To start off with I'm new to FEMAP and have been grinding my way through tutorials and examples for the past 3 weeks. I've been slowly getting the hang of it, although coming from using Abaqus for 6 years there are some big changes between the software’s. I've done a few API Stress Linearization’s dealing with simple pressure containing parts without any hiccups but now i'm attempting to run a bolted assembly with preload. On a side note I attempted to post this last night and thought it went through but it seems the topic didn’t get posted...so if there's a double post that’s the reason why. Back to the issue at hand, I whipped up this quick assembly to test my contact/glue/preload skills out and obviously they are not up to par. I think I’m getting convergence issues according to the one fatal error.
Step 1: Preload bolts with 51000lbf
Step 2 (not created yet) : Apply moment directly to short pipe end
1: It seems I cannot get the model to converge
1: Two pipes welded to plates
2: An all thread bolt with four nuts per bolt, which are preloaded to crimp onto the plate.
1: Is my approach of gluing the head of the bolt and contacting the underside (nut side) kosher? I was trying to keep the number of contacts down.
2: Any general comments about my approach to this model are greatly appreciated as I’m still getting used to transitioning from Abaqus.
3: General question on applying a "Force" to an Area (not pressure selection). Does it apply the magnitude to each area or does it divide up the force between the areas to act as an average pressure across all selected areas? I'm usually a traction force (pressure across vector) kind of guy myself since i don’t trust typing in Forces over an area.
See the attached file for my attempt. Thanks for any help!
It looks like you need to add contact between the shaft of the bolts and the slots on the top and bottom plates as shown below.
I also recommend reducing the value of the Max Search Distance for the Contact Property. This can reduce the solution time.
That 9137 error indicates the model is underconstrained. I'll take a look at the model you originally attached and see if I diagnose the issue.
I found multiple duplicate nodes inside of your bolts and was not able to successful merge them, so I recommend that you delete those meshes and remesh the bolts. This also means you will need to edit the Bolt Connection Regions to use the new mesh. To do this, edit the Bolt Regions and remove any assigned nodes, then mesh the Bolts, and assign the correct nodes to the Bolt Regions.
In any case, I rebuilt a 1/4 section of your model and was able to solve with both glued and contact. That model is attached. I did not that you have a very high bolt preload (51,000 lbs), so the stresses on the model using Contact properties are very high.
Thank you for the help! What method would you use to ensure no duplicate notes were formed during the meshing process? Still figuring out the nuances of FEMAP. Would you say that model constraints/loads are to be done prior to meshing, in which the meshing would be your very last step? I'll take a look at the file you sent over and see your approach. Once again thank you for your help.
For geometry constraints and loads, it makes no difference in the order you apply them, before or after meshing. The only recommendation I can give you is to check where the constraints and/or loads are applied if you make geometry modifications.
If you mesh multiple solid bodies, even if it's a single operation, you need to merge the coincident nodes after meshing. I did merge the nodes, but the elements seemed to disappear as I think I had an issue on my end with my preference for Geometry scale factor conflicting with your model's Geometry Scale Factor.