I have done modal analysis and when ANSYS asked to input the start and end frequency i typed 150 as my starting frequency and 2000 as my ending frequency. No of modes to extract 10 and no of modes to expand 10. Due to no of modes ANSYS has only displyed 10 results. When i entered in postproc and results summary only 10 results were displayed and starting frequency was 150.01 to 150. 39. Now if i want to see all the frequencies how is this possible???Should i maximise the no of modes or is their any other option to view the results???
And how can i determine tht this is the most suitable frequency or structure should be prevented to achieve this frequency???
Thanks
Reply urgently
Yasir
Those seem awfully close
Those modes seem awfully close. Are you sure these are not high modes for the system, possibly?
It is rare that we would want to know all modes, and usually engineers ignore higher modes unless there is excitation expected at their natural frequencies. In a continuum system, there are infinite modes; in a finite element, there are as many modes as the number of unconstrained degrees of freedom.
To view results for all the nodes, I suspect you would have to change the range of frequencies to cover all the results and the number of modes to expand to the number of free degrees of freedom in your model. I am only a novice at Ansys, but this is how it should work from my understand and how it does work in other codes. In a large model, this does not seem reasonable to me to do this.
If I understand what you
If I understand what you have said correctly, you specified 10 modes. It most likely takes the least of what you have specified, a maximum of 10 modes with frequencies from 150 to 2000.
I dont know what they mean by extract and expand, google search didn't help either. Perhaps someone can enlighten me?
In reply to If I understand what you by Mikael Öhman
Re: Mode expansion in ANSYS
The modes that you get may depend quite strongly on the applied boundary conditions.
Here's a sample script that I've used to calculate modes in ANSYS:
/solu
antype, modal
modopt, lanb, 30, , , ,
lumpm, off
pstres, off
outpr, all
save, filename, db
solve
finish
/solu
expass, on
mxpand, 30, , , , ,
outpr, all
outres, all
solve
finish
The expansion pass is needed you you want to visualize the mode shapes. According to the confusing ANSYS manual
"In its strictest sense, the term "expansion" means expanding the reduced solution to the full DOF set. The "reduced solution" is usually in terms of master DOF. In a modal analysis, however, the term "expansion" means writing mode shapes to the results file. That is, "expanding the modes" applies not just to reduced mode shapes from the reduced mode-extraction method, but to full mode shapes from the other mode-extraction methods as well. Thus, if you want to review mode shapes in the postprocessor, you must expand them (that is, write them to the results file). ... "
-- Biswajit
In reply to Re: Mode expansion in ANSYS by Biswajit Banerjee
Thanks for ue help. I will
Thanks for ue help. I will tryo to do it...