# Extracting Bolt (Beam) forces for Bolt Calculations

## Recommended Posts

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)

##### Share on other sites

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
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.```

##### Share on other sites

Hi,

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.

##### Share on other sites

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

SPCFORCE

and in Hypermesh there is a checkbox for OLOAD and SPCF, which would likely have same result.

##### Share on other sites

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.

##### Share on other sites

hi,

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

altair.com