Element Group Selections for bolts are disappearing

[luke_maloneVWR3M]

Hello,

I am using the Plot XY technique (https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/Can-the-Bolt-conne...) to find the reaction forces in bolt connectors in my linear static analysis. After I create a Group from the Beam elements of the fasteners I need to analyze, then close Nastran after saving and re-open it, the Group usually is gone and I have to re-select all of the elements to re-make the Group. How can I make sure the elements and the Group do not disappear after I close Nastran?

Thank you!

[John_Holtz]

Hi @luke_maloneVWR3M . Welcome to the Inventor Nastran forum.

What version of Inventor Nastran are you using? (In the Nastran environment, click the "i" symbol for "Nastran Support > About".)

You wrote that the group usually is gone, implying that sometimes it remains. Do you know what is done differently between the times that the group remains and the times that it disappears?

I suspect that the Groups are intended to work only with elements created by the mesher. Elements like the bolt connectors, rods, and rigid connectors are created in the Nastran file, so they may be treated differently. For example, if I edit an Element Group that has the bolt elements, I get this message:

I do not see a work around, other than using FNO Reader to output the results at all CBEAM elements (assuming the only beams in the model are the bolt connectors).

John

[luke_maloneVWR3M]

Hi John!

I am using Inventor Nastran 2023.

I have noticed that the Group definitely is gone if I re-mesh the model, which makes sense. In that case, if the mesh changes, those elements I originally selected to be in the Group then have a different ID, and therefore the original element IDs no longer exist.

That is the same message I receive. Perhaps I need to make sure my results file (.FNO) or the .NAS nastran file is always loaded prior to pulling the resulting reaction forces.

With the .FNO reader guidance, do you know if I could "simply" look at the Beam Forces in 3 directions for each of the beam connectors?

Thank you,

Luke Malone

[John_Holtz]

Hi Luke,

Try your suggestion of loading the result file before trying to plot the XY result at the group, but I think it will not make a difference. Perhaps regenerating the Nastran file will make a difference.

With FNO Reader, you can output the three force directions (axial, shear Y, shear Z) at the same time for all the bolt connectors, without needing to know the element numbers.

1. Use the workflow "FNO to Table".
2. On page 2, choose "Results > Element Centroid" and move the results you do not want to output to the "Number Available" box. Leave the results you do want to output visible in the "Number to Output" box.
3. On page 2, choose "Elements".  Alt+Click the "File" button in the first row of the spreadsheet. For the "File contents" column, choose "CBEAM beam elements, PID =". Leave the "File details" column blank if all the beam elements in the model are bolts where you want to output the results. Otherwise, click the search button in the "File details" column and select which ID numbers are associated with the bolts you want to output.
4. The rest of the input is to tailor the output to make it more suitable for your purpose.
5. Be sure to click the "Save" button in the top right so that you can do the same output if you change and re-run the analysis.

John

[luke_maloneVWR3M]

Hi John,

Thanks for the reply! Should I create my Fastener beam element Groups, then re-make the Nastran file, then go into the FNO Reader? What would be the correct order of operations before beginning step #1 you provided?

I did take a look at the .FNO Reader and made it to Step 2. I put the only .FNO file I've made with this analysis, did not regenerate the .nastran file, and made 1 fastener beam element group to test. At step 2, I don't see the option in the "Number to Output" box for the Beam Element End A-X, or the -Y and -Z results either. 

Thank you,

Luke

[John_Holtz]

Hi Luke,

FNO Reader does not use element groups, so no need to create that. (The element groups are not in the Nastran file either, so no need to re-make the Nastran file.) After running the analysis, you do not need to do anything else before going into FNO Reader.

At step 2 when you select the Results branch from the Tree View, you need to click "Element Centroid" and click the "Refresh" button. Beam stress output is based on the element, so the "Number to Output" box will only show the beam stress results when the filter is set to element centroid. The example on page 6 of the FNO Reader documentation, beginning at the header Result From Limited Locations, is similar to the steps that you will be using. (The discussion about GPSTRESS does not apply to your case. GPSTRESS changes what is output for solid elements. The beam elements do not change with GPSTRESS.)

John

[luke_maloneVWR3M]

Hi John,

This was very helpful! I was able to get a .csv file with a list of every Element ID for every Bolt Connector, and the resulting reaction forces for every load case, which is what I need. However, I just get a list of all of the Element IDs, and without making a Group in Inventor, I'm not sure which Element IDs belong to which Bolt Connector Group. Is there a way I can organize the results by Connector Group, like my example below? That way, I know which Element IDs are in Group A, B, etc.

Thank you!

Luke

[John_Holtz]

You need to create a separate table for each set of bolts that you want to be separate in the output.

1. Create the first table for set A.
2. When defining the element locations, click the search button in the File details column. See Figure 49. (In your case, you will just have 1 row in the spreadsheet, not many rows like in this example from the documentation.)
3. Check the box for set A. Note what other IDs are associated with the other sets B, E, ... See Figure 50.
4. Click "Use checked rows" to insert the ID for bolt group A into the spreadsheet.
5. After the input for table A is fully defined (subcases, results, locations), hold the control key and click the Insert new table after button . This adds a copy of Table A to the Tree View. Change the title to Table B.
6. Change the "File details" value to the ID for bolt set B.
7. Repeat steps 5 and 6 for each new table/bolt set.

John

[luke_maloneVWR3M]

Hi John,

For some reason, the search button is not available in the "File Details" column, any ideas?

Thank you!

Luke

[luke_maloneVWR3M]

Hi John,

I found the issue - I was using version 1.76 of the FNO reader, and was able to see the Search button with version 1.84, which I got from here https://forums.autodesk.com/t5/inventor-nastran-forum/read-binary-results-file-fno-with-a-program/td....

I believe this fixes everything, I'm now able to pull the reaction forces I need for the Bolt Connector groups I want to view. Thank you for the help, this is a huge time-saver!

Thank you!

Luke