Creating Flexible body in hm Optistruct

Hi Lokesh,

I have answered a similar question to one of your older posts. Please do check that. 

Sir i checked that but its not coming  like i am not able to limit the modes 

that is the reason i raised the question again

Please do help me with this

Thank You

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

Thank you so much..! i will check and let you know

Sir i am not using Motion View I am using Optistruct only to create Flexible bodies

and also sorry to say this file size is very huge and also i should not share the file 

I hope you understand

Thank you 

The definitions are the same regardless of the preprocessor used. 
 

 

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

Please see the discussion

https://community.altair.com/community?id=community_question&sys_id=b4668cf61b2bd0908017dc61ec4bcbc6

The definitions are the same regardless of the preprocessor used. 
 

from Practical Aspects of Multi-Body Simulation with HyperWorks

OptiStruct is used in the background to generate the flexbody. 

okay sir thank you i will try and let you know if any problem if i am facing

Sir this time i gave NMODES= 10 only but i got 112 modes which h3d file size of 5.54Gb and fbi 11Gb which i cant import in simpack to do the analysis

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. 

sir i am using hm 13 optistruct because when i tried with hm 14 that flexible body i cant import in simpack so i am using hm 13 only for creating flexible bodies

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

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:

 

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.

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

Sir but ASET's are required to generate the  markers in the SIMPACK software

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

@LOKESH KATARI

Please refer to Practical Aspects Of Multi-Body Simulation which is available at https://altairuniversity.com/free-ebooks-2/

ok sir thank you

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?

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).

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

The reason why it is not running the analysis for creating flexible bodies could be that there are already .h3D flexbody files created in the previous run.

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

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?

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

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

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

 

yes sir that is the only method for creating flexible body in optistruct..!  i guess

is there any other method than CBN for using flexible bodies?

@LOKESH KATARI

You can use Craig Chang method (CC method) which works without ASET

ERROR# 2839

For SIMPACK CMS generation the CMSMETH method CBN with ASET or CSET must be used..!

its showing like this

Use CBN with ASET