Hi, I´m doing a simulation where I want to apply bolt preloading in a first (static no lineal) step, and then I want to perform a second dynamic step, where I want to include an initial velocity to some bodies. I know that I can apply velocity with **INITIAL CONDITIONS,TYPE=VELOCITY, but is there a way to apply it in a second step?
Abaqus has an import functionality for that. In CalculiX, it would be more tricky. Maybe you could replace initial velocity with properly scaled gravity load.
Thanks, I need to simulate an impact load from a determinated height in a bolted part, but I want to save time and put the impactor just above the impacted zone and add the final velocity as bc, I thought that it was a direct procedure, but I find out that velocity just can be applied only as an initial condition.
Why not use an equivalent static load?
First, determine the spring constant of your bolted part on the impact point, say with a load of 100 N. From that you can calculate the energy stored in your structure depending on the displacement.
The energy from the impactor is M·g·(h_initial + displacement). At some displacement, the deformation energy will be equal to the spent potential energy from the impactor and the falling mass will stop.
The static load needed to yield the same displacement follows. And then it’s just a simple static calculation.
oh, looks nice!. Seems fast and simple.
Which could be the range of applicability?.
What if you use three steps instead of two?. The second would be introduced just to accelerate with a force the impactor from an initial velocity of 0 m/s to your desired velocity. I would say that’s what Calc_em is sugesting.
If the bolted part is in rest I guess you can use a dynamic explicit step with mass scaling. It can be very fast because there are no contacts and you are not worry about disturbances on the impactor. You just want a mass with certain velocity traveling to the tarjet. I don’t think nobody cares if it carry some Stresses.
The example compares with and without Inital conditions. Final velocity is the same. Just locate the Impactor a few mm before the impact (5mm) to allow space to gain speed.
*NODE 1,0,0,0 2,-0.02,0,0.01 3,0,0.0025,0 4,0,0.0025,0.01 5,-0.0175,0.0025,0.01 6,-0.0175,0.0025,0 7,-0.02,0.0025,0 8,0.0025,0.0025,0 9,0,0,0.01 10,0.0025,0,0 11,0.0025,0,0.01 12,0.0025,0.0025,0.01 13,-0.02,0.0025,0.01 14,-0.0175,0,0 15,-0.0175,0,0.01 16,-0.02,0,0 *ELEMENT,TYPE=C3D8R 1,5,13,7,6,15,2,16,14 2,1,10,8,3,9,11,12,4 *NSET,NSET=Bar 1 3 4 8 9 10 11 12 *ELSET,ELSET=Accelerated__with__Mass_Scaling 1 *ELSET,ELSET=With_Initial_Condition 2 *MATERIAL,NAME=Steel *ELASTIC,TYPE=ISOTROPIC 210000000000,0.3 *DENSITY 7850 *SOLID SECTION,ELSET=Accelerated__with__Mass_Scaling,MATERIAL=Steel *SOLID SECTION,ELSET=With_Initial_Condition,MATERIAL=Steel *INITIAL CONDITIONS,TYPE=VELOCITY BAR,2,10.0 BAR,1,0.0 BAR,3,0.0 *STEP,NLGEOM=YES,INC=100,AMPLITUDE=STEP *DYNAMIC,SOLVER=PARDISO,EXPLICIT 0.0001,0.001,0.001,0.001 *CLOAD 15,2,1.2265625 2,2,1.2265625 16,2,1.2265625 14,2,1.2265625 *NODE FILE,GLOBAL=YES U,V *EL FILE S,NOE,ENER *END STEP
Thanks for the advices!, I try to solving in the force brute way, just modeling the striker part in real position and then adding a first step static with the preloads, and a second dynamic with only gravity acting. I have tested the two steps separately and it works, the preloads acts in the bolts, and the striker impacts with very few penetration on the part.
The problem is when I try to put the two steps in one simulation… I get this error message at the begining of the second step:
STEP 2 *INFO reading *STEP: nonlinear geometric effects are turned on *WARNING reading *DYNAMIC: the initial time increment defined by the user will not be used since the time increment is determined automatically by the dynamic procedure based on stability considerations *INFO reading *DYNAMIC: for implicit calculations the calculation of the internal energy is activated. Dynamic analysis was selected Nonlinear material laws are taken into account Newton-Raphson iterative procedure is active Nonlinear geometric effects are taken into account *ERROR in CalculiX: in nonlinear calculations energy output requests, if any, must be specified in the first step
This is my input file, the two stpes definition only, there is no energy output request, don´t understand why I have such error:
*STEP,NLGEOM=YES,INC=100,AMPLITUDE=STEP *STATIC,DIRECT 0.1,1,0,0 *CLOAD,AMPLITUDE=pretensionsection1 43604,1,1 *CLOAD,AMPLITUDE=pretensionsection2 43605,1,1 *NODE FILE,GLOBAL=YES U *EL FILE S,NOE *END STEP *STEP,NLGEOM=YES,INC=100000000,AMPLITUDE=STEP *DYNAMIC 1E-05,1,1E-09,0.01 *DLOAD EL_ALL,GRAV,0,1,0,0 *DLOAD EL_ALL,GRAV,-9.8,0,1,0 *DLOAD EL_ALL,GRAV,0,0,0,1 *NODE FILE,GLOBAL=YES U,V *EL FILE S,NOE *END STEP
Trying adding this in the first step:
*EL FILE ENER
It´s working now with that, thanks! I look in the CCX manual the way to add the energy requirement but didn´t find it.
The thing is that CalculiX in implicit dynamics requests the energy balance by default:
For all dynamic calculations (implicit dynamics, explicit dynamics with penalty contact or explicit dynamics with massless contact) a energy balance can be requested. For implicit dynamics this is done by default, for explicit dynamics the balance is calculated if the user has requested the output variable ENER underneath a *EL PRINT, *EL FILE or *ELEMENT OUTPUT keyword.
And if it’s requested, it must be requested from the first step:
The keys ENER and ELSE trigger the calculation of the internal energy. If they are absent no internal energy is calculated. Since in nonlinear calculations the internal energy at any time depends on the accumulated energy at all previous times, the selection of ENER and/or ELSE in nonlinear calculations (geometric or material nonlinearities) must be made in the first step.
@rsmith , how do you compute the stored energy in the structure knowing its stiffness (spring constant)???
The other variable that would be interesting to compute would be the desaceleration of the striker after reaching the part, could it be computed knowing the stiffness?
F acting on a certain point of the structure will generate a displacement
x at that point. For this, it is assumed that response of the structure is linear, i.e.
F(x) = k·x, where is
k the spring constant.
You can determine
k using CalculiX by applying a point load on the impact point of your structure and then extract the displacement on that point from the FEA solution.
The work done by the elastic deformation is
Ed = ∫F(x)·dx = k·∫x·dx = k/2·x²
(You can also get this from CalculiX using
EL PRINT with
The falling mass converts potential energy into kinetic energy. The amount of this energy is
Em = M·g·(h₀+x), where
h₀ is the falling height before the mass hits the structure.
The maximum deformation is reached when all of the potential energy of the falling mass has been converted to elastic deformation. That is,
Ed = Em.
k/2·x² = M·g·x + M·g·h₀ ⇔
k/2·x² - M·g·x - M·g·h₀ = 0.
This is a simple quadraric equation that can be solved for
x. Once you’ve found
x, the equivalent static load is