Showing results for 
Search instead for 
Do you mean 

Using Contact Pressure to define an Input Load.

Hello FEMAP Experts,


I currently have 3-D FEA model of two concentric rings, there is an interferance fit between the two rings. The interferance is a result of a offset surface contact between the inner ring and outer ring. The model runs very quickly and the pressure and stress results match up perfectly with hand calculations. I'm looking to use the contact pressure generated between the two rings as an input for a seperate and different model. I have tired using the load from a model command button, but it seems to lock up FEMAP. Has anyone ever used contact pressure from one model to generate an input or data surface for a seperate model? Also this is a simplifed model to test this analysis technique for a more complex model. So directly applying dirrectly to the next model. I've had really good luck with submodeling in FEMAP, ion the past so I'm pretty sure this isn't outside the capabilites.


Thank you for your expertise and time.






Re: Using Contact Pressure to define an Input Load.



I have created earlier a FEMAP API to export contact forces on nodes of cylindrical surface to Excel. I attache this, maybe you can use it. This API work with Office 2010, when you use other, the reference in the API Programming Pane must be changed. In my case I use "Microsoft Excel 14.0 Object Library".


I make this API to export contact forces on nodes of cylindrical surface normal to XY plane, centre X0, Y0. When you will use other surface orientation to the formulas in API must be changed.


Best regard


Peter Kaderasz

Re: Using Contact Pressure to define an Input Load.

Dear JP,

The problem with contact pressure is that it is a nodal result value, not element value, then not possible to import at pressure loads applied to elements using command "MODEL > LOAD > FROM OUTPUT". But you always can create a FREEBODY of type INTERFACE LOAD, select the nodes of the surface, and the output of the freebody is just the force loads acting at each node.


Next issue command "MODEL > LOAD > FROM FREEBODY" and select the previously created freebody and you can create a new load case just loaded with the output of the freebody, OK?.



Best regards,


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

Re: Using Contact Pressure to define an Input Load.

Blas and kadpeter,


Thank you for your help, and suggestions. Blas once you jogged my memory about the interface pressure not being a true elemental pressure I knew how to solve my problem. Thank you!!! Using the list model results output to data table, I was able to collect the interface pressure on each node, along with the physical location of each node. I then generated a data surface, pasting this pressure data and location data into the data surface using the Arbitrary 3-D data surface tool. I was then able to copy this data surface to my new sub-model and apply this load on the surface of my solid using the data surface to map the pressure distribution. I'm going to upload both sample models incase anyone else needs a hand with this in the future.


One following on question, is there anyway to smooth out the pressure contour between dissimilar meshes.

Re: Using Contact Pressure to define an Input Load.

FEMAP Users,


I just wanted to provide a quick follow up, toeveryone regarding the Load ---> Map Output from Model command. It is currently not working in FEMAP 11.1.7. I have a Incident Report  in with Siemens. I'm hoping this bug can be fixed soon. FYI if you do need to use this command it does work properly in FEMAP version 10.3. I hope this information is helpful.





Re: Using Contact Pressure to define an Input Load.

Dear FEMAP users,


I just formally heard back from the Siemens / FEMAP team, and FEMAP 11.17 or 10.3 is NOT designed to work with submodeling on solid elements. The Load ---> Map Output command is not suppose to be used for sub-modeling.