Learning Forum

[shantashreejena97]

Hey Everyone, 

I am doing an analysis of a turboexpander model. Can anyone tell me how could I put Orbit plot in each analysis?

[Rob]

Which solver are you using? You may need to export both sets of data and manually plot the two values using Excel. 

[shantashreejena97]

Thanks @rwoolhou for your reply. I am using reduced damped solver for both modal and harmonic analysis. Can you explain the process in an expand way because I am new in putting orbit plot.

[Rob]

I'm not familiar with the Mechanical tools, so we'll need someone else to explain how to get the data, but in terms of plotting this https://www.crystalinstruments.com/orbit-plot/  explains it.  So you need time v displacement (or whatever it is you're plotting) for two variables and then plot the variables against each other. 

[shantashreejena97]

Thanks for your reply @rwoolhou. As a beginner, I couldn't get what exactly the link is saying. So could anyone please help me to do the orbit plot of my model? Its an imported file from Solidworks.

[Rob]

I'm not sure anyone on here is an expert in orbit plots: I had to look it up as it's not something I'd routinely use as a fluids specialist. 

You should have two curves or sets of data: 

      x displacement  against time

      y displacement  against time

Read those into Excel and plot x displacement  on the x-axis and y displacement  on the y-axis

 

[Zdenek]

Hi Shantashree18

• If you have a model from Solidworks, it will probably be imported with elements called SOLID187 or so.

What you have to do is to actually change it to elements called BEAM188. Here is an example with a model, where I have a simple rotor, already done with bearings and Campbell diagram.

---

 

Now, if you would run an analysis, with command called plorb, it would give you error :

The orbits cannot be calculated.  Make sure there are elements supported for orbit calculations in your model (BEAM188, BEAM189, PIPE288 or PIPE289), and that these elements are selected and rotating.  The PLORB command is ignored.

---

• So just go back into the Workspace, and duplicate your model

 

---

• open your model in SpaceClaim - you will now see it as a model with SOLID structure - split it into parts, so each part is only a shape of a cylinder:

---

• After that step, you will have it seperated into cylinders, listed in corner as shown here:


• be careful to set topology (visible left down) as Merge

 

• 

---

• the next step is to transform these SOLIDs to BEAMs :


• 

---

• the result will look like this:

---

• Now you are ready to go back to Mechanical Environment. Dont forget to update the model.


• In Mechanical, change the way to see the full elements (not only as a Beam):

---

• Now you will have to do the same thing, as it would be modal analysis, or harmonics


• so dont forget to set attachment for bearings


• dont forget to put any boundary conditions


• and finally, use the right setting for velocity and select vector of rotation


• The mesh is different now, but dont worry about it, this is how analysis looks like (for more info check Timoshenko beam theory)

---

• now, to create Orbit plot, you will need to add this command into solutions :

/POST1

esel,r,ename,, 188 ! Select BEAM188 elements to produce orbits

set, 2, 5 ! Visualize orbits for test point 2, modal 5

/view,,0.5,1,0.5 ! Change view (x,y,z)

/ANGLE, , 45, YS, 1 ! Rotate view (around Y)

/show, png  ! Create png (file in dir), where to store result of orbit plot

/rgb, index, 100, 100, 100, 0 ! Set white background

/rgb, index, 0, 0, 0, 15

plorb ! CREATE ORBIT PLOT

 

---

• after the simulation, you can see now, what you have been looking for !

 

Let me know if something is unclear ! Good luck !

[Zdenek]

Hello Mr. Rwoolhou,

I am not sure, if that icon bellow your photo is a mark, that you are an employee of Ansys or not, so please excuse me if I am asking the wrong person.

I wanted to make a video tutorial, how to do an Orbital plot in Ansys Mechanical - its much easier than try to explain things with photos and text.

However, I am using Academic Research and Teaching licence. Is there any restriction to this type of licence, in the meaning of posting video explanations for this student community on youtube ? Or is it already a violation of users agreement ?

Or do you plan to implement some tool for uploading video directly in here ?

Thank you for your response in advance.

[Rob]

The ANSYS label does mean I'm an employee, and the purple star thing may also mean something. 

There are various terms in the Research licences regarding (not doing) commercial work, but I'd be very surprised if creating a YouTube video to help out on here would come under that. Just leave the ANSYS logos visible and I think that will be fine. Thanks for helping out. 

We do have plans to overhaul the community page, but I don't know what features that will give us at this point: I just answer questions! 

 

[shantashreejena97]

Hello zdendoslav,

I am extremely sorry for the late reply. I have tried your procedure. but I could not understand how to open my SolidWorks model in space claim as I have done al the analysis using design modeler. is there any procedure to change design modeler file into space claim file?

[Rob]

In Workbench duplicate the Geometry block and then right-click on the "Geometry" box. You should see the option to Edit with SpaceClaim.  The duplicate is simply to save your model if anything fails during translation: I don't expect problems but don't know how you've built your model.