, 2019 at 10:33 amnish2608Subscriber
But these stresses are mostly around most of the bolt holes, do you think the mesh issue for stress singularity might be occuring on all of them?
I mean, do we ignore those stresses and focus only on the main structure?
July 8, 2019 at 10:40 amnish2608Subscriber
Also, when I tried to bond the surfaces instead of making the bolts, the stress diminished around the bolts holes and reduced greatly.
Would that also be a possible solution to mimic bolting and avoiding stress singularity?
July 8, 2019 at 10:46 amjj77Subscriber
This is a very long chapter - it depends what you are interested in really (bolts, or welds,...) - perhaps someone else can give some more tips
July 8, 2019 at 11:29 ampeteroznewmanSubscriber
nish2608, what did you scope the beam to at the bolt hole? If you scoped it to the edge, that creates a higher stress than the real bolt head which makes contact to an area under the bolt head. You can reduce this stress by imprinting a circle around the hole to create a face to scope the end of the beam to. The area of the face distributes the load and reduces the stress.
As jj77 requested above, please post some images in your reply so we can see your model and mesh.
July 8, 2019 at 12:03 pm
July 9, 2019 at 11:40 amnish2608Subscriber
So I tried with scoping the bolt hole to the face which reduced the stress to some extent. For a 2.5mm hole I built a split line region for 5mm OD and 2.5 ID around the bolt hole. Would that suffice? I have attached an image for you to see the split lines.
Also how does one realize a stress singularity at the sharp corners of the geometry? As in, how does one recognize it to ignore it?
July 9, 2019 at 11:47 ampeteroznewmanSubscriber
The split face around the holes look fine.
To remove the stress singularity at a sharp interior corner, edit the geometry and add a blend fillet radius to the sharp corner to remove it from the geometry.
July 9, 2019 at 11:48 amnish2608Subscriber
All right I'll try that. But about the bolt holes...would the 5mm split line help?
July 9, 2019 at 1:14 pmpeteroznewmanSubscriber
Yes, the 5 mm split line will help.
July 10, 2019 at 5:25 amnish2608Subscriber
Also, how would one recognize if the given stress at a point is a stress singularity and can be ignored?
July 11, 2019 at 7:16 amnish2608Subscriber
Hey, so here are some images of my solution.
Firstly the problem around the bolt holes has been solved. Thank you for that!
Secondly I am still getting unusually high stresses on the corner of the structure. I made a 0.5mm fillet on all the edges and the corners of a part of the object to try out the solution but the stress is very high there while it is not as much in the surrounding area. You can have a look at the images.
July 11, 2019 at 12:46 pmnish2608Subscriber
Could you help me with the above simulation?
July 11, 2019 at 4:44 pmpeteroznewmanSubscriber
- It looks to me like the high stress is in an appropriate location.
- If the input PSD is large enough, the stress in a part can exceed the yield strength or even the UTS.
- Changes to the design can move the natural frequency of the structure away from a high point in the PSD.
- To move a frequency, you can increase or decrease stiffness of the structure and/or you can add or remove mass.
- Please show the PSD plots and the list of modal frequencies from the Modal analysis marked on that plot.
- Which mode(s) are near the high values in the PSD?
July 11, 2019 at 4:49 pmpeteroznewmanSubscriber
This Random Vibration analysis is linear, which means it has linear materials and linear connections. If you can't change the design, you can do a Transient Structural analysis that allows for nonlinear effects to be included, like large deformation, material plasticity and frictional contact. You would need to synthesize a transient waveform that meets the PSD specification as the input load to the model
Transient Structural with nonlinear effects is a lot more work and requires a lot more computational resources and solve time than the Random Vibration analysis.
July 12, 2019 at 5:18 am
July 12, 2019 at 5:20 amnish2608Subscriber
Also I have some optical components inside the structure also having a problem with the stress. They have been bonded with the optical mounts which are bolted inside since I thought I can consider them to be in place while the loads are being applied. Could there be a problem with my modelling there?
July 12, 2019 at 11:38 ampeteroznewmanSubscriber
The stiffness of a structure is best increased by changing the shape of the parts from shapes that allow bending to occur in the part, such as the long flat parts I can see inside the cube, to parts that don't allow bending to occur, such as truss links that form triangle and tetrahedral structures.
Optical mounting should be designed so as to not transfer stress to the mount. There is a design methodology called Exact Constraint design that provides this benefit. If the connection between the cube structure and the optical mount is over constrained, that allows high stress to occur in the optical mount. Change the design to Exact Constraint, and the stress in the optical mount will be reduced.
If you want me to look at this design and offer suggestions, please use File > Archive to create a .wbpz file and attach that after you reply with the version of ANSYS you are using. Also say what CAD system created the geometry. If you imported a Geometry file into SpaceClaim or DesignModeler, put that file in a zip archive and attach that also.
The goal would be to move the modal frequencies above 1400 Hz because after 800 Hz, the PSD magnitude drops rapidly until 2000 Hz.
July 12, 2019 at 2:15 pmnish2608Subscriber
I will try sending you the file in sometime. I am just assimilating all my data. It would be great if you could help me.
Also I had a few more doubts:
1) Firstly, for modelling bolts in ANSYS, I use the beam version along with specifying a contact region between the bodies in contact. For now, I am using the no separation contact since I thought it would help me model the fact that the bolts would prevent the structure from separating in a direction perpendicular to the plane of the surface in contact. Is that correct?
2) How does one assert the structure in frequency based analysis? In the sense, does one look at the modal shape (in my case there are a 150 shapes) and see where the support or the truss is needed or does one just look at the modes and try to make them go higher by adding mass?
3) How does one know if the stress coming at a point is a stress singularity or just the stress due to the loads?
July 12, 2019 at 9:07 pmpeteroznewmanSubscriber
Here are the directions for sharing models. If you have a CAD file that was imported, put that in a zip file and attach that also.
1) The bolts hold parts at a fixed distance with the stiffness of the bolt shaft diameter, length and material. You don't also need contact.
2) Adding mass lowers frequency, which is sometimes helpful. When you look at modal results, you should look at the participation factor summary available under the Solution Information Folder. High participation tells you that mode is more important than a low participation mode so you should study that mode shape for clues about where to put material to prevent that type of flexibility.
3) If there is high stress at an interior corner in a Random Vibration analysis, it doesn't matter if you put a small blend there or not. A small blend is not going to change the stiffness of the structure significantly so won't change the result, but a huge blend, which looks more like an extra web supporting the corner, that would change the stiffness of the structure.
July 14, 2019 at 6:43 amnish2608Subscriber
As you said about the bolt, even I had thought the same way. But the problem is the solution shows an error if there no additional contact there along with the bolt. As in initially, everything comes bonded once the structure in imported in ansys WB. Then, I start adding beam connections and subsequently change the corresponding contacts in the structure to " No separation" since it causes an error if there is no additional contact.
Secondly, I understood your logic about the modal shapes. But the problem is that the structure is showing stresses at some other points in random vibration and shock response analysis which does not seem to come up in the top 5 modes (ranked acc. to participation factor) in each direction. Hence the problem in understanding the stress on the outer corner of the structure as shown above.
Also, I tried adding a fillet but that does not seem to change much in the stress.
I will archive the simulation by tomorrow evening and send it to you ASAP. Thank you so much for your help.
July 16, 2019 at 5:12 amnish2608Subscriber
Could you please help with the above problem?
July 16, 2019 at 4:03 pmpeteroznewmanSubscriber
Please upload the archive so I (and/or others) can take a look.
July 22, 2019 at 5:55 amnish2608Subscriber
I am sorry but I am unable to post my model on the archive due to confidential reasons. Is it possible for you to have a face-to face web session on skype or zoom where you could help me with the model?
It would be great if you could help me with the same since I am in a pickle regarding certain concepts about my model.
July 22, 2019 at 5:20 pmpeteroznewmanSubscriber
Yes, we could do a web meeting. Do you have a zoom account?
What time zone are you in? I am in the Eastern Time zone (USA).
I can talk for an hour between 8-10 PM Eastern Time on most days.
July 23, 2019 at 1:36 pm
July 23, 2019 at 6:05 pmpeteroznewmanSubscriber
You reply with your email ID and I will send you an email as soon as I read it, and delete your ID from your reply. Any day this week is open for me.
July 24, 2019 at 12:58 pmnish2608Subscriber
so my email ID is [removed]
I would like to have a chat as soon as possible. How about 8 PM according to your timezone?
July 24, 2019 at 2:07 pmpeteroznewmanSubscriber
8 PM today is okay. Send details to my email address.
- 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
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.