Create an MNF File with stress and strain for Adams/Car

Altair Forum User

Hello,

 

is there any posibility to create an mnf file directly from Optistruct or must I use Motionview to translate the h3d file to an mnf file. When I do it with Motionview I have no information about stress and strain so i can't see the eigenmoden in Adams/view.

Is there any instruction for this problem?

 

My main problem is that I would like to have the displacements in the mnf file to build an flexible suspension model in Adams/car. Is this information in the mnf file created with motionview?

 

Thank you,

Erik

Altair Forum User

Hi Erik,

 

When you translate H3D to MNF file, Stress and strain modes are not translated to MNF. Please refer to MotionView help for details.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Hello,

thats what I already know. But is there any other otpion to get stress and strain in an MNF file? Or should I save it as an abaqus File and do it with this program, because there it works.

Rahul_P1

Erik,

 

Optistruct can output a .mnf file, 

 

This file is created when OUTPUT, ADAMSMNF is presented during flexible body generation.

 

note - If GPSTRESS output is requested in addition to OUTPUT, ADAMSMNF, then nodal stress results for solid elements will be written to the .mnf file.

Altair Forum User

Hello Rahul,

 

Ok, thats the first point when I wrote MNF into the search window. I also included the required dci units card but there is no mnf created. Only the normal h3d, hm, out and other files are visible.

There is no error massage when I analysed my model and I can normally have a look at the eigenmodes in Hyperview.

 

Please help me to get the mnf file by analysing an normal meshed model with the eigrl loadstep.

Altair Forum User

Hi ErikBia,

 

Have you included CMSMETH load card in the model?

 

if not please add CMSMETH card and check if that helped.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Hello Prakash,

I tried to include the CMSMETH Card by following the OS-1930 Tutorial. I find no possibility to end the simulation wthout an fatal error neither to get an MNF file out of it. I also used the OUTPUT card with ADAMSMNF. Can someone analysed my control arm model similar to that one in OS-1930 and show me how to get an mnf file out of it?

Altair Forum User

Hi ErikBia,

 

could you share your model with us?

 

Please use the dropbox link in the below signature to share the model.

Altair Forum User

Hi,

 

did you get my model?

Altair Forum User

Hi Erik,

 

Thank you for sharing the model

 

I will look into this and get back to you soon /emoticons/default_smile.png' alt=':)' srcset='/emoticons/smile@2x.png 2x' width='20' height='20'>

Altair Forum User

Hi Erik,

 

I am able to generate MNF file at my end..

 

I will share the .mnf file with you through FTP. Please check and let me know.

Altair Forum User

Hi,

 

I’m in a similliar Situation.

 

I want to export a mnf file from HyperMesh (optistruct) to ADAMS View.

To simulate a pressure on a surface in ADAMS  I tried to applicate a force to a depended node of a RBE3 element set.

Therefore I created an ASET constraint for this point with all 6 DOFs in HyperMesh (Optistruct).

 

If I create a mnf file by running Radioss or Optistruct, I get the following error for all 6 DOF of the RBE3 depended Node:

A dependent d.o.f. of rigid elements is constrained in an SPC set.

 

Can anyone help me to solve this Problem?

 

Thanks a lot!

Altair Forum User

Hello,

Did you changed under analysis - loadtypes - constraint to ASET? You have to do this before you build up the constraints in your loadcollector named ASET.

Altair Forum User

I have another Problem occured in my model.
 I have build up our monocoque with composite material. When I wanted to get stress in my MNF File I have to choose the GPSTRESS Card. But when I start the analysis the Out.file tells me:

*** WARNING # 2505
 Corner stresses are not calculated for composite elements.
 Zero values will appear.

 

How can I get stress in my MNF file by using composite elements?

Altair Forum User

Hi Erik,

 

I think you will get the nodal stresses with GPSTRESS for composite material but corner values will be ignored.

Altair Forum User

Hey to everyone who have the same problem:

I finally managed to get the MNF files working with adams.

The best way is to do it like in the the Tutorial 'OS-1930: Generating a Flexible Body for use in Altair MotionSolve'. To find it go to the Hyperworks help home window an enter OS-1930 into the search window.

There is an example about an already meshed control arm. With the Eigrl card it doesn't work, so you have to use the CMSMETH Card like described in the tutorial. The Only thing you have to change is in the OUTPUT card you have to choose ADAMSMNF instead of H3D. The other thing is to change the 'Global Output Request' Control Card form STRESS to GPSTRESS so that the reduced system will claculate stress and strain.

In the CMSMETH Card you can chose your reduction method and how many modes you like to transfer. Notice that only the craig-bampton and craig-chang method can be used for creating mnf files.

For more background information you can get some information about the 'component mode synthesis'. After these informations you will understand how an MNF file is build up.