NASTRAN output coordinate system 1

[jmarcoj]

Hi everybody,

I am working with NASTRAN and I have a problem.

When I use CQUAD4 elements, the stresses are given in the element reference system. That reference system is computed by NASTRAN using the element diagonal bisector method. Basically, the x-axis is between the node2 and node3 of the element. Usually that coordinate system is not the one you want your output printed in.

The question is, is there any way to get the output printed (*.f06 file) in the coordinate system you want?

I have already tried using the material angle and in that way I can transform all my output in that coordinate system using a post processing code but I'd like to have the stress printed in the *.f06 file in the coordinate system I want.
I also tried using the OUTRCV command but that command works only with p-element and that is not my case, then it does not work.
Hope somebody can help me out.
Many thanks in advance.

Kind regards,
Marco

 

[40818]

You can output a report file in a coordinate system of your choice.

 

[jmarcoj]

Thanks for your reply but how can I do it?
I have been reading the guide but I can't find anything about that.

 

[40818]

Thinking about it, you can modify your nodes analysis coordinate system and analysis coordinate system to a coordinate system of your choice.

Element/modify/node/edit, then tick the "analysis coordinate frame" and "refer. coordinate frame", then give them the coordinate system of your choice.
I think then the output in your F06 file will be in that coordinate system.

Otherwise:

Results/create/report/overwrite file,
then select stress tensors, select positions (Z1, Z2 etc) and the quantities.
Use the normal results tabs to select your elements and then use the tab to select your coordinate transformation.

You will then get yourself a report containing all the info you want in your coordinate frame.

Hope that helps.

 

[jmarcoj]

The node coordinate system is the right one, the problem is that stresses are printed in the CQUAD4 element coordinate system which depends in the way the nodes are numbered. For that reason displacements are in the right coordinate system, but stresses are not.

I tried using:
PARAM,S1M,1
which is suppose to make NASTRAN give the stresses in the material reference system but, I do not know why, it does not work.

I also tried using:
PARAM,CURV,1
which should do the same thing of the previous one, but this does not work, either.

For what concern the report file I think it is a really good idea but I do not use patran, I use femap and I cannot find any option like that. Do you know NASTRAN commands to make it print that file? It would be really helpful.

PS I am running a non-linear analysis. SOL 106 or SOL NLSTATIC; and usually this problem happens when you use a orphan mesh, i.e. a mesh that was created by hand and equivalence of nodes.

 

[40818]

Just had a thought at home:

Cant remember how to do it at the moment, and dont have the Nastran manuals on my laptop so i might be wrong, but;

The results in the F06 file will be the unaveraged centroidal stresses of the element. I think if you request for nodal stresses in your output, and give the nodes the right coordinate analysis system and reference system, then in your F06 you will get the stresses plotted at each grid point in the alignment you want.

Might be wrong as i've had a glass or two of wine.
I will have a further ponder back at work tomorrow in the morning.

 

[jmarcoj]

You are right, the default option for stresses is:

STRESS(SORT1,PRINT,REAL,VONMISES,CENTER,RPRINT)=ALL

Where CENTER means that, for CQUAD4, the stresses are given at the centre only.
I have already tried using the option CORNER instead of CENTER to have also the stresses at the corner of the element but it didn't work.
I still obtain the STRESSES in the element coordinate system:
S T R E S S E S I N Q U A D R I L A T E R A L E L E M E N T S ( Q U A D 4 ) OPTION = BILIN

ELEMENT FIBER [highlight]STRESSES IN ELEMENT COORD SYSTEM[/highlight] PRINCIPAL STRESSES (ZERO SHEAR)

I think there has to be an option in the bulk data section that chances the output coordinate system but the ones I tried didn't work.

 

[40818]

Not sure why PARAM,S1G,1 wont work to give you grid point stresses for quad4. But this might work: you should be able to print or punch the results in the material coordinate system by OMID=YES, but this is not supported by pre-post processors so your OP2 or XDB are not changed.
Otherwise i'm stumped.

 

[jmarcoj]

Thank you very much indeed for your valuable help.

PARAM,OMID,YES does work with the linear solver 101 and that solves half of my problems
Unfortunately it doesn't work with the non-linear solver 106 although in Nastran manual it is written it does I keep getting the stresses in the element coordinate system when I run a NL analysis.

If you hear something about an equivalent parameter that works for NL analyses please let me know.

Kind Regards,
Marco