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?

A force `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 `ELSE`

.)

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 `k·x`

.