I am new in to non-linear analysis and have gone through the basic math of non-linear FEA.
Based on my understanding, in SOL 106, the user defines how many steps the load needs to be divided into and then further defining how many iterations are allowed for convergence for each load step. I understand the above.
However in advanced non-linear SOL 601, the time steps options are definied slightly different and I have a question regarding the same. I am just copying an image posted by user Blas_Molero in another thread for referencing my question (please ignore the beautifully highlighted red rectangle).
In Time Steps, there are two entry fields. "Number of Steps" & "Time Increment". I am a little confused about the "Time Increment" option. Doesn't Number of Steps define the time increment? Lets say the total load is 1 and if we define 10 steps, then the load is incremented by 0.1 when it starts from 0 (if my understanding is correct). Doesn't "Time Increment" become redundant?
I would like to understand more please. Would appreciate any responses.
Time Step in Advanced Nonlinear (SOL601) in nonlinear static analysis is often used to apply
incremental loads to help solution convergence. Please note that in a nonlinear static analysis (SOL601) with no time-dependent effects such as creep, time is just a dummy variable used for load variation.
For instance, the following problem is an equivalent analysis (without creep), although time step size is different !!. You make your numbers: for advanced nonlinear analysis (SOL601) you need to define the Time Curve explicitly, and then in the NXSTRAT card you enter the TOTAL TIME value of the analysis using Number of Steps and Time Increment values, ie, Total Time = No. Steps x Time_Increment. Is the same, other FEA codes use Starting Time, Final Time & Time Step Size (i.e., Time Increment) and the solver computes the number of steps, here runs the other way.
In general for nonlinear static analysis (without creep) with SOL601 I always use TotalTime = 1, then No. Steps = 25, and Time Increment = 1/25, easy, don't you?.
Please note that later you can activate ATS (AUTOMATIC TIME STEPPING) and surely the number of steps won't be 25, the solver will achieve convergence in less steps, then the SOL601 (ADINA) way of defining solution put emphasis in the time step size for the starting analysis, that is very important
Thanks for replying and for the explanation.
I just want to make sure I have grasped the concept of how time works in Sol 601. Let me try to explain my understanding with an example & hopefully you can clear the misconceptions I may have.
Lets say we have a cantilever beam with a transverse tip load of 10,000 lbs.
In SOL 106, I choose 100 of load steps and 100 iterations in each step. So each 'delta t' = 100. The solver will start from 0 then 100, 200 and so on until it reaches 10,000 lbs. Am I correct so far?
If I choose to run the same problem in SOL 601 and choose number of time steps to be 20 and time increment to be 0.05, then the Total Time = 20 x 0.05 = 1.
What this means is that the difference between load amounts = 10000/20 = 500. So the load will start with 0, 500, 1000 and so on until it reaches 10,000 lbs.
Is my interpretation correct?
Thanks & regards,
In NX NASTRAN BASIC Nonlinear Analysis (SOL106) if you define 100 Increments of Time steps then the solver will divide the solution in minimum 100 steps (please note that not any load vs. time curve function is required to define in FEMAP, the NX NASTRAN solver always use a dummy time of 1.0).
By the way, I suggest to use a reasonable value of Maximum Iterations/step = 25, the value proposed of 100 is quite largue, if the solution do not conveerge in 25 iterations per step is better the solver to stop and investigate the problem, to not wait till 100 iterations.
If you want to learn how to setup a nonlinear analysis using SOL106 take a look to my website in the following address:
Also, under FEMAP EXAMPLE Problems take a look to examples 25 till 29 (in FEMAP go to HELP > EXAMPLES). For Advanced Nonlinear (SOL601) take a look to examples 30 & 31.
To run the same problem in Advanced Nonlinear (SOL601) you first need to define in FEMAP a function vs. Time curve and associate this curve to the load. This is a dummy time because you run a nonlinear static analysis, not transient, this is a simply method to increment the load. For instance, a ramp function between (0,0) and (1,1) is quite typical. You can use any time, for instance (0,0) and (100,1). The important message is that at time =100 the load will have 100% value, ie, 10e3 Lbs.
Next, in NXSTRAT you need to define the time stepping:
• If you want to use 20 steps using the time curve (0,0) till (100,1) then you need to enter:
• If you want to use 20 steps using the time curve (0,0) till (1,1) then you need to enter:
Thanks a lot for the explanation, especially on how the ramp function works in FEMAP and accordingly the Time increment inputs in NXSTRAT.
I apprecaite it a lot.
I was performing a few test cases to get a better understanding in usage of gap elements as contact (especially in heel to toe contact situaton) using SOL 106.
I am having trouble interpretting a SOL 106 analysis. I was hoping you can help me based on your experience.
I have created a simple L-Joint with heel-toe contact feature using 1D gap element.
Here is a screen shot of my NLPARAM (non-linear control option) card entry in FEMAP.
Please ignore the high number of load increments. I had issues with convergence with lower load increments and with AUTO stiffness method option.
Anyways, when I look at the output set window, I see 33 steps (not 25) before the final load value was achieved. Again my understanding is that, the load increments should have started from 0.04, 0.08, .12 etc...but the first load set is 0.0025 and it increments by .0025 for another few steps and then changes again before finally incrementing the factor which was entered (Load Case 10 onwards).
Would appreciate your help.
Thanks in advance,
Thanks so much sir for clarifying.
A couple of more questions.
Any basis on why you are recommending ITER update for stiffness matrix instead of SEMI?
Also, any FEMAP resources to which you can point to, where I can learn more on some of the finer things about each solutions strategy? Like I am aware of the general overview of Newton Ralphson, modified newton-raplphson (not understood how arc or line methods works yet ) but I was not aware that Newton Ralphson method does auto time step if convergence is not achieved.
Appreciate your help & prompt responses immesnly. Truly you are helping in making the learning cuve a lot more easier.
In FEMAP go to HELP > NX NASTRAN and you will open the NX NASTRAN Manuals, this is the best source of documentation to learn anything about NX NASTRAN, the FEA code you run: everything is there!!. Go to the BASIC NONLINEAR ANALYSIS USER´S GUIDE (SOL106,129), there you can learn how to control iterations using the NLPARM entry.
Stiffness matrix update strategies are determined by a combination of the data specified in the two fields KMETHOD and KSTEP. Options for KMETHOD = AUTO, SEMI, or ITER. The KSTEP field, which is an auxiliary to the KMETHOD field, should have a value => 1.