read binary results file (FNO) with a program

[AstroJohnPE]

Hi,

The results of a Nastran analysis are written to a binary file (the .FNO file). Do any users have a program to read the binary results file (.FNO) that they would be willing to share with the group? It could be a simple program that just converts the file to a text format, or a more sophisticated program that converts selected parts of the results file and/or does manipulations on the data.

For example, imagine a transient response analysis with 100 time steps.  It is tedious to review all of the results manually. A program would more quickly allow these types of things to be done:

• find the highest stress at each time step.
• find all of the nodes or elements with stresses above some value for each time step
• sum the reaction force at the constraints at each time step.

Before I start work on such a program, I thought that I would ask first. (Also posting to the Nastran forum. Reply to either forum 🙂)

John

2025 Jan 2. This post has been updated to attach the latest, FNO Reader version 1.84

[darrenlovesmusic]

@John_Holtz 

Thank you for this helpful tool. However, I'm not quite sure if it has the nodal values of principal strains? Is it something that I missed out? 

[sigurd.naess]

Hi @darrenlovesmusic !

Did you specify GPSTRAIN(PUNCH) = ALL before running the analysis

That should give you all the nodal strains

[John_Holtz]

To elaborate on Sigurd's message, the results do not include the stress or strain results at the nodes by default. The results do include the stress and strain results at the corners of each element. (Although they are the same location in space, they are different mathematically.) So you could use the Element Corner output to see the principal stress/strain results.

When viewing the results in Inventor, it takes the results at all of the corners of the elements that are connected to a node, and averages the results. To get the same thing using FNO Reader, you could do one of these:

• Add the command GPStrain(Plot)=All to the Nastran file. See page 87 of the FNO Reader help PDF. You can use "Plot" instead of "Punch" as Sigurd suggested. Plot will put it into the FNO file so that you can extract it. Punch also puts it into the FNO file but also creates the PCH text file which usually is not too useful. (The PCH file is usually overwhelming with page after page of number.)
• If you only have the corner results, you could in theory use FNO Reader to output the strains at the element corners (using FNO to List or FNO to Table), use FNO Reader to output the element commands (using NAS to Text), and then calculate the average that occurs at each node using some type of calculation in Excel. If the analysis does not take long to run, it is easier to rerun the analysis with the GPSTRESS or GPSTRAIN command than it is to do the averaging in Excel. 

[darrenlovesmusic]

@John_Holtz  Its seems to be working for me. 

If I need principal stresses σ1, σ2, σ3 and equivalent plastic strain from a shell mesh, that would be: 

1. [115] SHELL MAX PRINCIPAL STRESS BOTTOM/TOP, σ1

2. [116] SHELL MIN PRINCIPAL STRESS BOTTOM/TOP, σ2

3. [712] SHELL MAX VON MISES STRAIN BOTTOM/TOP, εeq

[AstroJohnPE]

Hi @darrenlovesmusic 

Sorry for the late response.

I'm glad I read my own documentation, because I almost gave the wrong answer! Just to clarify, did you run a nonlinear analysis with GPSTRESS(PLOT)=ALL and GPSTRAIN(PLOT)=ALL manually added to the Nastran file? When I include those two statements in the Nastran file, I get the [115] and [116] results you mention. Without those statements, those results do not exist. (Only the element centroid and element corner results exist if the Grid Point statements are not added to the Nastran file. By the way, GP stands for Grid Point.)

Your question is hard to answer because there is a difference between the results you want (max and min principal stress) and the more accurate stress that follows the stress strain curve. In some cases, the difference can be significant, especially at corners and other "hot spots" in the analysis. If these do not occur, then the distinction may not be important. I suggest reviewing this article to clarify the difference between the the principal and von Mises stress compared to the equivalent stress and effective strain: Equivalent stress in a nonlinear analysis with Autodesk Nastran.

In summary, your options are the "regular" results of

1. [115] SHELL MAX PRINCIPAL STRESS BOTTOM/TOP
2. [116] SHELL MIN PRINCIPAL STRESS BOTTOM/TOP
3. [712] SHELL MAX VON MISES STRAIN BOTTOM/TOP
4. [714] SHELL MAX PRINCIPAL STRAIN (if you want a more consistent stress and strain)
5. [715] SHELL MIN PRINCIPAL STRAIN (if you want a more consistent stress and strain).

Or use these equivalent stress-strain output which then depend on the Yield Criterion chosen on the material dialog:

1. [716] SHELL EQUIVALENT STRESS TOP
2. [717] SHELL EFFECTIVE STRAIN-PLASTIC/NONLINEAR ELASTIC TOP
3. [719] SHELL EQUIVALENT STRESS BOTTOM
4. [720] SHELL EFFECTIVE STRAIN-PLASTIC/NONLINEAR ELASTIC BOTTOM

John.

[AstroJohnPE]

FNO Reader version 1.50 attached.

Hi all. I have added a few minor enhancement to FNO Reader that make a few items easier to use.

• When selecting the input file, the Select > Open dialog now includes the option to choose an Inventor File (.iam or .ipt). Selecting the Inventor file in FNO Reader will show a dialog that lists all of the analyses in the model. If you are also using Inventor Nastran 2021.2 or newer, the new dialog includes the text/name of the analysis. You do not need to know the random filenames now! (You just need to give a meaningful name to each of your analyses.)
• When converting the FNO results file to a text file, the subcase "Title" can now be replaced with the value associated with the title. For example, instead of writing out "[15] TIME=1.123E-4", you can write out "1.123E-4". This makes it much easier to graph the results of transient analyses versus time, or the results of a Normal Modes (modal analyses) versus the frequency, and so on. 
• You can now customize some of the defaults when FNO Reader starts. Do you most often use the workflow "FNO to Table"? You can set that as the default. (Previously, the chosen workflow was always "FNO to List".) Other defaults that can be set are the file extension when you browse for a file and the table layouts (the directions for the subcases, results, and locations) when using the "FNO to Table" workflow.

I hope you enjoy it.

John

[darrenlovesmusic]

@AstroJohnPE 

Thank you! Its working very well! 

[darrenlovesmusic]

@John_Holtz @AstroJohnPE ,

It is possible to get effective plastic strain as a nodal value? Is there a separate deck card for it?  I am getting an absurd value from the parameters [720] and [717]

Inventor Nastran InCad 2018

[John_Holtz]

Hi @darrenlovesmusic 

Those "strain" values almost look like stress values (if you were using psi units).

The Nastran parameters GPSTRESS and GPSTRAIN will output the stress and strain at the nodes by averaging the element corner values. I do not know if the GPSTRAIN output includes the effective strain or not. Search the FNO Reader documentation (the pdf file, accessible from the "?" button) for GPSTRAIN for instructions on adding the parameter to the analysis.

[darrenlovesmusic]

@John_Holtz John, I think its not possible to get nodal data of equivalent plastic strain. PLSTRN is the case command for other software using NASTRAN code. 

[AstroJohnPE]

FNO Reader version 1.58 is attached.

Hi everyone. I made a few minor changes to FNO Reader, one bug fix, and one "medium" size enhancement. Here is a brief summary. (The documentation has the full details of the changes.)

1. Bug fix. Translating a Nastran file to text (workflow NAS to Text). If the last value on the line was a single character (such as a node number less than 10), and if the value was aligned to the left side of the column, the value was not written to the text file. This has been corrected.
2. Enhancement for the workflow FNO to Table. When choosing which locations (which nodes or elements) to extract the results, you can indicate to read the locations from the Nastran file. Instead of limiting the cards that can be read to a hard-coded list (such as CTETRA and FORCE), a new dialog lets the user define the Nastran cards.

John

[hbhu]

Thank you very much.  I think it is a good idea to turn this program into a stable released software in some way, what do you think?

[frankRMLDF]

Hi John,

Thanks for making the FNO Reader it is a very helpful tool. I was using it and it looks like the "Split output file(s) into lines of length. N =" is not working for  NAS to Text. It is also possible that I do something wrong but for FNO to List it works.
Probably you can take a look at it.

Kind regards,
Frank

[John_Holtz]

Hi @frankRMLDF 

I just tried it using the current version (1.58) and did not see a problem. Perhaps there is a bug depending on the options? Can you let me know the following:

1. What cards were checked to output? (page 2. I tested CTETRA and GRIDS)
2. What file extension was set on page 3? What column separator was set? (I tested .txt file and "Automatic" which would use a Tab to separate the output.)
3. What did you use for N lines to split? (page 3. I tested 5000, 20000 and 30000.) How did you type the number? For example, did it include a period (like 1.1E5) or a comma (like 1,1E5 depending on where you are located in the world).
4. How many lines are output? (50542 in my test.) 

Thanks.

John

[frankRMLDF]

Hi John,

I made a video. See attachment.

I also tried some things, and noticed that a dot was the problem. If I use 1.0E6 it does not work. If I use 1,0E6 or 1E6 it works fine. 

This is different from the FNO to list because if I use 1.0E6 or 1E6 it works fine but if I use 1,0E6 it makes a lot of output files.

Kind regards,

Frank

[John_Holtz]

Thanks @frankRMLDF .

I found the problem, and you are correct that it is related to using the period (".") versus the comma (",") as the decimal symbol and how I was converting the number. Somewhat strange, but "1.0E6" (with a period) is being interpreted as 10E6 when the period is not the decimal symbol. Since your output did not have more than 10 million output lines, the program did exactly what I told it to do. 🙂 Unfortunately, I did not tell the program to do it correctly! 😞)

"1E6" and "1,0E6" were properly interpreted as 1 million output lines. 

I will correct this in the next release. The next release will not be for a few months because I am in the process of making other changes and want to test and release everything together.

John

[AstroJohnPE]

Hi everyone,

I have released a new version of FNO Reader. Version 1.72 is attached to this post. (I will also attach the current version to the original post so that it is easier to find in the future. This thread is getting long and hard to find the latest version!)

The changes in this version include the following:

1. The number input to split output files into N lines now supports the period and comma for the decimal symbol according to the computer's region settings. (bug reported by one of the users)
2. Compare FNO now matches subcase values in the two files when they differ so that the comparison continues. 
3. Compare FNO now matches result types in the two files when they differ so that the comparison continues. 
4. FNO to Table. The following changes were made to the File contents Editor:
   1. Corrected a problem that prevented an image of the Nastran card format from being displayed.
   2. Added a Merge command so that different lists of Nastran cards created by you and your friends can be merged. 
   3. Corrected issue in Edit File contents that limited the number of cards to 20.
5. FNO to Table. Improved efficiency of reading Nastran file (.nas) when extracting node or element numbers for the locations.
6. FNO to Table. Corrected issue when results were given as “NaN” even though the location was correct, and the result did exist at the locations. (bug reported by one of the users)
7. Text to Nas can now force the numbers to be an integer or real (as required in the Nastran file).
8. Other minor changes to the interface as detailed in the help documentation, "Updates" section.

John

[gbrisbinUZ9NP]

Hello,

I've been attempting to use your program, and outlined process, to get contact force values for sizing welds. I am able to successfully follow your example, and execute the same process on smaller assembly models, but on a particular large assembly I am receiving either "NaN" or "0" values for my contact forces. Any thoughts on what could be causing this? Any help would be appreciated.

Thank you,

Garrett

[John_Holtz]

Hi @gbrisbinUZ9NP 

I do not know what is happening, but here are some questions.

1. Are you using FNO Reader version 1.72? (That is the latest version and includes a fix for some type of shell element that caused "NaN" to printout instead of the actual value.)
2. What version of Inventor Nastran are you using?
3. What element types are used at the contact? Solid? Shell?
4. I assume that you are specifying the nodes at which to print out the contact force results by selecting the Nastran file and using "BSSEG Contact face, ID =" and entering the ID number in the "File Details" column. Have you confirmed the ID number is correct for the current version of the Nastran file?
5. From the contact force contour plot in Inventor, you can see which nodes have a force. (It may be helpful to hide one of the parts and use the right-click "Nodes > Query Display".) Do the node numbers that have a contact force appear in the FNO Reader output? Be sure to check both parts to confirm that both have equal and opposite force.

Both "NaN" and 0 could be valid numbers, but there should be nodes that have nonzero contact force.

• "NaN" indicates the node number was obtained from the Nastran file, but the results file does not include that node number. This can occur when one of the contact faces is much larger than the other face, and as a result, many nodes on the larger face do not have any contact elements. That is okay.
• A zero value indicates there is a contact element but the force is zero. This may be okay as long as only some of the nodes have values of 0.

John

[gbrisbinUZ9NP]

Hi @John_Holtz,

Thank you for your response. I apologize for my delay in replying.

1. I am using FNO Reader 1.72

2. I am using Inventor 2024.2 (I'm not certain how to check the Nastran version, but all updates have been performed)

3. I am using all solid elements in my analysis

                 - I am not using continuous meshing. I'm guessing that could be the source of my problem?

4. I rather certain I am using the proper ID from the appropriate Nastran file.

5. When reviewing the contact force contour plot I've found I have zero value contact forces shown throughout my model. My stress results appear accurate, and there are clearly stresses being transferred between bonded contacts. What could be causing my model to not display contact forces?

                 -My model's output sets have both "Force" and "Stress" checked.

Thank you,

Garrett