Hello,
Is it possible to conduct a purely mechanical simulation by considering the expansion value and assuming a delta T (change in temperature) of 1? If so, how can I express these conditions in an input file to ensure a purely mechanical simulation?
Thanks in advance
Yes, you can use *TEMPERATURE for that - it applies a temperature field in a mechanical (*STATIC) simulation.
I have written conditions for purely mechanical simulation like below
** Nodes
*Node, NSET=Nall
1,0,0,0
2,5,0,0
3,10,0,0
4,0,5,0
5,5,5,0
6,10,5,0
7,0,10,0
8,5,10,0
9,10,10,0
10,0,0,5
11,5,0,5
12,10,0,5
13,0,5,5
14,5,5,5
15,10,5,5
16,0,10,5
17,5,10,5
18,10,10,5
19,0,0,10
20,5,0,10
21,10,0,10
22,0,5,10
23,5,5,10
24,10,5,10
25,0,10,10
26,5,10,10
27,10,10,10
*Element, type=C3D8, elset=Set-all
1,1,2,5,4,10,11,14,13
2,2,3,6,5,11,12,15,14
3,4,5,8,7,13,14,17,16
4,5,6,9,8,14,15,18,17
5,10,11,14,13,19,20,23,22
6,11,12,15,14,20,21,24,23
7,13,14,17,16,22,23,26,25
8,14,15,18,17,23,24,27,26
*Nset, nset=Set-Ground
1,2,3,4,5,6,7,8,9
*Nset, nset=Part-1
1,2,5,4,10,11,14,13,
2,3,6,5,11,12,15,14,
4,5,8,7,13,14,17,16,
5,6,9,8,14,15,18,17
*Nset, nset=Part-2
10,11,14,13,19,20,23,22,
11,12,15,14,20,21,24,23,
13,14,17,16,22,23,26,25,
14,15,18,17,23,24,27,26
*Elset, elset=Part-1
1,2,3,4
*Elset, elset=Part-2
5,6,7,8
** FreeCAD material name: Steel-Generic
** MaterialSolid
*MATERIAL, NAME=MaterialSolid
*ELASTIC
200000,0.3
*EXPANSION
-0.0027531, -0.0012346, -0.0114969
*Initial conditions, Type=Temperature
NALL, 20.00
*Solid Section, elset=Set-all, material=MaterialSolid
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*TEMPERATURE
Part-1, 21.00
** Outputs → frd file
*NODE FILE
U
*EL FILE
S, E, PEEQ
** outputs → dat file
** reaction forces for Constraint fixed
*NODE PRINT, NSET=ConstraintFixed, TOTALS=ONLY
RF
*END STEP
**----------------------------------------------------
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*TEMPERATURE
Part-2, 21.00
** Outputs → frd file
*NODE FILE
U
*EL FILE
S, E, PEEQ
** outputs → dat file
** reaction forces for Constraint fixed
*NODE PRINT, NSET=ConstraintFixed, TOTALS=ONLY
RF
*END STEP
Is this is correct ? your suggestion on this really helpful for me
*TEMPERATURE must be applied to all nodes in the model (not necessarily the same value). So you should add it for Part-2 as well.
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*Initial conditions, Type=Temperature
NALL, 20.00
*TEMPERATURE
Part-1, 21.00
*END STEP
**----------------------------------------------------
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*Initial conditions, Type=Temperature
NALL, 20.00
*TEMPERATURE
Part-2, 21.00
*END STEP
Now, Is this correct?
No, because CalculiX requires *TEMPERATURE for all nodes (both parts) in the first step. Also, no need for initial conditions within the steps.
In the provided INP file, I am executing a layer-by-layer simulation(2 layer Simulation) to obtain results for each layer individually. for this, I have organized the analysis into two steps. The first step for the first layer (part), while the second step is for the second layer (part). Is this approach is not correct for doing layer by layer simulation
You can use multiple steps this way but you have to define some temperature for the remaining nodes (of the second part/layer) in the first step. It can be the same as the initial and zero thermal strain (*TEMPERATURE, ZERO=...) temperature so that there are no stresses in that part during the first step.
For example:
** Nodes
*Node, NSET=Nall
1,0,0,0
2,5,0,0
3,10,0,0
4,0,5,0
5,5,5,0
6,10,5,0
7,0,10,0
8,5,10,0
9,10,10,0
10,0,0,5
11,5,0,5
12,10,0,5
13,0,5,5
14,5,5,5
15,10,5,5
16,0,10,5
17,5,10,5
18,10,10,5
19,0,0,10
20,5,0,10
21,10,0,10
22,0,5,10
23,5,5,10
24,10,5,10
25,0,10,10
26,5,10,10
27,10,10,10
*Element, type=C3D8, elset=Set-all
1,1,2,5,4,10,11,14,13
2,2,3,6,5,11,12,15,14
3,4,5,8,7,13,14,17,16
4,5,6,9,8,14,15,18,17
5,10,11,14,13,19,20,23,22
6,11,12,15,14,20,21,24,23
7,13,14,17,16,22,23,26,25
8,14,15,18,17,23,24,27,26
*Nset, nset=Set-Ground
1,2,3,4,5,6,7,8,9
*Nset, nset=Part-1
1,2,5,4,10,11,14,13,
2,3,6,5,11,12,15,14,
4,5,8,7,13,14,17,16,
5,6,9,8,14,15,18,17
*Nset, nset=Part-2
10,11,14,13,19,20,23,22,
11,12,15,14,20,21,24,23,
13,14,17,16,22,23,26,25,
14,15,18,17,23,24,27,26
*Elset, elset=Part-1
1,2,3,4
*Elset, elset=Part-2
5,6,7,8
** FreeCAD material name: Steel-Generic
** MaterialSolid
*MATERIAL, NAME=MaterialSolid
*ELASTIC
200000,0.3
*EXPANSION, ZERO=20
-0.0027531, -0.0012346, -0.0114969
*Initial conditions, Type=Temperature
NALL, 20.00
*Solid Section, elset=Set-all, material=MaterialSolid
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*TEMPERATURE
Part-1, 21.00
Part-2, 20.00
*NODE FILE
U,NT
*EL FILE
S,E
*END STEP
**----------------------------------------------------
*STEP, NLGEOM
*STATIC
*BOUNDARY
Set-Ground, 1
Set-Ground, 2
Set-Ground, 3
*TEMPERATURE
Part-2, 21.00
*NODE FILE
U,NT
*EL FILE
S,E
*END STEP
Thank you for the reply.