×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Seismic Analysis

Seismic Analysis

Seismic Analysis

(OP)
I am doing seismic analysis using ANSYS 5.7.
After doing response spectrum analysis to find responses(displacement and stresses)for three INDIVIDUAL spectra (say in X,Y ,and Z directions)using SRSS mathod of combination,how to get the COMBINED RESPONSE DUE ATO ALL THE THREE SPECTRA ?How to proceed in the Postprocessor?please help.

Thanks in Advance
brc01

RE: Seismic Analysis

Hi,
This is infact a question back to you. I have a similar problem now. I saw your question when I was searching for seismic analysis.
As far as I know it, the 3 directions are independent in terms of the response and has to be given as such. I've no knowledge of any combination of the 3 response spectra.
In case the 3 have to be combined and there is a way to combine the 3, please let me know.
Thanks in advance,
jharish

RE: Seismic Analysis

(OP)
The three have to be combined coz an earthquake shakes your structure SIMELTANEOUSLY in all the three directions.

Well,COSMOS uses "SRSS:Square root of sum of squares"method to combine these responses to get the net response.I am not sure if anything similar is there in ANSYS.

RE: Seismic Analysis

How do you specify the exact position where you want the earthquake to act.How do you input the earthquake data (eg. Northridge) for the spectrum analysis. I have tried using the commands from the ansys eXAMPLE INPUT VM70 input listing and it only applied the earthquake load to one side of my model. Please help

RE: Seismic Analysis

The earthquake inout is given at the fixed locations on the component. Say, the component that has to be tested for seismic compliance is bolted to a frame, the seismic input has to be given to the bolts, after giving a suitable constraint while doing the modal analysis. The seismic procedure also depends on the type of input spectrum you have.
Hope this helps.
-Harish-

RE: Seismic Analysis

The complete combination of the X, Y and Z directions is carried out in ANSYS using the

lcoper,srss,all

command (subsequent to setting the three loadcases as a loadcase definition - lcdef).

RE: Seismic Analysis

Drej,
Ordinary loads and reactions can be combined using the SRSS method. But my question is whether the same procedure can be followed for a seismic analysis. I'm questioning this as all the test reports I've seen come with separate response curves for the 3 mutually perpendicular directions. So the question still stands... Can it be done for a seismic analysis. Sorry for being so persistent, but it's vital for me.
Thanks.
-Harish-

RE: Seismic Analysis

If you are performing a SPECTRAL analysis, you MUST combine the three directions after the modal responses have been combined. The combination of modes is performed by inputting the .mcom file in a /post1 session, using /input,filename,mcom. (If you specified CQC combination, the responses in each direction will be CQC'd by inputting this file, but will also SRSS the responses as well at the end - check the list of .mcom file commands by opening it!). Anyway, you must combine the three directions together after this - why? What happens when a seismic event occurs? all three directions are shaken simultaneously - not individually. Once you have this, you will have what is known as the Complete Sesimic Case (but you will need to factor these loads if you are using a code).

Hope this helps i happy ANSYSing

  - - D R E J - -

RE: Seismic Analysis

If you are performing a SPECTRAL analysis, you MUST combine the three directions after the modal responses have been combined. The combination of modes is performed by inputting the .mcom file in a /post1 session, using /input,filename,mcom. (If you specified CQC combination, the responses in each direction will be CQC'd by inputting this file, but will also SRSS the responses as well at the end - check the list of .mcom file commands by opening it!). Anyway, you must combine the three directions together after this - why? What happens when a seismic event occurs? all three directions are shaken simultaneously - not individually. Once you have this, you will have what is known as the Complete Sesimic Case (but you will need to factor these loads if you are using a code).

Hope this helps - happy ANSYSing

  - - D R E J - -

RE: Seismic Analysis

Hi,
 I am doing similar analysis.
Can any body help me as what exactly to look for in Seismic analysis for PSD input viz. the displacement or 1 sigma stress. Also when I go for /post26 my screen shows that the initial memory allocation has been exceeded and the ansys window goes off. I am using Ansys 7.0.I have 108000 elements in all.Has anybody faced a similar kind of problem?

Thanks in advance.
Bhawesh.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources