local coordinates system

[ananthaces]

Hello everyone. I have to define a local co-ordinate sytem in my model. Wjat i did was modified the material angle. is that the right way to do? by default would i be getting all the stresses in the local or global direction? if i get it in global how do i get the results in the local coordinate. is there a way i could switch my solutions back forth between local and global? thanks.
Ananth

 

[SWComposites]

What FEA software and pre/post-processor software are you using? What version? No way to answer your question without this info.

 

[ananthaces]

i am using Femap/Nastran 8.3...actually whati have done is, i updated the material angle so that each of the shell plane in my model falls on the x-y plane. next in the nastran editor i changed the setting in the reuslt process parameter to basic( which menas global) and then i ran it.next i changed the setting to element( which means element co-ordinate system) and i ran.i am getting the same result for both types which is weird. So, i was wondering if i update the material angle to rotate the global x-axis is enough? thanks.

 

[GBor]

Since you say FEMAP with Nastran 8.3, I'm assuming NENastran. You can change from global to local, but what you may be looking for based on your description is "material" coordinate systems. It sounds like you left the "element coordinate system" aligned with the global coordinate system (hence the same results for the two) and compensated for the offest between element and global by altering all the material angles. That is one way to do it and it valid (although maybe not "elegant"), but you may need to look at "material" coordinate system instead of element.

Garland E. Borowski, PE

 

[ananthaces]

you are right gbor i am using nenastran.i changed the settingd to material under result process paramteres in ne editor but i still get the same solution for both the cases.is there any other settigns in femap i got to use b4 i cld see the contours. Thanks

 

[GBor]

May be my mistake on the "material" coordinate system. Now that I think about it, that may be your laminate orientation...in other words, you may need to set your local coordinate system and tie your laminate to that local coordinate system. For a laminate, however, you should be able to see ply-by-ply stresses which should change depending on your orientation, unless you entered "smeared" properties. The ply-by-ply stresses would be relative to the global or element axis. It's been a while since I played with this...someone else may need to take over for more detail...Frank Meyers seems to know what he's talking about (fkmeyers). Also SWComposites.

Garland E. Borowski, PE

 

[ananthaces]

hope to hear from them soon...

 

[ananthaces]

hey gbor..is there a way to plot the internal forces in nenastran..or the nodal forces...thanks

 

[GBor]

Try this link to one of NENastran's tutorials:

http://www.nenastran.com/newnoran/p...s&&filename=04_TUTExtractingInternalLoads.pdf

If for some reason is doesn't work, log in (registration is free), follow the "knowledge database" and select tutorials. This is one on "Extracting Internal Loads". It should be helpful.

Garland E. Borowski, PE

 

[ananthaces]

Thanks gbor. i really appreciate your concern.

 

[GBor]

Hope this works for you...

Garland E. Borowski, PE

 

[SWComposites]

I think you need to read the manuals again in regard to material angles. See the section for CQUAD4 elements in the NE/Nastrain Reference Manual and the section for defining material angles in the FEMAP Commands manual. When you define a material angle in FEMAP you are not rotating any coordinate systems, rather you define a vector direction or coordinate system axis which is then projected onto each element and the material angle for each element is then calculated. This angle defines (for each element) a local coordinate system for stress/strain output. NASTRAN actually has the capability of defining material angles by reference to the x-asix of a coordinate system (MCID field on the CQUAD4 or PSHELL cards), but FEMAP for some stupid reason won't output the MCID values; FEMAP calculates the material angles and outputs the angles for each element on the CQUAD4 cards. To turn on results output in the material coordinate systems you set the ELEMRSLTCORD parameter to MATERIAL in the NE Editor. Unforturately I have never found a way to figure out in FEMAP what coordinate system the stresses and strains are in once they are read back into FEMAP. (Another problem with black box postprocessors). There is a way to transform stress output from element to a material coordinate system inside FEMAP, although again there is no dianostics provided by FEMAP to tell you what it is doing. The transformed stresses are put into new output vectors.

Without knowing detailed specifics of the coordinate systems, element orientation and desired material angles it is impossible to diagnose your issue. I suggest that you build a very small, simple flat plate model in the y-z plane, apply a simple axial load, define a material coordiante system that is rotated at 45 degrees in the y-z plane, and run the model 3 times getting stresses in the basic, element and material directions. If you do this and still can't understand the results then post a description of your results and we will take it from there.

 

[fkmeyers]

SWComposites has it right. The stresses when read back into FEMAP are in the coodinate system NEiNastran calculates them in. For V8.3 that is the element system. Setting ELEMRSLTCORD to MATERIAL puts them in the material system which can be controlled in FEMAP. I think in V8.4 the new default is all stresses are in the material coordinate system (i.e., when they ship V8.4 the ELEMRSLTCORD will be set to MATERIAL now not ELEMENT), so I have been told. FEMAP does not translate stresses unless you tell it to. Also, all loads and displacements are in the basic system when read into FEMAP. There is a way to put these in a local system if anyone ever need to know how.

 

[ananthaces]

Thanks meyers and sw for you suggestion. I modeled a simple one to see how this coordinate system behaves in nastran. its juss a simple bar with 2d orthotropic properties and then i ran the analysis without changing any material angle. the result looked weird. thats because the material coordinate was aligned with the global coordinate system. Now here i have a question..whats the difference between material and element coordinate system. i thought material coordinate,element coordiante and global coordinate system is the same unless material angle is updated.
Next i changed the material angle and ran the analysis without changing the ELEMRSLTCORD parameter in the ne editor. it was by default basic( i assume basic means global)..i got some results from this analysis. next i turned the elemrsltcord parameter to material and i ran the analysis. i still get the result as i get in the earlier procedure i.e; elemrsltcord=basic.
I don't understand this. Could you please englighten me? thanks once again for your patience and time.

 

[SWComposites]

Ananthaces - exactly what type of element are you using in FEMAP (bar, plate, ?) and NASTRAN (CBAR, CQUAD4, ?)

 

[ananthaces]

In the previous example which i have explained i have used plates with quad4.

 

[SWComposites]

The material, element and global coordinate systems are not necessarily the same. The global system is the basic reference frame for the entire model. The element system for a CQUAD4 is defined by a vector which bisects sides 1 and 3 of the element (see the manual section on CQUAD4). The material system for a CQUAD4 is defined by default as parallel to side 1 of the element; if an angle is given on the CQUAD4 or PSHELL card the angle is measured from side 1 of the element (see the figure in the manual). The 3 systems will only line up in the following case: the elements are in the x-y plane of the global system, and the elements are rectangular, and sides 1 of the elements are parallel to the x-axis of the global system.

Instead of describing the results as "weird" please use quanitative terms. You need to more fully describe your model and results, such as: A plate of dimensions X by Y located in the ?? plane, loaded with ?? loads in the ?? direction with ?? boundary conditons on the ?? edge. The stress in the plate should be ?? by hand analysis. The results for the stress in the ?? direction in the ?? coordinate system are ??, etc., etc. If you cannot describe your model and results in this detail there is no way we can give you specific answers.

 

[ananthaces]

yes sw shall be specific in future. I have another question. suppose there is a 4x4 inch plate. and i define a local coordinate system or i modify the angle of the element such that the element x is aligned with global y direction. now i want to apply load and constraints. are the constraints and load applied with respect to the global or with respect to the local system? Thanks

 

[SWComposites]

Constraints are defined in the NODAL output coordinate system, which you can specify in FEMAP. For loads it depends on the type of loads. Nodal loads are specified in the nodal output system, pressure loads are defined as normal to an element surface, etc.