Showing results for 
Search instead for 
Did you mean: 



Hello experts,


here a basic problem:


What ist the correct definition of NX grid point forces in output request or post prozessor UI?

I can't find the correct help entry in NX documentation.


1. If I get the unaveraged grid point forces I can see at different eleements positive and negative GPFs at the same grid point. Does the summation yields the external load  put on the grid point or the reaction force standing in equilibrium with external force?


2. Is the unaveraged grid point force at a unique grid point in one element the part of loading of that element node (grid point) depending on external loadings or the loading of all other elements due to the stiffness and deformation effects of that unique element grid point?


What is the direction of grid point force at grid point: into unique element or out of unique element into the other elements? - Is it a reaction force or a loading force?


Here my test model:








It looks like beeing reaction forces as my elements are loaded with tension-pressure of 1000MPa at an area of 10x10 mm². Or do I misinterpret it.


Any suggestion will help.


Best wishes, Michael

I'm working with NX 8.5.2.

Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX11
Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".


Siemens Phenom Siemens Phenom
Siemens Phenom



First let me provide some background. Grid point forces represent the forces and moments acting on the grid point (node) from each source. The sources to grid point forces include:


Applied loads

Reaction (SPC) forces

Element elastic forces

MPC and rigid element forces

Thermal loads

GENEL forces (not discussed further)

DMIG referenced by K2GG case control (not discussed further)


Listings of grid point forces will show the contribution of each entity at a given node such as listed here. For a better view of the data, see the attachment:


       3775                  APP-LOAD       0.0           -3.018542E-13  -3.078016E+03   0.0            0.0            0.0

       3775                  F-OF-MPC       7.029212E+05   4.132010E+04  -6.695782E+05   0.0            0.0            0.0

       3775           400    HEXA          -3.659631E+05  -2.509668E+05   3.367471E+05   0.0            0.0            0.0

       3775           450    HEXA          -3.369581E+05   2.096467E+05   3.359091E+05   0.0            0.0            0.0

       3775                  *TOTALS*       5.238689E-10  -6.111804E-10  -2.677552E-09   0.0            0.0            0.0

       6681                  F-OF-SPC       6.203707E+05  -3.975727E+04   6.820799E+05   0.0            0.0            0.0

       6681          3641    HEXA          -2.943106E+05  -2.285283E+05  -3.406983E+05   0.0            0.0            0.0

       6681          3681    HEXA          -3.260601E+05   2.682855E+05  -3.413816E+05   0.0            0.0            0.0

       6681                  *TOTALS*      -5.820766E-11   0.0           -5.820766E-11   0.0            0.0            0.0

Here node 3775 is connected to elements 400, 450, and an RBE2 that is seen as the F-Of-MPC contribution. There’s also a pressure load on element faces that use this element, so the pressure shows up in the APP-LOAD contribution. Not evident above is that this model included a temperature load (constant temperature across all nodes). The temperature load produces internal element forces, therefore its influence shows up in the listing of the element force contributions.


Now compare the above with what is available in Simcenter. Post processing will decompose the grid point force results into


Grid Point Force (element-nodal)

Grid Point Reaction Force (nodal)

Grid Point Reaction Force MPC (nodal)

Total Residual Force (nodal)


UNAVERAGED Grid Point Force in post are equivalent to the element contributions listed in the F06. Grid Point Reaction Force are equivalent to the SPC force listings in the F06, and Grid Point Reaction Force MPC represents the MPC listings in the F06. Total Residual Force are equivalent to the TOTALS line in the F06. I’m running SC 11 and I don’t see a result type for the applied load contributions. That could be a bug.


For equilibrium to be met, the Total Residual Force should be zero at each node. The sum of all contributions needs to be zero.


To your first question, post processing supports averaging, or in the case of grid point forces, nodal combination of element-nodal data. It makes sense to SUM grid point forces, but not much to AVERAGE them. A summed grid point force display will show the nodal result of summing all element contributions at a given node. It effectively will be equal and opposite to all of the other contributions at the node. That is evident from the fact that equilibrium requires that all contributions to grid point forces at a node must sum to zero.


You are correct with your approach in the second question. The unaveraged grid point force from a single element at a single node is the force that the element exerts on the node. That element’s force on the node will be influenced by the applied loads, other element loads, and other force contributions at that node. The key is that all forces contributing to a node’s force must sum to zero for static equilibrium. The force contributions are reacting against one another.






Mark Lamping

Simulation Product Management

Simulation and Test Solutions


Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.





thank you for answering.


Do I understand it correctly if I assume, that the "grid point force - element nodal, unaveraged" provide a kind of inner resilience force due to outer deformation of element?

And if differences between elements values (absolute value) occur at the same grid point, it means that there are additional grid point loadings like forces or something like that.


That means if I try to get an information about the "area substitution forces and moments" (I do not know the correct phrase in English, sorry) of a plain grid point layer between two mesh areas which are connected correctly by those grid points solely, I have to sum all "grid point forces - element nodal, unaveraged" of ONE SIDE of those mesh areas. Both areas will yield sets of forces and moments with opposite orientation.


Here my final question:

1. The cutting force and moments of one area is then the negative values of the summation of ITS OWN "grid point forces - element nodal", correct?


2. If I lead in e.g. a lateral pressure at that grid point layer element faces the difference between area summations of both sides will yield the summation of that pressure, correct?


3. Does gravity yield "grid point forces - applied load" as a unique combination of contribution of ALL connected elements or can I find the elemental contribution separately?


Best wishes, Michael

Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX11
Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".


Siemens Phenom Siemens Phenom
Siemens Phenom



You are doing a good job of interpreting grid point forces. They are used to validate equilibrium and loading conditions. They are used to generate free body diagrams – loads at a junction relative to one side or the other of the junction. Since the model has to be in equilibrium, the loads on the two sides of a free body diagram junction will be equal and opposite one another.


This article in the online help explains the use of grid point force data in post processing.



Post processing supports creation of free body diagram results. Select the Post View from the Post Processing Navigator, then MB3 Free Body Results. The dialog will ask for selected elements, and interface nodes. The selected elements will typically be all elements that define one side or the other of a free body junction (or cut plane). The interface nodes will be all nodes on the cut plane. The final selection step is to specify where the resulting forces should be summed for the moment calculation. Forces and moments are displayed graphically and summarized via text.





Good Day Mark,


just hipotetically,


If I would export grid point force as a field from one solution, would it be possible to import those forces as a load into another solution? As I understood the result should be the same right ?


Intention of the question is as follows:

- perform SOL105

- export grid point force from one of the buckling modes as field (which field will be the best?)

- apply those forces (as a field - how ?) in SOL106 and multiply them apporpriately in order to obtain proper initial deformations

- in second step of the SOL106 add additional load in order to check buckling stability


is that doable ?

Thanks Smiley Happy


Siemens Phenom Siemens Phenom
Siemens Phenom

Grid point force output is used to generate loads from one model for use in another model. The use cases I've seen have been related to linear statics solutions of coarse meshed "global" models representing an assembly and fine meshed "local" models representing a component or portion of the assembly. In post processing, you can choose Sum as the nodal combination option in a grid point force contour plot. You can also choose to NOT INCLUDE in the sum elements that aren't in the display. So, If you have a cantilever beam, and display half of it in a grid point force contour plot, you would end up with non-zero loads where the beam is cut. Those loads can be used in another model to represent the load condition of the beam at the cut. The trick is accurately distributing the loads to the local model. Typically you use nodes from the global model in the local model too. Load those nodes with the grid point force output. Then connect those nodes to the fine mesh model directly (i.e. merge coincident nodes) or via rigid or constraint elements from the loaded nodes to fine mesh nodes near the global nodes. This is a common practice in the airframe industry. There will be a global model of an aircraft that is used to generate loads for local models of components and sub-assemblies. The same load cases are run on the local model as the global model.








may I ask one question to your last posting:

Is it the same

- using the "grid point forces - element nodal" at a cut face in addition with "grid point forces - applied loads" or

- using the displacements representing the deformation state of the complete model?


In order to create a sub model with mesh refinements I normally use the displacements of the global model in the vicinity of cutting faces for creating sub model enforced displacements by using a spacial distributed displacement table in combination with the remaining loads of newly meshed sub model geometry (like pressures or gravity or temperature strains).


Is there a reason for using the forces instead of displacements? - Or is using the grid point forces the better way? - And when doing so, do I need to have identical boundary meshes for global and sub model?


Best wishes, Michael

Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX11
Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".


Hi Michael,


I have a reason why I need to use Grid Point Forces instead of prescribed displacements, that's I try to do so (and still have to work over this a little).


When you 'extract' displacements from one global model, and apply them on the local fine mesh, you will get results on the local mesh, but the nodes which will have applied 'enforced displacements' will remain stiff and their further displacement is not possible, menaing their position will not change even if you will add additional external load on the local model.


In my case I wan to use Grid Point Forces (properly scaled) from one global (buckling) analysis in order to obtain in subcase 1 (SOL106) initial displacements. The shape of displacements shall be the same as for certain buckling mode - but scaled according to specific code requirement.


In next subcases I want to add additional external loads to the model in order to check propagation of the deformation of the global model. If I would use 'enforced displacements' in the frist subcase, in next subcases the model will not deform at all.


Any hints how do this properly ?




Hello Tomek,


I understand the problem of fixing deformations for additional solution analyses.

But I'm not sure, if only transporting the grid point forces will yield the same buckling eigenform.


What kind of solutions do you want to use for postbuckling analysis? - In solution 601 or 106 I had always lots of problems in running through a bifurcation point and quality of results depends on selected strategy parameters in Sol 601.


I found in NX Help the following chapter after searching for "bifurcation nonlinear":


Home > CAE > NX Nastran 8.5 > Basic Nonlinear Analysis User's Guide > Nonlinear Analysis Types > Nonlinear Buckling Analysis


... a method in solving post buckling simulations...




Restrictions and Limitations in SOL 106


* In postbuckling analysis with arc-length methods (NLPCI Bulk Data entry), the iteration algorithm may 
jump between different buckling modes when multiple bifurcation points are present in the structure.
It is recommended to check all possible buckling modes with the linear buckling solution sequence SOL 105
before making a run with SOL 106. You have to introduce initial imperfections
(loads or enforced displacements) to keep the structure in the intended buckling mode.


Is that the way you do?


Best wishes, Michael

Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX11
Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".


For all those who tracket the thread.

Finally after Christmas I had time to investigate this case little bit more.


The case wast to 'export' the shape of the structure, for the chosen mode, from SOL105 (linear buckling) results to the SOL106.

The easiest way that I found to achieve that (for further post-buckling analysis) was:

- go to desired mode SOL105 Results

- go to grid point force - element-nodal --> Identify Results --> select all (box) --> Create field (independednt- NODE ID, Dependent: parameter space)

- Create new SOL106 --> New Subcase --> Add load: NODE ID TABLE --> in Scaling ID TABLE choose previously defined field, in magnitude you can scale your loading in order to get 'initial deflection' on desired level.



Then is the case of setting proper parameters for Non-Linear Buckling analysis. And here the question arises, how to understadn arc-lenght method parameters in NX Nastran ?


I hope it helped Smiley Happy


Happy New Year !