Regarding Connecting two parts that will have nuts and bolts

  • 144 Views
  • Last Post 2 weeks ago
ygauri posted this 3 weeks ago

Hello,

 

I am performing Modal Analysis on Gas Compression Skid. Parts like engine and compressor are bolted to pedestal in reality. So while performing Modal analysis what type of connections I should use?

I tried to use bonded connection between two faces but not getting desired output. Looking for some helpful guidance urgently.

Order By: Standard | Newest | Votes
peteroznewman posted this 3 weeks ago

I would also have chosen bonded contact. Why do you think you are not getting the desired output?

ygauri posted this 3 weeks ago

I am not sure. I think may be my connections in region of bolts should not be bonded and must be something different. Is there a way to give contact region of certain diameter around the holes, so that rest of area will be free and only the region falling within that diameter will be bonded. 

peteroznewman posted this 3 weeks ago

Please reply with some images of your geometry and show me what your area of concern is.

You can divide faces and bond only on local areas instead of the whole face.

ygauri posted this 3 weeks ago

So basically my entire modal is huge and many different parts. So to avoid long computational time, I am using block of same weight as of original engine. An engine is mounted on feet and then feet on pedestal. So what's best way to connect engine on feet and feet on pedestal to get correct natural frequencies?

 

Also I am not considering Pre-Stress Analysis because for modal analysis unbalance forces don't need be consider, correct?

 

Thank you in advance for all your help and guidance Sir. I really appreciate it.

peteroznewman posted this 3 weeks ago

Bonding the whole flat surface of the grey foot to the pedestal is overly stiff.

You can instead make a beam connection between the ID of each bolt hole in the foot with the adjacent bolt hole in the pedestal. You get to specify the beam radius and its material.

ygauri posted this 3 weeks ago

yes, I will try that and will let you know whether it worked or no. Also its fine if I don't consider Pre-Stress Analysis for my modal? 

peteroznewman posted this 3 weeks ago

I doubt the Pre-Stress will move the Modal results very much at all, but it is easy to setup and run both ways to check.

ygauri posted this 3 weeks ago

is there way in ANSYS to apply directly horizontal and stretch components value of unbalance forces at CG?

 

Also for connections: connection between pedestal and plate, I have selected edge of pedestal (brown color geometry) and entire surface of plate (dark grey flat surface) is that appropriate or it will make my modal again overly stiff?

peteroznewman posted this 3 weeks ago

How many bolts hold the brown pedestal to the grey plate?  Put holes in both parts and use Beams to connect the two holes.

The best way to apply a horizontal force to the CG of a body is to use an Acceleration load. Calculate a = Force/mass. Note that the acceleration applies to all mass in the model, not to a single body.

ygauri posted this 3 weeks ago

Thanks for the info sir, but brown pedestal will be welded to plate. And welding will be done at the boundaries of pedestal. So for that what would be the appropriate connection.

ygauri posted this 3 weeks ago

Also I am getting many extra natural frequencies and mode shapes that are not according to my expected results.

peteroznewman posted this 3 weeks ago

Make the four sides of the brown pedestal a Fixed Support and suppress the grey plate from the analysis.

Please describe the experimental results and how they were measured and then describe the Modal analysis results.

  • Liked by
  • Jackely
ygauri posted this 3 weeks ago

I am trying to extract 6 mode shapes. The values are as follows in Hz from Modal Analysis:

27.5, 31.2, 33.5, 44.6, 46.4, 50.2. 

I am just trying to match the results with the report I have from some outsourced company. According to them for same model I should get results as:

26.4, 33.4, 46.9, 50.2, 55.7 and 62.

So according to me I am getting extra modes in-between. I have used I beam connection for holes with dia of 0.5. For fixtures I have used elastic support to the base plate because that will be filled with concrete. The value for elastic support I have used is of 10000.

To describe my setup: Engine, compressor frame and cylinders are mounted on pedestal. Entire pedestal is mounted on plate called deck plate. Deck plate is welded to frame made up of I beams.

 

ygauri posted this 3 weeks ago

I am trying to extract 6 mode shapes. The values are as follows in Hz from Modal Analysis:

 

27.5, 31.2, 33.5, 44.6, 46.4, 50.2. 

 

I am just trying to match the results with the report I have from some outsourced company. According to them for same model I should get results as:

 

26.4, 33.4, 46.9, 50.2, 55.7 and 62.

 

So according to me I am getting extra modes in-between. I have used I beam connection for holes with dia of 0.5. For fixtures I have used elastic support to the base plate because that will be filled with concrete. The value for elastic support I have used is of 10000.

 

To describe my setup: Engine, compressor frame and cylinders are mounted on pedestal. Entire pedestal is mounted on plate called deck plate. Deck plate is welded to frame made up of I beams.

So is there anyway that you can guide me to rectify my mistake, so that can get desired results.

peteroznewman posted this 3 weeks ago

Here is how I would lay out the frequencies and the modes.

Please rerun the Modal analysis and request 12 modes and fill in the next few cells to see if you get close to 62 Hz.

When a structure is symmetric, ANSYS will report a double mode, one for each coordinate direction, but an experimental report will see only one mode, and will not report a double mode.  I haven't seen the shape of the modes but that could be happening for one of the closely spaced modal frequencies. You haven't shown the mesh, you might find that as you refine the mesh, you get slight movement in these frequencies. Please reduce the element size and rerun the Modal analysis.

While ANSYS shows mode shapes, what is in the experimental report on the mode shape?  How did they determine a resonance frequency?  Did they use accelerometers to measure the response of the structure?  How many locations did they monitor?  How many axes did they monitor? It is quite easy for a sensor to miss a mode that is calculated by ANSYS if a mode does not excite the motion at that particular location. That happened in this example.

ygauri posted this 3 weeks ago

yes sir, that might be case of double mode. And the report with which I am comparing is of Modal Analysis using ANSYS. In short I have report of modal analysis performed using ANSYS by someone else and I am trying to perform the modal analysis on same modal and get the same outputs. But somehow m y output is not similar to him not even mode shapes. I will post mode shapes as well in a while to give you idea about how my model is behaving.

ygauri posted this 3 weeks ago

so these are the 1st and 2nd mode shapes that I am getting. For first 2 mode shapes the value should be around 26.4 and 33.4. But mine are different.

peteroznewman posted this 3 weeks ago

Oh, I thought the outside company was providing an experimental result, so you should have their mode shapes if it is a Modal analysis.

Do you know how to Suppress Geometry? Go in and suppress all the geometry except for the brown pedestal, the four feet and the engine block. Make the four sides of the brown pedestal a Fixed Support.

Click on Mesh and in the Details window, you want to make sure it is using Quadratic elements and has at least two element through the thickness of the thin walled part of feet.

ygauri posted this 3 weeks ago

Yes sir, I have their mode shapes. So by doing this suppress thing, what should be expected?

Just to know about connections?

While importing modal ANSYS generates the connections on it owns, so if check overlapping it says few connections are overlapping, so is there any easy way to fix those overlapping. It seems if one face has many connections then ANSYS consider it as overlapping.

Also the solving method I am using is Direct because its giving me error in PCG metho (iterative)

Also the mode shapes from other company has same mode shapes (first 2 mode shapes) to mine but the frequency values are different.

 

ygauri posted this 3 weeks ago

So sir, to have atleast two elements through thickness, I should just select the feet and use Num cells across gap =2 ?

peteroznewman posted this 3 weeks ago

Suppressing unnecessary geometry will result in the Modal analysis taking less time to solve. That is all.

Turn off the automatic detection of contacts on Attach.  However, suppressing does not require a new Attach. Delete all the new contacts that were created.

Direct solving is best unless it is a very large model and you run out of RAM.

Two elements through the thickness is a Global setting.  It might cause your frequencies to move around a little because of a better quality mesh.

ygauri posted this 3 weeks ago

so if my modal is created in solidworks and all the parts are matted properly then I don't need to create any contacts in ANSYS?

peteroznewman posted this 3 weeks ago

The mates in SolidWorks keep the solid bodies in the correct location in space.

When the geometry comes into ANSYS for the first time, you have to either manually or automatically define Contacts.

If you have the SolidWorks CAD interface, so ANSYS brings the model straight into Mechanical from SW, then you can bring geometry updates from SW into Mechanical and all the work you have previously done creating contacts should be maintained and all the contacts will simply update to the new geometry.

ygauri posted this 3 weeks ago

Hello Sir, I did the way you told by just considering engine, pedestal, cylinders. The pedestal was fixed at bottom and T supports were fixed at bottom. So now I got results that are very off. I have attached the pic

ygauri posted this 3 weeks ago

Sir, can you also guide me how to resolve this error, I tried to look but was not able to solve this.

peteroznewman posted this 3 weeks ago

The Mesh setting for Proximity that I showed in my post above is what automatically puts 2 elements through the thickness.  Did you do that?  It sometimes doesn't take if some other settings are way off, like the element size.

ygauri posted this 3 weeks ago

Yes, I tried with that just now, still the output is not according to expectation.

peteroznewman posted this 3 weeks ago

Would you like to save a Workbench Project Archive .wbpz file and attach that after you reply with the version of ANSYS you are using?  I will take a look.  Note the file size must be < 120 MB.

ygauri posted this 3 weeks ago

can I email you that file sir? 

 

Would be happy to get your email id.

 

ygauri posted this 3 weeks ago

Is there way to arrange meeting via webex to better understand my modal. Because sir I won't be able to upload file because of my privacy issues.

Show More Posts
Close