XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Defining load cases in Workbench
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Sat Aug 08, 2015 10:33 am  Reply with quote

Hi,

I want to simulate a steel structural component in Workbench for different load cases (about 10). Is there a method to do so?

Or the only way out is to create 10 different files with individual load case input.
_________________
Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Sat Aug 08, 2015 11:17 am  Reply with quote

On 08/08/2015 18:33, sushant.goel wrote:
Quote:
I want to simulate a steel structural component in Workbench for different load cases (about 10). Is there a method to do so?


Providing you are not using an antique version of Workbench Mechanical
then the answer is yes. In Analysis Settings>Number of Steps enter the
number of load cases. Once you have done this each of the loads will
become a table where you can input the desired value for a particular
load step.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Sat Aug 08, 2015 4:09 pm  Reply with quote

Quote:
In Analysis Settings>Number of Steps enter the
number of load cases


Dear Mr Liddle,

I am using Workbench 14.5 so this is possible.
I don't want to add these load cases. I want to evaluate results for each of them individually. I thought of using your approach of creating load tables and then unloading the structure to zero and then loading it to another separate load case [see image].

https://www.dropbox.com/s/kfxnxlvqsvyxm6j/loads.PNG?dl=0

So, these would be my 3 individual load cases. I am using non-linear steel and have non-linear contacts in the model. Will the unloading bring the model to initial [unloaded, undeformed] state?
_________________
Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
liam.mealey1
User


Joined: 08 Dec 2014
Posts: 7

PostPosted: Mon Aug 10, 2015 12:36 pm  Reply with quote

You'll have to check your own model to see if removing the loads returns it to an undisplaced/unstressed state before reapplying the next load case. (I can't access Dropbox, so can't see your model)

There are a couple of ways if you want to setup several models to run within the same project page. The easiest is probably to duplicate them on the project page - if you right click on the 'Results' box within any project panel, it duplicates everything prior to the results. If you open mechanical it will have one set of conditions for all of the geometry, mesh and contacts, and a then an individual tree for each of the loading cases, all accessible from within the same mechanical session.

The other way is to setup and control parameters from the project page, though you should probably look through the manual for that as there is a bit too much in it to include in one forum post.
_________________
Liam Mealey
OneSubsea, Leeds, UK
Back to top
View user's profile Send private message
aaron.caba
User


Joined: 30 Aug 2011
Posts: 157

PostPosted: Mon Aug 10, 2015 1:31 pm  Reply with quote

If your material and contacts are non-linear, just returning to zero load may not take you back to your original configuration or material state, e.g. if your material has any pasticity.

So another way to reuse the mesh and materials is to use different systems on the project page. Just drag a new system onto the "model" like this:
https://dl.dropboxusercontent.com/u/106368051/Capture1.PNG

Then you can apply different loads and boundary conditions like this:
https://dl.dropboxusercontent.com/u/106368051/Capture2.PNG

Aaron
_________________
Aaron C. Caba, Ph.D.
Sr. Member Technical Staff
Nuvotronics, Inc.
7586 Old Peppers Ferry Loop
Radford, VA 24141
http://nuvotronics.com/
Back to top
View user's profile Send private message
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Sun Nov 01, 2015 11:46 am  Reply with quote

Quote:
There are a couple of ways if you want to setup several models to run within the same project page. The easiest is probably to duplicate them on the project page - if you right click on the 'Results' box within any project panel, it duplicates everything prior to the results.


This works fine.
Thank you for the responses Liam and Aaron.
_________________
Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Fri Dec 11, 2015 11:12 am  Reply with quote

Hi again,

I am using the procedure mentioned in last post for defining different load cases. I am getting an error when I try to save the Workbench file after adding a stress or strain plot to the 'Solution' tree. Please see the attached image for error information.

https://www.dropbox.com/s/5whbiy15izt37sm/151211.PNG?dl=0

I tried to resolve this using the information provided at this link-
https://www.dropbox.com/s/5whbiy15izt37sm/151211.PNG?dl=0

But it doesn't work and I get the same error. I have to go to Windows task manager and 'End Task' Workbench. Does anyone have a solution for this?
_________________
Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron