EXTRACT NODAL FORCES FROM ENTITY

[darrenlovesmusic]

Hi,

Is there a way to directly extract nodal forces from an entity (blue line) as listed below? I'm assuming that NASTRAN can only extract elemental values. Is this true?  

Thank you. 

[John_Holtz · Accepted solution]

Hi @darrenlovesmusic 

There is a result named Internal Forces that is given at the nodes, but Inventor will not display those results. (It does show another result named internal forces, but that is the sum of internal forces which is almost always zero.)

You could use FNO Reader to extract these forces:

[85020] NODE 3 T1 INTERNAL FORCE

[85021] NODE 3 T2 INTERNAL FORCE

[85022] NODE 3 T3 INTERNAL FORCE

[85023] NODE 3 R1 INTERNAL MOMENT

[85024] NODE 3 R2 INTERNAL MOMENT

[85025] NODE 3 R3 INTERNAL MOMENT

• You need to know the node numbers that you want to extract from the results. In your type of model, I would put the bracket plate with the force on a different idealization. Then you can get the node numbers where you want to get the internal forces based on the PID (the PSHELL ID) of the shell CQUAD elements and the coordinates. That is, you know the nodes of interest are at X Y or Z = some value and are on the elements assigned to Idealization PID.
• The FNO file only has results at the corner nodes. Therefore, you need to use a Linear mesh. You cannot use a parabolic mesh because the results are not given at the midside nodes.

[darrenlovesmusic]

Thank you @John_Holtz 

I want to extract forces to size welds. I think the linear mesh approach will work for me, albeit, I'll need an additional analysis 

[darrenlovesmusic]

@John_Holtz 

I'm thoroughly confused with the FNO results. From what I understand, the FNO reader is giving me interpolated values of centroidal elemental forces at the nodes? What is the orientation of the NODE with respect to the coordinate system?? For example, in the image below, I need the nodal forces at the toe of the weld, but NASTRAN provides all four nodes. How can I identify only the relevant nodal values?  

[g.ceruti · Accepted solution]

hi @darrenlovesmusic ,

try with these Case Control commands (or a combinations of them):

• GPFORCE https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2019/ENU/NSTRN-Reference/files...
• SURFACE https://knowledge.autodesk.com/it/search-result/caas/CloudHelp/cloudhelp/2019/ITA/NSTRN-Reference/fi...
• ELFORCE https://knowledge.autodesk.com/it/search-result/caas/CloudHelp/cloudhelp/2019/ITA/NSTRN-Reference/fi...

to limit the output size,  use previously defined SET on each command

• SET   https://knowledge.autodesk.com/support/inventor-nastran/learn-explore/caas/CloudHelp/cloudhelp/2022/...

if you want, you can get an output on a text file, instead of a binary FNO file.

you have to select the PRINT option in the output requests.

edit the *nas file, change the output option, run the analysis:

ELFORCE(PLOT,CORNER) =ALL ==> ELFORCE(PRINT,CORNER)= "element set number"

GPFORCE(PLOT) = ALL  ==> GPFORCE(PRINT) = "node set number"

and so on

[darrenlovesmusic]

@g.ceruti , another query - Nastran Inventor/FNO reader has no way to view values of stress at Gauss points within the element? am I right here? All I can get is Nodal" (averaged), "Elemental" with/without averaging at either the corners or the centroid. 

[g.ceruti]

Hi @darrenlovesmusic,

Sorry, but I never used the FNO reader, and I can't guaratee what is written in the FNO file, maybe @John_Holtz may help you.

for sure, the rule for nastran output results are:

• DISPLACEMENTs and FORCEs are typcal nodal results, and are computed at nodes
• ELSTRESS, ELSTRAIN, ELFORCE (note that ELFORCEs are force for unit length) are typcal element results, but you can request in the text output (PRINT option), also at element nodes (CORNER option) or at element Gauss points (GAUSS option). However, element results with CORNER option are not avaraged quantity at node, they are the element contribution to each element corner nodes.