Random Vibration analysis

  • Last Post 24 July 2019
nish2608 posted this 08 July 2019

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?

Order By: Standard | Newest | Votes
jj77 posted this 08 July 2019

Can you add some images of these regions and high stresses. Also are bolts modelled in 3D or by beams or the like?

  • Liked by
  • peteroznewman
nish2608 posted this 08 July 2019

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.

jj77 posted this 08 July 2019

It is most likely what is called a stress singularity - look it up and you will see a lot of info on that.



nish2608 posted this 08 July 2019

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?


nish2608 posted this 08 July 2019

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?

jj77 posted this 08 July 2019

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

peteroznewman posted this 08 July 2019

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.

nish2608 posted this 08 July 2019

Yes, in fact I did scope the bolt hole to its edge. I will be uploading the images in a few hours (since I'm not at my laptop ) and it would be great if you could help me out. 

Also I will try the method you stated in the above post. Thank you so much!

nish2608 posted this 09 July 2019

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?

peteroznewman posted this 09 July 2019

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. 

  • Liked by
  • Jackely
nish2608 posted this 09 July 2019

All right I'll try that. But about the bolt holes...would the 5mm split line help?


peteroznewman posted this 09 July 2019

Yes, the 5 mm split line will help.

nish2608 posted this 10 July 2019

Also, how would one recognize if the given stress at a point is a stress singularity and can be ignored?

nish2608 posted this 11 July 2019

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.

What should I do about it?

nish2608 posted this 11 July 2019

Could you help me with the above simulation?


peteroznewman posted this 11 July 2019

  • 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?

peteroznewman posted this 11 July 2019

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.

nish2608 posted this 12 July 2019

Firstly how do we increase the stiffness of the model in that region?

Secondly I have attached the PSD table in the image which is applied in 3 directions.

And I am attaching an image for the 150 modal ferquencies I have found.

nish2608 posted this 12 July 2019

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?

peteroznewman posted this 12 July 2019

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.

nish2608 posted this 12 July 2019

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? 


peteroznewman posted this 12 July 2019

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.

nish2608 posted this 14 July 2019

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. 

nish2608 posted this 16 July 2019

Could you please help with the above problem?

peteroznewman posted this 16 July 2019

Please upload the archive so I (and/or others) can take a look.

nish2608 posted this 22 July 2019

Hi peteroznewman,

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.


peteroznewman posted this 22 July 2019

Hi nish,

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.

nish2608 posted this 23 July 2019

That'll be great sir. Can I have your email ID so that I can send you the details for zoom account and all the details (Also I can communicate more easily than on the form here ) ? Also when would you like to have the web meeting?

peteroznewman posted this 23 July 2019

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.

nish2608 posted this 24 July 2019


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?

Show More Posts