FEMAP deformed model coordinates 2

[TheBrx]

Hello to all! I've been watching this forum for a while and must admit it helped alot...

Now I have a question to ask...

Is there a way to export a deformed model node coordinates? I.e., I have a deformed and analyzed model, and now I want to use that deformed model as a new model for another analysis...well, something like that...

If anyone has an idea, please share it...

Thanks and regards!

 

[trainguy]

I know it's possible, but can't recall how. However, if you have no-linear (geometric) capability, you my not need to do this.

What exactly are you attempting?

tg

 

[rb1957]

i think the easiest way is to use the f06 file ... use the displaced shape as the new co-ords ...

1) export a NASTRAN BDF of your model
2) run the model "print and post-process" output option
3) from the f06 file you'll have a listing of grids in their displaced shape
4) copy this table into the bdf overwriting the original grid co-ords
5) import this editted bdf into Femap and analyze ...

Quando Omni Flunkus Moritati

 

[rob768]

is it not easier to use the output of a first run (the "save databse for restart" option)?
Save you editing and the chance of errors.

 

[rb1957]

if you ran geometrically non-linear ?

Quando Omni Flunkus Moritati

 

[BlasMolero]

Hello!,
1.- After solving your model run the macro under "CUSTOM TOOLS > POSTPROCESSING > Nodes Move by Deform with Options" command. This will update your model grid nodal coodinates with the deformed shape.
2.- Then you can export your DEFORMED model in nastran format using "FILE > EXPORT > Analysis Model" command.
3.- Alternatively you can export your deformed mesh using "FILE > EXPORT > GEOMETRY > Stereolithography (*.stl)" command. The stereoli­thography file is only applicable for a meshed model. FEMAP will export a faceted representation of your model using the FEA mesh as the basis of this file.
4.- Or if your model is shell based you can generate geometry based in your deformed mesh!!. Yes, in fact, this is a new feature of FEMAP V11, using command "Geometry > Surface > From Mesh..." will attempts to create a surface from any number of selected shell elements.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[TheBrx]

"1.- After solving your model run the macro under "CUSTOM TOOLS > POSTPROCESSING > Nodes Move by Deform with Options" command. This will update your model grid nodal coodinates with the deformed shape."

Mr. Blas Molero......really, the true spirit of FEMAP

Thanks and best regards!
Brx

 

[GruntCZ]

Hi Guys!
I have a similar problem. Is there a way, how to export plastically deformed model in to another analysis? So don't use elastic deformation. For example flange deformed by pretensioned bolt, and then by inner pressure and elevated heat.
Or is there any other way how solve this kind of issue?

 

[jbrackin]

A few things to consider:
If you deform the model using the displacements to create a new model, then you are starting the next analysis at zero stress, but with a new undeformed shape. Is that really what you want to do?

If you really just desire to apply a loading history with different loads being added or subtracted as you continue the analysis, then you just need to create subcases in the nonlinear solution. Each subcase should completely define the loads desired for that subcase, in other words, do not add an "incremental" load, apply the total load desired for that particular subcase. Nastran will automatically find the "delta" load by comparing to the previous subcase.

subcase 1 = preload only
subcase 2 = preload + mechanical load
subcase 3 = preload + mechanical load + thermal load

If you wanted to investigate different loading scenarios,and your model is large so that run times are an issue, then set up a run to apply preload only and save the nastran database(scr=no)
Now do a "read only" restart from that run to apply different mechanical loadings as desired.

I would only suggest restarts for experienced Nastran/Femap users.

 

[Flev]

Hello!
I have the same problem.
I have tried to do a restart analysis but it seems that Femap can't read the new loading.
I have run a SOL 106 with "Save Database for Restart" option flagged.
The solution is converged

Then, I have created a new analysis with "Restart Previous Analysis" flagged and with different boundary conditions, but the results are the same of the first analysis without any trace of the second loading conditions.
Where is the problem?

Flavio

 

[jbrackin]

We would need to see at least the case control sections of both the original and restart decks to understand what is happening.