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
- Inertia Relief problem setup in Femap

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
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2014 04:10 PM - edited 08-20-2014 04:21 PM

Hello everyone,

I was wondering if anyone used this feature in Femap with NX Nastran. I tried looking for some tutorials on this but had no luck. It would be great if someone help in setting up interia relief problem.

Look forward to hearing from you..

I tried on some basic model which has a rigid spider on both ends. One end of the spider has a fixed constraint boundary condition (all 6 dofs are fixed)and the other end subjected to a force. It runs fine if I just run static analysis but if use the parameter inertia relief in bulk data entry then it throws a fatal error

**A SUPORTI BULK DATA ENTRY IS NOT PRESENT FOR INERTIA RELIEF ANALYSIS (PARAM,INREL,-1). **** ^^^ USER ACTION: REMOVE PARAM,INREL,-1 OR SPECIFY A SUPORTI BULK DATA ENTRY. **

Dont know how to modify the constraints that could able to run this feature.

any help is appreciated.

Thank you in advance for help,

na

5 REPLIES

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

08-21-2014 03:32 AM

Dear Na,

It seems to me that you have used the manual inertia relief method where the SUPORT entry must be specified explicitly along with PARAM,INREL,-1, no, better use the automatic method.

The automatic inertia relief method is the recommended inertia relief method. With the automatic method, the specification of the SUPORT entry is no longer needed. To turn it on, simply add **PARAM,INREL,-2** to the input file. The reference frame is selected automatically, in a manner that poor solutions are unlikely because of the choice of reference frame variables.

In the NASTRAN BULK Data Options select the AUTOMATIC method:

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

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

08-21-2014 02:20 PM

Thank you so much Blas for helping me with the graphics. I really appreciate your help.

It did help me to resolve my problem.

I have a another question though. i have seen some people using this WTMASS (with factor 0.00209 or something like that)option as a part of inertia relief FEA setup. I was wondering if you know anything about it.

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

08-21-2014 03:34 PM

Dear na,

In some cases, you may want to use the WTMASS parameter to express the mass in terms of weight units instead of mass units. The WTMASS parameter multiplies the assembled mass matrix by the scale factor you specify with the WTMASS parameter.

For the steel example, you can enter the mass density a weight density of 0.283 lb/in3 with a WTMASS parameter of 0.00259 (which is 1/386.4). However, if you enter any of the mass in terms of weight, you must enter all the mass in terms of weight. The WTMASS multiplies all the mass in the model by the same scale factor, with the only exception being the mass you enter in Direct Matrix Input.

I run SI units where we don't need to use at all the WTMASS parameter.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

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

08-21-2014 03:54 PM

Thank you Blas for sharing some insights in WTMASS parameter. This clarified some of my misconceptions.

Thanks you again!!! I really appreciate it.

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

08-21-2014 04:13 PM

Hi Blas,

Thanks again for those quick replies. I am new to Femap so experiencing some basic transition problems and this is my first inertia relief simulation ever.

Hey, by the way, I successfully ran one inertia relief simulation on 3D model and it shows von mises stress approximately 78% less( 36 MPa for inertia relief vs 169 MPa for normal static) than the regular static analysis with constraints(fixed 6 degrees of freedom) . Are these results trustworthy. is it common? How do we actually validate these results.

For regular static analysis we can validate by some approximate hand calculations. I was wondering is there any way that we can validate the inertia relief problems. Do you have any help files that shows some basic calculation.

It would be great if you could share some of those files if you have any. Hey stop me if I am asking you too much.

I visited your website for some reference but its not written in english so i couldn't understand anything.

Thank you again for valid inputs..

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc