After attempting to run a simulation, I have ended up with a large number of 4297 (EQD4D) errors. I understand that I need to find the listed elements and correct the mesh in that area to make them more rectangular.
Can anyone suggest a good workflow for finding these bad mesh locations? Currently I am openning the error log and manually typing in the element number into the Windws -> Show Elements dialog, and then re-running to see if they disapear.
Is there a better (i.e. less manual) way to find where these errors are?
Solved! Go to Solution.
Try using the command Tools > Check > Element Quality. Select all the elements and click OK. Click the Nastran Tab. Turn off all checks except for “ Quad IAMax > Value”. You can change the value to what you like. If check “Details To Data Table” under Options is selected, the Data Table will propagate with the elements IDs and values that fail this test. You can then use the "Show When Selected" button in the Data Table to pin point where these elements are.
This may be one of several work flows that can help.
Also note the "Make Group" checkbox...there was an old "NASTRAN 4 Windows" tutorial that used that feature to create the group and then bring across the nodes too.
It then used the "shrink element" view function to find the "linear" plate elements (i.e. look like lines)
Having them in a single group allows you to work on a small portion of the model, especially if they're all connected.
Hi thanks for the information, it was useful, but not quite what I was looking for.
My questions is, after I have run the Nastran solver and recieved a list of elements that are failing or have warnings, is there a way to see where these elements are on the model?
My model is passing the element quality checks, but I am getting errors and warnings after running the elements that I would like to understand.
Currently, I am manually typing in the elements and nodes from the log file into the Window-Show Entities selection box, which is a lot of work!
If you can get a text list of those elements (I think it'll be in the *.f06 file), the "Entity Selection" dialog has a "Paste" feature.
Look under the Pick button. It's hidden right under the "Paste" in the pic below, right above "OK"
You can "see" them using Show Entities
You can also try Tools > Check > Element Quality and under the Femap tab set the Jacobian at 1. This should pick up the elements that have an internal angle greater than 180. Also check "Make Group with Distorted Elements". You will then be able to propagate an entity selection dialog by that group.
Was the mesh produced by Femap? Are you able to post any picture of region where the failing elements are?
The problem is that the entities come in a table with other information. I have imported the .log file with excel as a space formated list, extracted the entities numbers only, and pasted it in as you suggested...but this workflow is nearly as painful as just manually typing in the list manually.
Sorry, my original post was a bit misleading. What you are suggesting works great for finding meshing errors prior to running the solver, but the issue I am now having is finding the elements that are causing the solver to fail after it runs.
For example, the log file generated by the NX Nastran is spitting out 108 warnings, with a list of elements numbers as part of the those warnings. If possible, I would like a way to see those elements that is not quite so manual.
I think you're close...
Take one element that is causing a run issue and do a "Distorted Element Check" on it. You'll get a readout:
Don't Pay attention to the # Failed, but the Values
Use those values and edit the values in the Element Check in FEMAP (Ref any of T_Giampietro's pics).
I think what's happening is the Element Check in FEMAP is different that the values in the Analysis:
You can see that you can bypass the check within the analysis, but I'd confirm you're good in FEMAP first.
That should give you the list in FEMAP and allow you to group/layer, etc. there before the run
...In other words, some of the Analysis checks are set to fatal and the threshold values are different than the FEMAP element check...thus they're not being picked up in FEMAP, giving the impression you're good to go.