Extracting Bolt (Beam) forces for Bolt Calculations
I've created an solved a small assembly with bolted connections, with its contacting face 'separated' for the bolt calculation.
Question: How can I extract bolt forces (Axial, Y-shear, Z-shear) for entry into the spreadsheet.
Comment: When using the Property feature to create Beam properties, the Calculate function computes the four entries with minus (-) sign, which had to be manually edited to (+) sign for Optistruct to solve. I had simply entered the value for R2, but not R1. (SimLab 2017)
Find more posts tagged with
Altair EmployeeHi,
Inserting these text can be done directly in SimLab Itself. Go to LBC browser > Loads and Constraints > Right click > Text Data. All unsupported cards of SimLab can be added here and it will get exported in deck in corresponding field.
<?xml version="1.0" encoding="UTF-8"?>
Yes, after I inquired locally and hwsupport for the best process to extract was via the GUI. Rather painful. Now nearly automated via Optistruct fem input.
With regard to Simlab SET definition, I was surprised one could drag-select a half dozen or so entiities -- EXCEPT for BAR elements. Why not? Just display BAR elements, and drag-select the group when definiing a SET (to be exported into the fem input file)
Ditto for summary of applied forces and reaction forces, just add input/output text
OLOAD
SPCFORCE
and in Hypermesh there is a checkbox for OLOAD and SPCF, which would likely have same result.
Can Altair respond to why BAR elements cannot be graphically drag-box selected to define a SET? And add to Bulk Data. Then the user only needs Case Control: ELFORCE(OPT)=[set-id]
Please add to the set of entites to define a SET, Simlab 2020 is not too late. More useful that defining RBE2's to a SET.
Altair Employeehi,
Hope you are trying to pick bar element after opening set dialog. It wont work, Since SimLab not support to assign SETs for Bar elements or bodies. Please let us know the use case and priority of this request, based on that will support to add set for bar elements.
Also, SimLab already has support to select the bar bodies or bar elements in rectangular selection / drag box selection. Please refer the attached video.
Thanks & Regards
KamalRaj
Senior Application Engineer – SimLab
Altair | Nasdaq: ALTR
kamalraj.rajagopal@altair.com | altair.com
Connect with us: LinkedIn | Twitter | Facebook
For some reason, even with BAR filter, the selection of individual elements did not always work. Sometimes. And did not work for drag-box selection ever. Must be a screen graphic issue.
Rather than extracting element bolt forces (BAR) for x, y, z via the Simlab results display, or Hyperview display, a more efficient method is to simply ASK FOR IT in Simlab. Output is written to the *.force file.
Insert a text file for Input/Ouput
ELFORCE(OPTI) = 900, where 900 is desired SET ID
Insert a text file for bulk data
SET 900 ELEMENT LIST
+ 199036 199038 199040 199042 199044 199046
+ etc
*.force output file:
ITER 0 1 1 6 LOAD: 8 (LOAD) Load 20 000 lb BAR #-END AXIAL SHEAR-1 SHEAR-2 TORQUE BENDING-1 BENDING-2 199036-A -7.3239E+04 -6.3574E+04 2.0407E+04 2.0429E+05 -1.6279E+06 2.3561E+05 199036-B -7.3239E+04 -6.3574E+04 2.0407E+04 2.0429E+05 2.5625E+06 -1.1095E+06 199038-A -1.2324E+04 -4.9177E+04 2.5647E+04 3.5277E+05 -1.6517E+06 2.9854E+05 199038-B -1.2324E+04 -4.9177E+04 2.5647E+04 3.5277E+05 1.7521E+06 -1.4766E+06 199040-A 2.3169E+04 -3.6805E+03 5.7895E+03 5.0671E+05 -1.8987E+05 8.1687E+04 199040-B 2.3169E+04 -3.6805E+03 5.7895E+03 5.0671E+05 4.4348E+05 -9.1460E+05 etc.