Is there a way to get the forces in a bolt? I know SolidWorks simulation it will give you a readout but I’m not finding something like that for PrePoMax. I’m surprised since bolted assemblies are such a common occurrence in design. is there a straight forward way to get forces? It doesn’t even have to be for a solid bolt but just getting anything would be nice. I’ve tried creating RBE with an RP and getting the RF values but that only works if the nodes themselves are constrained which isn’t always ideal. I’ve read all over the forum and YouTube but still not finding anything concrete. Is there not a quick and dirty workflow I could use that will work for most cases? Particularly I have 2 bolts in an out of plane shear that I’m trying to get forces for.
With a solid bolt, you can use the custom *SECTION PRINT keyword as shown here: https://youtu.be/ZSDf1bNXo8g?si=-_dmrdIWIEsSG93N&t=505
When it comes to simplified bolted joint models, it depends on the approach. You can find some tips in this thread and other mentioned there: Best way to find force in bolted connection
Okay thank you for the links. I did the section print and only the preload force is showing, not the external load as well. Do the bolts need to be part of the boundary condition in order to “see” some of the reaction force? I see in my results the Von mises stress on the bolts, is there a way I can total that up? Or can I somehow get the external load to show up on that section print?
Section print calculates forces by integrating stresses so it doesn’t need BCs and should be what you want to get. In your analysis, do you have two steps (preload and external load) and freeze the preload in the second step ?
Yes I followed the steps in your video exactly for my model. I’ve been playing around with different forces and see the numbers changing but not anything significant. For testing I put a 1lb preload on the bolt and then a 4lb shear force on the bolt face and it barely changes not even over 1lb. Idk if it’s wrong or maybe I just don’t understand the results
Do you have hand calculations to verify the results ? You can find some tips and examples in this thread: Pretension shear/tensile resistance - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX). and this one: Bolted Connections - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
If you need further help with that, please share the .pmx file (or at least some screenshots but PrePoMax model would be much better).
Yes I do have some hand calculations. Okay I’ll look through those links.
Here is the link to the file
https://drive.google.com/file/d/1b1pESfn4kPSutbP8ui8sXxWs4r1hOz3Q/view?usp=sharing
The model looks good (apart from some overconstraints in ties but CalculiX ignores them - I just had to resolve them to check the model in Abaqus). Section print may provide inaccurate results for coarse meshes (and this one is rather coarse) since it calculates the forces from stresses. There are other ways to check bolts forces such as requesting RF (reaction force) from the pre-tension section node. I got different results this way and also different in Abaqus (using free body cut too). It’s hard to say what levels of force increase to expect but they are rather low indeed. The highest I got was around 0.026. It’s much lower for the other bolt.
Thanks for taking a look. Should I refine the mesh more? Do you think the model is set up correctly? How do you get the reaction forces on just the section?
It’s always a good idea when working with initially coarse mesh. I doubt it will significantly affect those results though.
I haven’t noticed any significant mistakes apart from some overconstraints in ties but if you run a frequency analysis (I think you already did that since some results of this kind were saved in the file) and nothing flies away then it should be ok (but you could try swapping the master/slave surface assignments in the affected tie constraints sharing the same slave surfaces just in case).
You can do it using the Keyword Editor:
*NSET, NSET=pret
507036, 507037
…
*NODE PRINT, NSET=pret
RF
Nodes 507036 and 507037 are the pre-tension section nodes.