Editing Nastran Input File

[Nicholas.Peacock]

Hello,

I was wondering if it is possible to edit the Nastran input file in order to assign a spring connection to every node belonging to a specific idealization? I know things like this are possible in other FEA software. If it is, how would someone go about doing this?

Thanks.

[John_Holtz · Accepted solution]

Hi @Nicholas.Peacock 

Yes, it is possible. The input file is a text file with an extension of .nas. This article describes the general steps for modifying the file directly: How to edit the input file in Nastran In-CAD. (In-CAD is the old name for Inventor Nastran.)

For your specific problem, the steps would be something like this. (I have not tried it, so these may need to be tweaked.) If I remember, you have a shell model where you want to put the base plates on a soft support.

1. Add as many springs as possible to the model so that you create the pattern of text lines that need to be copied in the Nastran file. For example, you should be able to add springs to the corners or endpoints of the edges. 
2. Determine all the nodes where springs are needed. If they are shell, you could use a unique idealization for the base plates. For finding the element numbers associated with the unique idealization number, you can get the node numbers. Alternatively, use Appendix C in the FNO Reader documentation to see what type of dummy load can be applied to the element type to "identify" the nodes. (Keep in mind that with parabolic elements there are nodes at the corner and midpoint! Some loads on some element types only apply a load to the midside node!)
3. Based on the springs that were applied to the model, copy one text line and change the associated node (GRID) number to apply the spring to all the other nodes. (The spring is probably some type of CBUSH command.)
4. Hopefully the same spring stiffness can be used for all nodes. If not, then you need different property commands (probably PBUSH) that give the different stiffness. Even if the mesh is uniform, should the spring at a midside node have the same stiffness as the spring at a corner node?
5. I imagine you are using grounded springs. What else needs to be added manually to setup the grounded spring?
   1. Do you need to add a node for the grounded end of the spring? If so, copy the GRID commands for the model end of the spring, create new node numbers, and change the appropriate coordinate to offset the node. (Maybe a grounded spring has a length of 0, so the coordinate does not need to be changed but the node number does?)
   2. Do you need to add a constraint to the grounded end of the spring? If so,  copy the SPC1 command for one of the grounded springs and update the node number.

Of course, try a small test model first. You may need to run the analysis a few times to work out the detailed procedure. The work itself is not too hard, but it may be tedious to extract and transform all of the data in a real model.  FNO Reader can help with extracting the Nastran text lines so that you can manipulate them in Excel, and then transform them back to Nastran format so that you can paste them into the Nastran file. (Version 1.58 is the latest version.)

Let us know what you find out.

[Nicholas.Peacock]

Hi @John_Holtz ,

Thanks for the response, going through the process has been a great learning experience. I know how to add spring elements now. I am wondering about extracting element IDs. My base does has a unique shell idealization, meaning I can easily identify which elements in the .nas file belong to it using the PID of the shell. However, I want to make sure I'm extracting the grid point numbers appropriately.

So, each node element specifies which nodes are associated with it using G1 -> G8, correct? If I took G1 to G8 (or G6 for CQUAD6 elements) for every element of a specific PID number and extracted the set of unique numbers, I would obtain every grid point ID that makes up that idealization. I could then take them and assign CBUSH elements appropriately.  Is this what you would recommend doing?

[John_Holtz]

Yes, what you said is correct.

• The shell element numbers are in column 2 on the first row.
• The shell "idealization" number is in column 3 on the first row.
• The corner node number on the element are in columns 4 through 7 (for quad elements) on the first row. The midside nodes are in columns 8 and 9 on the first row and columns 2 and 3 on the second row.

Extract all the node numbers, sort them, and remove the duplicates. This leaves the node numbers that are on the base plates.

You might want to keep the corner node number list separate from the midside node number list, just in case the spring elements need to have a different stiffness at the midside node. I know that for force loads, the midside node takes a higher percentage of the load than the corner nodes. (Twice the load at the midside node? One way to find out is to apply a fix constraint and see what the SPC reaction force is at the corner node versus the midside node.)

John.