Showing results for 
Search instead for 
Did you mean: 

center of gravity displacements - FEMAP


Hi all!


I start in forum posting a brief (and maybe basic) question that drives my crazy since last week.


I´m trying to obtain the displacement of the center of gravity (COG) of a model.


This means, an undeformed model has a certain COG, whose coordinated couId be obtained via the .f06 file (for sure there should be a simplier way directly in FEMAP).


The goal is to obtain the COG of the deformed model after running it with NX Nastran.


Thank you very much in advance for your help.


Re: center of gravity displacements - FEMAP

Siemens Phenom Siemens Phenom
Siemens Phenom

If you create a node attached to the mesh at the COG, you can simply extract the displacements of that node.


If you need to locate the COG of the mesh, use the command, Tools > Mesh Properties > Mass Properties.

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: center of gravity displacements - FEMAP


Hi Chip Fricke,


thanks a lot for the quick response.


I´ve thought about that, but the issue comes on how to attach the COG node to the mesh without modifying the stiffness of the structure but capturing properly the COG displacement. (a massive weighted RBE3 doesn´t seems as a good solution to me)


Thanks a lot for your help

(and tip! Mass prop. command seems really useful) 

Re: center of gravity displacements - FEMAP



Another option is to put FEMAP to work: deform your model in FEMAP using the macro Custom Tools > PostProcessing > Nodes move by Deform, then make FEMAP recompute the CoG through Tools > Mass Properties > Mesh Properties.

But a RBE3 that takes your entire model should be fine as well.

Compare both methods and see what comes out!






Re: center of gravity displacements - FEMAP

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom


In my opinion the simplest method is the following:

  • Take note of the coordinates of the CoG of the FEMAP model using command TOOLS > MASS PROPERTIES > MESH PROPERTIES.
  • Put a POINT there using command GEOMETRY > POINT and enter the previous computed X,Y,Z coordinates of CoG.
  • Use LIST > MODEL > NODE and search for the nearest node to the previous created point: in the ENTITY SELECTION dialog click in PICK^ and select AROUND POINT, click the point and next in the SELECT BY DISTANCE FROM POINT dialog choose AT LOCATION and the nearest node will be selected.
  • Simply edit the node with MODIFY > EDIT > NODE command and pick the POINT to update the coordinates of the node with the point, and you are done!.
  • Rerun the analysis and inspect the resultant displacements of the node located in the CoG.

Best regards,


Blas Molero Hidalgo, Ingeniero Industrial, Director
Blog Femap-NX Nastran:

Re: center of gravity displacements - FEMAP


Hi Blas,


thanks a lot for your quick and precise response.


However, I don´t fully agree (or understand) the suggested methodology. As far as I can read. This mill modify the original mesh, translating a single node (the closest) to the COG.


As the model is modified, once runned, it will result in a different deformed than expected. Of course, these variations depends of the geometry.


As always, thanks you very much for your time and efford. (80% of my FEMAP knowledge comes from your blog and youtube channel).


Re: center of gravity displacements - FEMAP

Good morning astrium_tls ,

this seems not as a good solution but as THE solution. This "Nodes move by Deform" function is really powerful.

Regarding the RBE3, I assume using this emelent could be thrustful if you have a "compact" model. With compact I reffer to a model where the COG is more or less in the geometrical center. This may be the start of a big discussion. But, there to be say, using a massive (weighted ) RBE3 delivered less displ.(more stiff) of the COG than using the custom API.

Thank you very much for your time.