Output FORCE resultant through a surface

[tovallmoli]

Hi!

I think the topic has been already presented but never with a clear answer, and is quite useful for other variables instead of my case FORCE.

I'm having a cylinder with described displacements on the endings and I am looking for an output of the resultant force through it. I cant use any postprocessor for the summation, so I have to code it. My approaches have been the following

- ELFORCE of the section elements with results in X, Y and XY in local coordinates and depending on the element length. (I found it too much of a hassle the summation for such an easy request)
- GPFORCE of the section nodes with results X,Y,Z and Moments in global coordinates. (but this time each node has the contribution of the 4 elements linked and I'm not getting the desired results)

There is not in Nastran any option like it would be in Abaqus of creating a NSET, use *TRANSFORM to have it in desired coordinate and output the forces?
Also Abaqus prints MAX/MIN/TOTAL and that TOTAL would be the one I am looking for.

I had a look on Nastran Surface Definition, but my elements are rotating and is not so straightforward.

Thanks in advance!!!

 

[dmapguru]

I have some questions. I may have more depending on your answers.

Which version of Nastran are you using?
Are we talking linear or nonlinear analysis?
You wrote "but my elements are rotating" - what did you mean by this. Is this large displacement analysis?
In trying to understand what you need, I looked at the *TRANSFORM keyword; I don't see MIN/MIAX/TOTAL options - could you elaborate on this?
By "Nastran Surface", do you mean the SURFACE command in the OUTPUT(POST) section for GPSTRESS etc. use?

DG

 

[tovallmoli]

Hey dmapguru!

Thanks for you reply, let my clarify your questions,

- Nastran 12
- Linear (very small displacements too)
- By elements rotating i ment that since is a cercle, they local coordinate system is always changing and therefore, makes more difficult the postprocesing (if the output is local)
- Well, *TRANSFORM would associate a chosen coordinate system to all the nodes in the SET. Then the output requested (for instance NFORC would output forces in the nodes of the elements) would be without the issue of the "rotating" coordinate system. The MIN/MAX/TOTAL would be related to the NFORC output print in the .dat file
- Exactly! But I couldn't work it out..
SURFACE id, SET esid, [SYSTEM system], [AXIS x-axis], [NORMAL normal]
and also I think I'd have to do a SURFACE for each of the element raw (that share the coordinate system)... I cant do a cylindrical surface and anyway looks too much of a hassle, there might be a easier way

Thanks a lot for your time, I hope you have any suggestion. Cheers and good weekend!

 

[dmapguru]

Forget the SURFACE command. This is specifically for elemental stress (or stress discontinuity) recovered at the GRID points, not for element or GRID point forces. What SURFACE does is provides an averaging surface over which the field of GRID point stresses may be interpolated, accounting for some geometric discontinuities, like edges. It allows, for example, the computation of a unique stress value at a GRID point for each direction, instead of having as many values as there are elements connected to the GRID point.

Nastran 12 sounds like NX Nastran, so I don't know how much more help I can be (that's why I asked this question). In MSC Nastran, there are monitor points, and specifically the MONPNT3 to allow free body diagram loads to be computed. Basically, you define a section at which you want to sum the forces at the GRID points around some location in space. The sum can be made over any section, about any point and in any coordinate system. This works by using the same concept as GPFORCE, but GPFORCE only gives you the breakdown of forces at each GRID point according to what is connected to that GRID point (elements, applied loads, SPC, MPC, DMIG, contact,...). MONPNT3 takes the GPFORCEs and sums them to provide you a TOTAL as you put it, in each of the 6 directions of the nominated coordinate system. Perhaps NX has a similar thing.

For MSC and NX Nastran, you can place any GRID point into a local coordinate system by using either the CP field on the GRID entry or the CD field. CP is the coordinate system in which the GRID point coordinates are defined, CD is the coordinate system in which the displacement solution is expressed. These 2 systems may be different. GPFORCE output is in the global coordinate system, so if you define local coordinate systems in the GRID point CD field, your output will be in these local coordinate systems. If you want the GPFORCEs to be aligned with the edges of 1D/2D elements, take a look at the parameters PARAM,NOELOF and PARAM,NOELOP.

Finally, there are tools available in post processors to do the sum over a section. In MSC Patran, they are called free body loads, and they do exactly the same thing as the MONPNT3, except as you point out, in one case it is the solver doing the work and in the other the post processor.

DG

 

[tovallmoli]

Hello!

MONPNT3 is also working on NX Nastran and it's exactly what I was looking for! Thanks a lot!

The only think is that I followd the sample of the User Guide in page 4-11

https://docs.plm.automation.siemens...ces/nxnastran/12/help/tdoc/en_US/pdf/User.pdf

- I added the 'MONITOR = ALL' in the end of the SUBCASE

- I added the MONPNT3 in the end of the Bulk Data:
$1.....12......23......34......45......56......67......78......89......9+
MONPNT3 A1
123456 1 0 0.0 0.0 0.0
0
$1.....12......23......34......45......56......67......78......89......9+

And ended up with the following errors (Is strange that the User Guide Samples are not working)

13 MONITOR = ALL
*** USER FATAL MESSAGE 601 (IFP1D)
THE KEYWORD ON THE ABOVE CARD TYPE IS ILLEGAL OR MISSPELLED.

*** USER FATAL MESSAGE 307 (IFPDRV)
ILLEGAL NAME FOR BULK DATA ENTRY MONPNT3

Mention that as a ELEMGRP of the MONPNT3 i assigned 1 which is a SET defined in the Control Data. I don't think is the issue here.

Thanks a lot!