Jump to content
LOKESH KATARI

Creating Flexible body in hm Optistruct

Recommended Posts

I am creating flexible body in optistruct of a truck chassis with trailer which is very big model with so many number of nodes and elements.

CBN method is used UB_FREQ given 20

but i am getting 131 modes and fbi file size is about 15GB which is too much to import in SIMPACK

and then i gave NMODES 40 but still its giving 131 modes which is very high

So please help me with this

Thank You

Share this post


Link to post
Share on other sites

Hi @LOKESH KATARI

 

MotionView allows you to specify a limit on the modal information contained in your H3D file. Two methods are available to set these limits. You only need to define frequency upper bound or number of modes, not both.

-Specify a maximum number of Eigen modes for which modal data is included in your H3D file.

OR

-Specify an upper cut-off frequency for the Eigen modes. When a cut-off frequency is specified, normal modes analysis can be performed using one of two algorithms: Lanczos or the automated multi-level sub-structuring eigenvalue solution, AMSES.

 

 

You can manually insert certain cards in the Optistruct input deck to run the Component Mode Synthesis routine. These cards allow file size reduction of a flexbody. This helps in faster pre/post-processing and overall better efficiency of the process.

You can manually edit the preparation file generated by FlexPrep to reduce the size of the flexible body H3D. By modifying the input deck, you can:

•request only the skin elements of the flexbody to display .

•request stress and strain information for a selected set of elements.

•use released degrees of freedom for the interface nodes.

 

If the problem persists please share the model

LOKESH KATARI likes this

Share this post


Link to post
Share on other sites

The definitions are the same regardless of the preprocessor used. 
 

Quote

 

Use Released DOF method to keep the number of CMS modes low for models that have a large number of interface nodes.
For example, release the rotational degree of freedom for a revolute joint. The released DOF (degrees of freedom) feature
enables the user to free some degrees of freedom of the interface nodes which removes modes that are unnecessary to

describe the motion of the flex body, thus reducing the flexbody file size. If the appropriate DOF are released for a particular
interface node the simulation is not affected in any way. The DOF released will depend on the kind of kinematic constraint
applied at the interface node. For example, a revolute joint has one DOF in the MBD model. This DOF can be released in at
the interface node, since there is no constraint to apply a torque in this direction. The modal information in this direction
is useless to the simulation. Similarly, for a ball (spherical) joint, the three rotational DOF can be released for the same
reason.

 

from Practical Aspects of Multi-Body Simulation with HyperWorks

Share this post


Link to post
Share on other sites
Guest

Hi,

 

Please let me know the version you are using and the method as well so that I can check with the dev team on the same. 

Share this post


Link to post
Share on other sites

How many interface nodes are in the model? Try to reduce them to see if it affects the number of modes. 

 

From Practical Aspects Of Multi-Body Simulation with HyperWorks:

Quote

 

9.3. Component Mode Synthesis CMS Methods
There are two CMS methods supported in Optistruct that will reduce the FE model to a set of orthogonal mode shapes.
• Craig-Bampton – In this method, two sets of modes are computed:
- the fixed interface constraint static modes are calculated by applying a unit displacement at each interface node in
each degree of freedom individually while leaving all the other constraints active.
- the fixed interface eigen modes are calculated with all the interface nodes constrained (# of modes is specified by
the user)
Finally, the both sets of are orthogonalized producing the modal matrix of modes shapes that represent flexible body.


• Craig-Chang – In this method, two sets of modes are also computed:
- the inertia-relief attachment static modes are computed by applying a unit displacement on each interface node in
each degree of freedom individually while all the other interface nodes are free. When calculating the static modes
the model is “mathematically” constrained by inertia, hence inertia-relief, to produce structural deformations required
for calculating the mode shapes.
- the free-free eigen modes are computed (i.e., without any constraints on the body)
Again, both sets of modes are orthogonalized producing the producing the modal matrix of modes shapes that represent
flexible body.


9.4. How To Choose The CMS Method?
Craig-Bampton - best when most of the degrees of freedom of the interface node are constrained by the MBD model.
Craig-Chang - best when most of the degrees of freedom of the interface nodes are not constrained in many degrees of
freedom by the MBD model.
Further Details on the CB, C-C CMS Methods
Craig-Bampton and Craig-Chang modes are not the same modes as calculated using conventional normal modes analysis.
They may look similar, but strictly speaking will not compare exactly with a normal modes analysis.
The number of modes generated to represent the flexible body is equal to:
• number of degrees of freedom restricted for each interface node (static modes) +
• the number of fixed interface or free-free eigen modes (user requested)
For example: 4 interface nodes * 6 modes/node + 10 fixed interface or free-free eigen requested modes = 34 modes
calculated by OptiStruct.
Note: The default number of restricted degrees of freedom for each interface node is 6 DOF (fixed joint) in FlexPrep, but can be
edited manually in the preparation file
As the number of fixed interface or free-free eigen modes calculated increases so does the accuracy of the solution and the two
methods describe above converge. The number of fixed interface or free-free eigen modes to use as well as which method to
use it dependent of the problem at hand, and the determination of what works best for a give problem requires trial and error
and experience.
Rule of thumb: start by including modes with frequencies at least 2x the frequency

 

There is no explanation on how modes are computed for CBN method.

Share this post


Link to post
Share on other sites
Guest

Hi,

 

As explained in one of the previous posts, 

if you remove the ASET you should get the same number of modes as specified in NMODES.

 

The extra modes are the number of FEM DOF that are in the interface

Share this post


Link to post
Share on other sites
20 hours ago, Ivan said:

How many interface nodes are in the model? Try to reduce them to see if it affects the number of modes. 

 

From Practical Aspects Of Multi-Body Simulation with HyperWorks:

There is no explanation on how modes are computed for CBN method.

sir thanks for your time and explaining this..! now i clearly understood 

can you share any material regarding the above explanation which you gave?

it would be helpful for me

thank you

Share this post


Link to post
Share on other sites
On 11/14/2018 at 2:52 PM, Ivan said:

How many interface nodes are in the model? Try to reduce them to see if it affects the number of modes. 

 

From Practical Aspects Of Multi-Body Simulation with HyperWorks:

There is no explanation on how modes are computed for CBN method.

Sir you are talked about NMODES. 

Now my doubt is :

What about the UB_FREQ ?? can we control the no of modes with UB_FREQ?

 

Share this post


Link to post
Share on other sites

Yes, we control the number of modes with either NMODES or UB-FREQ. NMODES explicitly defines the number of modes, while UB_FREQ defines frequency upper bound, i.e. all modes below the specified frequency will be included (note that we usually do not know in advance the number of nodes below certain frequency).

LOKESH KATARI likes this

Share this post


Link to post
Share on other sites
On 11/20/2018 at 2:05 PM, Ivan said:

Yes, we control the number of modes with either NMODES or UB-FREQ. NMODES explicitly defines the number of modes, while UB_FREQ defines frequency upper bound, i.e. all modes below the specified frequency will be included (note that we usually do not know in advance the number of nodes below certain frequency).

one question Sir:

1) In hm 13 if i am not giving ASET's its running the analysis for creating flexible bodies.

2) In hm 17 if i am not giving ASET's its not running the analysis for creating the flexible bodies.

so which is correct and why?

awaiting for your reply

Thank you

Share this post


Link to post
Share on other sites
Guest
23 hours ago, LOKESH KATARI said:

2) In hm 17 if i am not giving ASET's its not running the analysis for creating the flexible bodies.

 

Are you using the same methods for in 13 as well?

2 minutes ago, LOKESH KATARI said:

oh okay..! but ,u question is..! is it necessary to give ASET for creating flex body?

If you don't need a constrained body, you can ignore ASET

 

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...