I would like to know if there is a quick and easy way to assign a unique fixed displacement constraint to multiple individual nodes. I have attached an image for your reference. It could be very tedious and time-consuming to input the displacement constraint for every single node (~ 1000+ nodes).
Greatly appreciate your help!
Thanks and regards,
Solved! Go to Solution.
its very easy to define constraints on a face or surface or plain area of nodes if we talk about NX CAE.
1. If you have a underlying body you can define the constraint by using the appropriate face (polygon face) of the body.
2. If you don't have not body you can select all nodes by a method for smart selection of objects: feature angle nodes.
3. Furthermore you can build a group with all nodes inside by multi select your nodes by positioning your cuboid in a way that all nodes appear in line and then selecting it with "selection rectangle" (Press left mouse button, drag the mouse pointer sharp around the line and release mouse button).
You also can do so in selecting directly without a group. Keep in mind to set selection type filter to "nodes".
Best wishes, Michael
Thank you for your response!
However, I am referring to a scenario where you have to input a different displacement constraint value for every individual nodes. In this case, I could not select or group the nodes together and apply similar values for all. I was hoping that maybe there is a way to identify all the nodes on my surface of interest and create a table in note or excel to input the corresponding constraint values before solving.
Thanks and regards,
thats also possible. You can define an enforced displacement with spatial distribution.
Type of constraint: Enforced displacement constraint
Tpy: Magnitude and direction - Spatial
Magnitude - Select or define a field table or define ein function for components.
Here you can insert values made of coordiantes and displacements from excel or input file.
If your distribution is a function you can use a function to describe it, too.
You also do not nessesarily need to define for all nodes a sampling point because NX can interpolate, extrapolate and map.
There is also a way to use displacement values from other simulation as input...
Nevertheless I think you have to select the objects (Nodes) where you want to apply your efd.
Thats all for the moment. Best wishes,
I think I get your point and I think that Michael didn't understand you in 100% ( my impression).
Of course you can do this. Application of different displacements for different nodes my be done by editing NASTRAN input file. But you have to remember that once you specify those boundary conditions you have to maintain nodes numeration for all the simulations you will perform, meaning: you can not modify your mesh because you will loose the integrity between BC and Solution. To do that you can simply lock the mesh of the object under consideration in *.fem file
In order to apply such BC, prepare your model with all Loads and BC except the one you want to define for "different nodes".
Then go to Solution, Click "Solve" in *.sim file and then choose an option Write input file, Edit and solve (or something like that. There is a dropdown list. I do not have an access to NX now so do not remember exactly).
Then in input file you can paste your predefined Boundary Conditions for nodes. And here the most challenging fun starts. You need to keep the convention of the Nastran input file which is not easy.
BC you can prepare in Excel by using some macro or in any Text Editor. and just simly paste it in the window that will popup after clicking mentioned above "Solve". It is far easier and faster than clicing nodes one by one.
Another question is whether you really have to do that. My impression is that you want to apply those BC that are result of displacement from another soltion. For that purpose you can use "Enforced displacement" feature and simply imprt a displacement filed that will an output from different analysis.
I hope that's helpful