hexagon logo
Register Sign in
  • State Not Answered
  • Replies 27 replies
  • Subscribers 3 subscribers
  • Views 282 views
  • Users 0 members are here
Options
Related

Modeling of Bolts

ron.kunz
Dear all,
I have a big assembly and want to model bolts in the complete assembly. What is the best and accurate way to model this.
Cbar analysis is accurate enough to analyse the bolt forces. Boltstress is of secundair interest.
Are there examples for these bolts?
In addition bar orientation for this CBAR property, how can this best be modeled?
 
Thanks in advance
  • 0
    Ron, I can import my example file into Patran 2017, so the problem has something to do with your installation. I suggest you contact MSC Support, and log a support request.
     
    As I said in another topic/question, You can use Contact Bodies in SOL 101; they are NOT limited to SOL400 (for MSC Nastran 2010++). (We call it "Linear Contact".)
  • 0
    Thanks Ken
    MSC support has helped me with the issue I had. I couldn`t load BDF-files.
    When I open your file then I see several subcases.
    When I have the same bolts I can imagine I can use the same subcases but when I have different size of bolts then I have to specify for each bolt seperate subcases?
    Thanks.
  • 0
    The number of Subcases is NOT related to the number of bolts.
    You need a BOLT entry for each "bolt" you want to preload.
    Enter your preload as a FORCE on GRIDC (control node) of each BOLT. Each force can be a different magnitude (like any force input). Your Subcase LOAD= needs to point to all the FORCE cards.
     
    Assuming you want to "lock" the bolt, you need to use a displacement at the control node. With SOL 101, this takes 2 steps:
    1) In the first run, the preload is defined with forces at the control grids.
    2) In the second run, the preload is defined with displacements at the control grids (using displacements from #1 above).
    So, my example (with 4 subcases), isn't something you can do in the real world (because you don't know the displacement for subcases 2 and 4 until you have the results from subcase 1). I put them together to keep things simple.
    In the real world you might use this process:
    Job 1/SC1: preload forces to get control node displacements
    Job 2/SC2: preload displacements (optional - as a check on preload forces)
    Job 3/SC3: pressure only, gives load distribution without preload (optional)
    Job 4/SC4: pressure + preload displacements
     
    Once you're confident in creating preloaded bolts, you only need to run Job1/SC1 and Job4/SC4.
     
     
     
     
     
     
  • 0
    Dear all,
    can someone have a look at my bdf attached to this message?
    This is part of my big assembly. I have decided to leave boltpretension out of the model and try to model it as I did before in Hypermesh/Nastran combination, which means a conservative approach for bolts. A spider for the hole which is connected by a bar.
    Before I have checked the contact setting, before I had a glued contact and no bolts.
    This model worked.
    Now I have added the bolts and change the contact setting from Glued to Touching.
    But somehow this does not work. I think the bolt is somehow not modelled correctly because the analysis run does not converge.
    If this method is working I can have a go ath the big assembly so please let me know what I should change.
    Thanks.
  • 0
    Ok it seemed I forgot to attach the group for the bars in the selection for the analysis...
    Attached I have the model which runs. Added I have a Force to check the touching condition. The results seems reasonable.
    Now I would like to know if the approach for the bolt is also correct.
    If I want to read the axial force this is the component yy? And for the shear one can take the resultant for xx and zz?
    Is this the right approach?
    Thanks.
    Attached Files (1)
  • 0
    Your bolts look fine, although note that one of your RBEs is not centred in its hole, so the bolt there doesn't run between hole centres.
     
    For the bolt forces, you should request element force output (this is not present in the mode attached above). You should then see "Bar Forces, Translational" in your results in Patran. The output is in the element coordinate system, so axial force is the XX component, and the shears are YY and ZZ. You can compare the plots with the f06 output if you want to check this:
    ScreenShot2098
    ScreenShot2097
© 2025 Hexagon AB and/or its subsidiaries. Privacy Policy | Cloud Services Agreement