I am fairly new to using SOL 601 Advanced Nonlinear Static Analysis. I am having convergence problems with the my 3D Lap Joint model.
The goal of this model is to determine the load distribution among multiple fasteners in a lap joint that has a tensile applied load as well as bolt preload.
I have modeled in FEMAP a single lap joint with one fastener, all with parabolic brick elements with midside nodes (with the exception of some wedge elements at the center of the bolt). All mesh are matching. I will eventually have the model with four fasteners. The plates and fastener are made of steel. The bolt head, nut, and bolt shaft are modeled as one piece.
Pre/Post Processor: FEMAP 11.1.2.
Solver: NX Nastran (packaged with FEMAP)
I have created contact between the two plates as well as the bolt and plate interface by creating regions based on element face and creating appropriate Connectors. I did not model friction. The connection properties are set to default.
-Pinned constraint at one end of the plate
-T3 Constraint (vertical) at the other end of the plate where the tensile load is applied.
-T2 Constraint (along with width of plate) at the center line of the two plates because the net displacement in the 2 Direction from Poisson's effect is zero.
-250,000 psi pressure at the end of the plate. This equals 10,000 lb. I have created a linear ramp function and applied it to the pressure to increment the load because I would like to see the change in fastener distribution as the load increases.
-2006 lb bolt preload. I created the bolt preload region at the center row elements of the bolt shank and used the global Z direction for the axial axis (this is fine since I have the bolt modeled at (0,0,0)
NXSTATParameters : I have followed the guidelines from the following posts.
The bolt preload portion seems to work great, but after a few hours of running the bdf through the solver, the model will stop converging at Time Step 56 , which based on my time step setup, this is 56% of the 10,000 lb tension load. I have tried changing auto increment from Total Load, Stabilize to On. I have also tried leaving autoincrement turned off with line search turned on. I have also tried increasing the time step to 200 and reducing the time step to 0.005 as well as using the 3-D Iterative Solver. None these solutions have helped the model converge.
I am also having some issues getting NX Nastran to generate the .res file so I do not have to run the entire analysis all over again when it does not converge. In the NASTRAN Executive and Solution Options menu, I have checkboxed Save Databases for Restart. In the NXSTRAT Solver Parameters menu, I have used Normal for the Restart Options. After NX Nastran finishes solving, no .res is anywhere to be found.
Does anyone have any suggestions on getting the model to converge? I know that increasing the Time steps and reducing the time increments and using auto increment should help, but I have not made any progress with these solutions. Also, can anyone explain more in detail how I can get the Restart feature to work?
I have included the bdf for the model
Solved! Go to Solution.
Is the analysis reaching the number of allowed cut-back?
What is the constraint on the bolt?
I'm not quite sure what you mean by "cut back," but the Auto Time Stepping, ATS, is running through up until the maximum number of subdivisions without convergence has been reached.
I did not constrain the bolt. The only constraints I have are for the plates.
I made a few changes to the model. I realized that because the geometry of the bolt and the applied load is symmetric, a T2 constraint may be applied to the nodes on the bolt cut by the XZ plane. I also changed the convergence criteria from Energy and Displacement to Energy.
I set up a few models with different NXStrat Parameters. I decided to start out with smaller time steps and here's what I found so far. All have a total time of 1. (Number of Steps X Time Increments = Total Time). The final load is 10,000 lb.
Number of Steps = 10, Time Increment = 0.1, Bolt Force Increments = 10, ATS = Off
Completed 90% of 10,000 lb and then stopped
Number of Steps = 25, Time Increment = 0.04, Bolt Force Increments = 25, ATS = 1...On
Completed 89.4% of 10,000 lb and then stopped
So far, it's reaching convergence better with those changes, but not fully converging. Although I loosened the convergence tolerance, I don't believe it would significantly affect the load in the fastener which I am fine with.
Do you know of a way that I can set up X time steps and increments from Time =0 to 0.9 then set up Y time steps and increments from Time = 0.9 to 1? I would prefer to avoid Auto Time Stepping if I can since I would like to have results where the increment load is constant . This is just to make it easier to compare with models with different fastener setups.
"cut back" = subdivisions and if I understood your note then SOL601 is reaching the maximum number of allowed sub-division without convergence
Without constraint on the bolt how do you stop it spinning on its axis? I guess now with your T2 constraint as per your update
I am assumig you know what your doing by changing the convergence criteria! I was told/advice a long time ago to "...never change convergence criteria unless you know what your doing". As most of the ime I do not (!) I dont' touch these. Usually, at least for the "old" MSC.SNastan sol601, convergnce criteria default values were tested over a wide range of nonlinear problem to give the "best guess" choice.
Looking at run 2, the analysis clearly goes all the way to 68% of the load (17*0.040) without any problem then does the 1st sub-division at step 18 (2 cut back actually to get convergence in step #18). Might be worth checking what is happening (contact, deformation, etc)
you get a better convergence because you loosed the convergnce criteria. One should not loosen convergnce criteria and change other things (nb of steps for example) otherwise you do not know what is effective (changing to many things at once!)
to have a constant load step you may need a very small one. The whole point of the "auto stepping" is that it "decide by itself" (ABAQUS can even increased the load step if could convergence is obtained) what is needed. Just needs to point it in the right direction
Create two steps
Step 1: 0.68*10,000 = 6800 (nb of load increments ~15, 18 should do !)
Step 2: 10,000
Thanks for the feedback so far.
I actually am using the default convergence criteria in SOL 601, which is just set as Energy.
I may have found out what is causing the convergence issue. Take a look at the picture below.
This is a side view of the lap joint. The purple elements are the bolt head and nut, the red is the top plate, and the blue is the bottom plate. You are seeing the total ACTUAL displacement at 9000 lb of load from the 10 Time Steps, 0.1 Increments, Auto Off model.
You can see that the top plate is penetrating into the bottom plate. I measured about 0.1 inch of penetration in the Z direction. I have seen in the results that at lower load, the penetration is very small. As the load increases, the amount of penetration becomes greater. This may explain the reason for the model to converge at small loads, but struggle with the larger load.
I have also compared this with a Linear Static Analysis that converged as shown below. There is very minimal penetration between the plates.
Then I realized I also had this error in the f06 file, but it still solved
I currently have the contact property set to Default. The contact surface compliance is set to 0. This means that there is no interpenetration allowed. From what I am seeing in f06, the contact surface compliance is not being used for some reason, which is allowing the nodes to penetrate one another. Do you know why this would happen and how I can fix this?
What 's causing that "kink" in the bottom plate?
Have you checked the contact output results?
The messages indicate that your bolt preload converged fine in 10 increments in the first run. No need to set BOLTSTP=25. In fact, there may have not been a need to set it to 10. Did you try the default of 1?
Does the penetration only happen at the edge of the contact region or does it extend across the whole face? If it is only happening on the edge, extendend the target surface may help. Try setting EXTFAC to 0.1 on BCTPARA
Do you have friction defined on the contact regions? Adding friction may help stabilize things as well.
TSTEP continuation lines can be used to control the stepping thorugh the time history. The following would use steps of 0.1 from 0 to 0.9 seconds, then steps of 0.01 from 0.9 to 1.0 seconds:
TSTEP 10 9 0.1 1 + + 10 0.01 1
You can add as many continuation cards as you need, following the same format (number of steps; step size; output frequency).