turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- How to load a beam model with a sine shaped deform...

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-04-2014 06:38 AM

I would like to simulate the stresses when a beam is forced in a particular shape. In this case the shape is the half of a sine. At the moment I can only think of the following way: Add nodal displacements as loads to multiple nodes and tell the load definition to look into a data surface to find the correct position.

I hoped that I could just use the x-position as variable in the load definition, but it don't seems to be available, the variable and/or equation fields stay greyed out (?).

Can anyone give me more information on how to apply loads that vary along a certain axis?

Furthermore I would like to simulate the behavior when the sine shape moves though the model. I can perform advanced analysis so time dependency is an option. Experiences with this are welcome.

8 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 08:44 AM

Dear Rob,

If i well understood, you want to import translation data from sine analysis and apply them on another analysis. Assuming that you have the same nodes IDs between the two models

. Start by listing all the translation for all the nodes under the sine results.

Then, go to Femap, Create a New Nodal Load Set. Choose displacement and put 1 in Tx direction. Under Method choose Data surface / and arbitray 3D. Past your nodal results (from excel, csv..) Note that the three first column are nodes coordinates and the fourth is your Tx displacement. Hit Ok and you're done. If you want to visualise a contour plot of your loads create a new output set, activate it then go to model / output / from load and choose displacement. You will see that displacement output vectors are generated. F5 / contour / choose the Tx disp for example and judge your inputs values...

Regards,

SN

Seif Eddine Naffoussi, Stress Engineer

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 09:54 AM

Hello SN,

Thanks for your reaction. You explained the use of a data surface, but I would like to make is more parametric.

I have three shapes in Excel, see image. The equation per shape are known and my idea was to give in the equation in Femap, somewere...

My model consists of multiple beams, each node is supported by a DOF spring. The beams simulate a pipe, the springs are the ground. the length of one beam is half the diameter of the pipe. At specific positions, I would like to add a displacement, with a value that lies on the curve.

Is there a function type that can use the x-position to calculate the vertical position and then use this value for the load?

Goal of the model is to compare the bending stress in the pipe when it is forced in a certain shape, and to find out the effect of prescribing the displacement on only a few points.

Hereby also a snapshot of my model, which is much longer than only this detail.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 10:17 AM

In Femap you can create a function where you could define a known equation and then Use this function when defining the load set. Instead of data surface you can select variable and lick on advanced to define your equation.

I attached a pdf file which explain how to define an equation loading to a tank based on the h position.

Look at the pdf file for more details. Note that at the end you will find a direct link to watch the video.

Hope this will help you

SN

Seif Eddine Naffoussi, Stress Engineer

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 10:22 AM

Hello Rob,

If you have analytical definitions of loads, you can repeat exactly what SN said, except check "Variable" for Method, you can then enter an equation which, for example, references node positions via functions XND, YND, or ZND.

Read these sections in the Help:

- Commands 4.3.3.2 "Model, Load, Nodal" > "Choosing a Load Creation Method"

NB: don't miss this: "you must select a variable (default is i"

=> this means that you must write xnd(!i) , as shown a few lines below

- User Guide > C.Function Reference for the available functions when writing an equation.

AP

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 10:28 AM

the variable option is grayed out somehow? I have tried different options for the load definition but it stays this way.

I will look into your suggestions Astrium_tls, but first I have to find out why I can't use the equation option.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 10:31 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 10:51 AM

unfortunately it is only available for elemental loads and nodal loads that are "per node". Nodal loads that are total (i.e force, moment, etc) and per length (force per length, etc) must be constant.

But for what you want to do, the function does it well.

Seif Eddine Naffoussi, Stress Engineer

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

06-05-2014 11:14 AM

This works indeed, easy that one can use the Value field! Also a equation data surface is a good option.

But... all these options have a 'Static' behavior; once the value for the displacement has been calculated, the value field gets a constant value. For example when I make use of a data surface, I can change the equation of the data surface but no load will change as a result.

I think I have to make an enhangement request for this..

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc