Cancel
Showing results for 
Search instead for 
Did you mean: 

Inertia Relief problem setup in Femap

Creator
Creator

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

Re: Inertia Relief problem setup in Femap

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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:

 

inertia_relief.png

 

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/

Re: Inertia Relief problem setup in Femap

Creator
Creator

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.

Re: Inertia Relief problem setup in Femap

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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/

Re: Inertia Relief problem setup in Femap

Creator
Creator

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

 

Thanks you again!!! I really appreciate it.

Re: Inertia Relief problem setup in Femap

Creator
Creator

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..